NC Express FPL Manual - Finn-Power International, Inc.

Finn-Power International
710 Remington Road
Schaumburg, IL 60173
USA
Tel. +1 800 344 7143
Fax +1 847 885 3200
www.finnpower.com
Finn-Power Oy
P.O. Box 38
FIN-62201 Kauhava
Finland
Tel. + 358 6 428 2111
Fax + 358 6 428 2244
www.finn-power.com
FINN-POWER
Laser
FPL
L6
NC Express♠ v6
User Manual
Edition 1.11.06/GB

This document contains proprietary information and trade
secrets and is not to be distributed, published or copied partially or
fully without prior written authorization by Lillbacka Corporation.
All registered names and trademarks referred to in this
documentation are sole property of their respective owners.
This documentation includes listed items and their operation descriptions, procedures,
and other exclusive information that are proprietary information and/or intellectual
property of Finn-Power Group, protected under international copyright or similar laws
and/or by patents or patents pending. Listed items are defined herein to include, but not
limited to: components, features, modules, methods, software, systems, technology,
options and the like. Further information of said patents and patents pending can be
requested in writing from:
Director of Engineering, Lillbacka Corporation, P.O. Box 38, 62201 Kauhava, Finland.
2

INTRODUCTION 7
1 OVERVIEW 8
2 SETUP OF NC EXPRESS 9
2.1 LOADING MACHINE INTO NC EXPRESS 9
2.2 NETWORKING NC EXPRESS 9
2.3 STARTING NC EXPRESS (ENVIRONMENT) 10
2.4 NCEXPRESS OPTIONS 13
2.5 MATERIAL DATABASE 15
2.5.1 MATERIAL TYPES 15
2.5.2 UPDATING MATERIALS 16
2.5.2.1 Directly from Laserprm (Read Laserprm…) 17
2.5.2.2 Manually enter material 18
3 PART PREPARATION 19
3.1 CAD FEATURES 19
3.1.1 CAD 19
3.1.1.1 Selection 20
3.1.1.2 Snap Modes 20
3.1.1.3 Use of construction lines 23
3.1.1.4 Numerical input (Evaluator) 23
3.1.1.5 Selecting Elements for Using Copy/Move Functions 24
3.1.1.6 CAD Functions 24
3.2 IMPORT DXF FILES 34
3.2.1 IMPORT A GOOD DXF FILE 34
3.2.2 DXF FILES THAT ARE NOT OK 35
3.2.2.1 Duplicate lines 35
3.2.2.2 Duplicate lines (automatically taken out) 36
3.2.2.3 Open contour 37
3.2.3 EXERCISE 38
3.3 CP FILE (PART FILE) 38
3.3.1 CREATE NEW PART 38
3.3.2 STORING CP FILES 40
3.3.2.1 Exercise- Changing Default Part Directory 40
3.3.2.2 Networking Part Directory (Sharing) 41
3.4 PARTS DATABASE 42
3.4.1 ADDING PARTS TO THE DATABASE 42
3.4.1.1 Editing Parts within the Database 43
3.4.1.2 Sorting Part Information within the Database 43
3.4.2 SUPER PART REPORTING (GRID PARTS FEATURE) 44
3

4 TOOLING PARTS 45
4.1 AUTOMATIC (AUTOTOOLING) 45
4.1.1 CAM DATABASE 45
4.1.1.1 Saving Settings to CAM Database 46
4.1.2 SETTINGS 47
4.1.2.1 General tab 47
4.1.2.2 Microjoint tab 48
4.1.2.3 Path/Leads tab 50
4.1.2.4 Lead in – Lead out settings 51
4.1.3 SINGLE PART 58
4.1.4 PRESHEARED PARTS 59
4.1.5 COMMONLINE PARTS 59
4.1.5.1 At part level 59
4.1.5.2 At nesting level 59
4.1.6 EXERCISE- AUTOTOOL PARTS 60
4.1.7 AUTOTOOL EXAMPLE 1- GENERAL 65
4.1.8 AUTOTOOL EXAMPLE 2 – PIERCE POINT 66
4.1.9 AUTOTOOL EXAMPLE 3 - AUTOCYCLING 70
4.2 MANUAL TOOLING 71
4.2.1 TEXT MARKING 71
4.2.2 MANUAL CYCLING 72
4.2.3 DELETE TOOLING 76
4.2.4 TOOLING MODIFY FEATURES 76
4.2.4.1 Piercing Technology 76
4.2.4.2 Process Technology 76
4.2.4.3 Tabs 77
4.2.4.4 Break Laser path 77
4.2.4.5 Leads 77
4.2.4.6 Direction 78
4.2.4.7 Loops 78
4.2.4.8 Fillets 78
5 NESTING 79
5.1 NC EXPRESS NESTING THEORY 79
5.1.1 PLATES DATABASE 80
5.1.2 PARTS DATABASE 81
5.2 CREATING A NEST 81
5.2.1 RUN ID 82
5.2.1.1 Re-using/Overwriting Run Folders (Dynamic Nesting) 82
5.2.1.2 Keeping old Run Folders (Static Nests) 83
5.3 NESTING PARTS 83
5.3.1 GLOBAL PARAMETERS 84
5.3.1.1 Plate Margins 84
5.3.1.2 Nesting Theory Summary 84
5.3.1.3 Part Separation 84
5.3.1.4 Nest Accuracy 85
5.3.1.5 Nest Direction 85
4

5.3.1.6 Grid Nesting 85
5.3.1.7 Nest by Work Order 85
5.3.1.8 Nest in Holes 85
5.3.2 PART LIST 86
5.3.3 PLATE LIST 88
5.4 NESTING EXAMPLE 89
5.5 MODIFYING PART’S/TOOLING (FOR PARTS THAT ARE ALREADY NESTED)
91
5.6 PRESHEARED PLATE NESTING 92
5.7 INTERACTIVE NESTING 92
5.7.1 DRAG AND DROP PARTS 92
5.7.2 COPY PARTS 92
5.7.2.1 Move Selected 93
5.7.3 ADD PART 93
6 OPTIMIZATION 94
6.1 AUTOMATIC LASER OPTIMIZER 94
6.1.1 EXERCISE- OPTIMIZATION 94
6.1.2 EXERCISE- OPTIMIZATION (SCRAP CUTTING AND CROP LINE) 99
6.2 INTERACTIVE OPTIMIZER 102
6.2.1 MODIFY 102
6.2.2 VIEW ONLY 102
6.2.3 EXERCISE- INTERACTIVE OPTIMIZER 103
6.2.3.1 Modify (without Graphic Mode) 103
6.3 BATCH OPTIMIZATION (AUTO-PROCESSING MULTIPLE SHEETS) 106
7 CREATE NC CODE 108
7.1 SIMULATION 108
7.2 NC CODE 108
7.3 REPORTS 111
8 HIGH SPEED – NORMAL CUTTING MODE 112
8.1 HIGH SPEED CUTTING MODE 113
8.1.1 HIGH SPEED CUTTING MODE FOR 0MM – 1.5MM 113
8.1.2 HIGH SPEED CUTTING MODE FOR 1.5MM – 3MM 115
8.2 NORMAL CUTTING MODE 116
8.2.1 NORMAL CUTTING MODE FOR 3.5MM AND HIGHER (AND O2) 116
8.2.2 NORMAL CUTTING MODE FOR 0MM – 3MM 118
9 ORDERS MANAGEMENT SYSTEM (MRP NESTING) 119
9.1 DATABASE ORDERS DIALOG 119
9.2 ADDING/MODIFYING PARTS IN ORDERS DATABASE 121
9.3 EXERCISE- USING ORDERS DATABASE 124
5

10 CREATE PARTS 128
10.1 CREATE PART3 128
10.2 CREATE PART4 129
10.3 CREATE PART5 130
10.4 CREATE PART6 131
11 AUTOTOOL SPECIAL PARTS EXERCISES 132
11.1 COMMONLINE CUTTING AT PART LEVEL 133
11.1.1 COMMONLINE EXAMPLE 1 134
11.1.2 COMMONLINE EXAMPLE 2 135
11.1.3 COMMONLINE EXAMPLE 3 137
11.2 COMMONLINE CUTTING AT NESTING LEVEL 138
11.2.1 COMMONLINE WITH SAME PARTS 138
11.2.2 COMMONLINE WITH DIFFERENT PARTS 144
11.3 PRESHEARED PARTS 146
12 NESTING EXERCICES 148
12.1 NESTING 1 148
12.2 NESTING 2 149
APPENDIX A- AUTOTOOL SETTINGS 150
APPENDIX B- NEST PARAMETERS 156
APPENDIX C- OPTIMIZER SETTINGS 160
APPENDIX D- PARAMETERS NC CODE 162
6

INTRODUCTION
W elcome to NC Express integrated part creation and nesting system. NC
Express is an easy to use Windows-based application. Any computer
running Microsoft® Windows NT 4.0/2000/XP Professional operating systems
can install and use this software*. NC Express follows the conventions of a
contemporary Windows based application. Therefore, any user familiar with
Microsoft® Office Suite or Windows operating systems should already have all
the knowledge necessary to work with this package. Although a working
knowledge of these programs is beneficial it is not a prerequisite to using NC
Express.
*NC Express does not run on Windows 95/98/Me.
NC Express is a scalable application. It may be used as a single part drafting
and tooling program or as a fully automated machine tool management system.
Either way the results will be the same, automatic NC code creation. Users are
easily guided through the process of creating NC code. When first started the
user will notice the ease of use, with the program’s menu-driven system. Each
section of the system is divided throughout the program. What makes NC
Express unique is that the system is driven to form a state of automation. The
NC Express user can import or draw geometry and process it into NC code
without any manual intervention.
NC Express can be divided into five different sections. These five sections will
need to be understood in order to properly prepare NC Code.
Five sections:
• CAD drawing or import DXF
• Tooling
• Nesting
• Optimization
• Creating NC Code
• MRP system (Material Requirements Planning)
7

1 OVERVIEW
NC Express for FPL training course will be covered as follows:
• Setup of NceXpress
o Loading machine
o NceXpress Options
o Material Database
• Part preparation
o CAD system
o Import of DXF files (+ problems)
o Creating a CP file
o Parts Database
• Autotooling
o Microjoints
o Lead-in/lead-out
o Path/Leads
o Manual Intervention (Intertooling)
o Exercises
o Commonline cutting
o Preshear
• Nesting
o Global parameters
o Part/Plate list
o Manual Intervention
• Optimization
o Interactive Optimizer
o Exercises
• Create NC Code
o Reports
• Orders management system
o Order Database
8

2 SETUP OF NC EXPRESS
Setup of NC Express for the FPL machinery is minimal. There is no need to
declare tools within a tool library as well as declaring tooling positions within a
turret. The machine parameters are setup by Finn-Power to declare maximum
and minimum working areas of the machine, as well as clamp settings and other
options of the machine. The machine parameters should need no adjusting by
the customer.
When customer has installed NC Express on desired computer* there is a
directory created C:\fms\ncexpress. Within this directory there is a bin
directory, which holds all pertinent files for NC Express to run. Customer
machine (ex. laser_mm or ‘customer name’) will be stored in the
C:\fms\ncexpress directory. When working in NC Express the parameters set to
create code for specific machinery come from the customer machine folder
within C:\fms\ncexpress.
*NC Express is not supported nor will not run on Windows 98 or Me.
2.1 LOADING MACHINE INTO NC EXPRESS
Make sure the customer machine, given with software, is stored in
C:\fms\ncexpress. Place the dongle on parallel port of computer or USB port.
Open NC Express from either the shortcut on the desktop or go to Start menu
then programs, NC Express. Go to File menu | Open → Machine if machine
name appears on list do not follow the following.
Loading machine: Go to File menu | New → Machine. (Note- if grayed out call
Finn-Power support for password) Type letter for letter name of folder/directory
that was stored in C:\fms\ncexpress directory, then click OK. NC Express will
ask ‘Do you want to add this machine folder to the system’, click OK and
machine is now added.
2.2 NETWORKING NC EXPRESS
NC Express allows only one folder to be networked for the FPL. The Part
directory (taken from C:\fms\ncexpress\(your machine)\Partdir) can be used on
the network and shared amongst more than one user. The Partdir can be copied
to a mapped network drive.
To map through NC Express:
Copy Partdir on a mapped network drive
Go to Settings menu | Machine Parameters |select Environment
Select the second TAB-page : Directories
Next, where Part directory is declared click Browse…
Find Partdir on network, open directory and select a part, and then
click Open.
Note- Machine must remain within hard drive where NC Express resides. The work
directory must also remain within the machine folder. All setting and machine
parameter limitation reside within these folders.
9

2.3 STARTING NC EXPRESS (ENVIRONMENT)
Open NC Express by double clicking NC Express icon on desktop, or by going
to Start menu | Programs then NC Express folder. On first open check the
settings of where the part directory is being defaulted:
Go to Settings menu | Machine Parameters | Environment:
User- On the top right of the Environment dialog User is visible. Entering a
user name here is not a password for the system, but will give the ability to view
who did what within the system.
Material database- This is explained in the description of the material
database. Chapter Material Database.
For each material and thickness there is a HSP type defined and a default cutting
mode.
The HSP type can be :
10

The cutting mode can be :
This is more explained in the chapter about autotooling.
System settings –
Units – is the type of unit we are working in. These can be set to MM or INCH
Tolerance- Is the acceptable distance of open geometry for automatic tooling.
This number is unit dependent. Tolerance is used primarily as a CAD tolerance
during geometry import. It is also used in the Autotool portion of the program
as a tooling tolerance except for the cases where greater tolerance value was
explicitly set in Autotool dialog.
System tolerance could be set in a certain range without affecting system
performance but should always be greater than finest detail in the drawing
(shortest distance between to holes, smallest radius, etc.). Sometimes tolerance
can be increased to correct an error in part drawing but we strongly advice
against it because geometry download program in this case would simply shift
vertices and distort geometry.
Default value for the tolerance (0.0001 inch or .0025 mm) will serve fine for
most applications and seldom has to be changed.
11

On the second TAB-page you can find back all the path settings for the
direcorties :
Part directory- is where the parts will reside. Not only is this the location of
where the parts reside but also the location where each run folder looks for parts
to be nested. To be able to save parts to the correct directory make sure the
correct directory is listed. To select a path the path can be typed in manually or
user can browse to find correct location (cp file must reside in the desired
location in order to select directory). (Note- This directory can be on the
network.)
Note- This directory can be on the network.
Database directory - is the default location of the Database for parts, plates and
orders. This can be shared amongst multiple users.
Note- This directory can be on the network.
Turret directory is the default location of the turret files.
Tool library directory is the default location of the tool library.
Zip Machine Data allows you to quickly zip up the machine setup along with
databases. This allows for quick and easy way to send information on the
current nest that is in question. The current nest listed within the Environment
Run ID window will be zipped up along with the machine setup. This file is
saved within C:\fms\ncexpress as a default.
12

2.4 NCEXPRESS OPTIONS
Options will handle functions within Nesting and Post Processing. To find
options go to Settings menu | select Options.
General
Language- Option to select different language for the software.
Background – here you can select the color of the background
Use split-screen dialog – this allows us to see a drawing of the part
when we open the part database
Autotool
Start Unloading Robot dialog automatically- For machines that have a
robot unloader; the software has the capabilities to place the robot
automatically. In the case that a user will manually place the robot
suction cups for a part this option will toggle on/off the display of the
robot dialog after Autotooling.
Start advanced CAD functionality on system start- If we disable the
option Start advanced CAD functionality on system start then
NCeXpress will start without the Cad system. It is possible to start the
CAD functionality after start up by going to Drawing in the menu bar
and the toolbars will appear on the screen.
13

Report
Generate report PDF file automatically after post-processor-
Automatically create a PDF file of the report, which is saved to the
default location chosen in the Post Processing dialog. You can also select
a default report that should be used as template.
Print report automatically in nest explorer after accepting- When all
sheets within the Nest Explorer are post processed they are ready to be
accepted. Accepted meaning that the sheets will be ran at the machine.
Post Processed sheets within the Nest Explorer are highlighted and
Accepted. When this is done the reports are printed for each nest
selected.
Show report tool station name- Displays station name from the turret
setup. Each station within the turret layout can have a station name
setup by the user.Show report picture within tooling- This option will
allow the report to show all tools and contours within the nest. When de-
activated the picture within the report will only show the external
contour of the parts within the nest.
Show report tool order as postprocessor- Displays the order in which
tools are used within the NC file. If there is a reposition within the
program the tools may be displayed twice with this option enabled.
• Open report automatically after postprocessor- Automatically create
a PDF file of the report, which is saved to the default location chosen in
the Post Processing dialog.
• To the right of this option is a drop down to select which type of report
that will be created. Within the drop down is ‘Plate report’ and ‘Run
report’. This will determine which report type will be created as a PDF
in the background. The report type is selected at the bottom of the
Report section of the Options dialog. ‘Plate report’ creates the PDF of
the report selected in Plate report and ‘Run report’ creates the PDF of the
report selected in Batch report.
Generate “.fms” file automatically after post processor- Activating
this option will allow the Post Processor to create an fms file when the
NC file is created. The fms file is used within Powerlink at the machine
for queuing of programs. It has information pertaining to the NC file
(run time, material used, sheet size, etc…).
Order
Always open nest explorer- Nest explorer will be opened when parts
are nested to view the different plates in that particular run.
Always add parts with the same material as fillers- Checks that filler
parts are tooled with the correct material type before adding to a nest.
Default manufacturing window- Value within this field is the amount
of days (ex. 5 equals 5 days behind or 5 days ahead). This is for nesting
filler parts. If a part is nested with a date outside the manufacturing
window and has a large quantity ordered the part will only be nested on
the current sheets. No extra sheets will be created for the filler part.
14

Basically is just used to fill in open holes within sheets, generally small
parts used for this.
• Run name - Enter a nest number only here (1-999998). This tells the
Database Orders which nest number to start at. For example, if you enter
1022 and nest parts from Database Orders the newly created nest would
start at 1023.
2.5 MATERIAL DATABASE
When creating parts within NC Express user (programmer) must use the same
material code and thickness that will be used at the machine. To do this
correctly NC Express uses the same database that resides in the FPL machine.
When the FPL machine is first started up it uses a database named
Laserprm.mdb. This stores all data relating to cutting conditions for the
machine.
The Laserprm database is copied from the machine to the programming
computer when or if any new materials are added to it. The reason the database
is copied to the programming computer is to easily match material setup at the
machine to what is setup in the software. The Laserprm.mdb is not actually
needed to run programs within NC Express. When a material is created within
NC Express it is stored to the Cam.mdb. The Cam.mdb holds all data set for
each material code and thickness within NC Express. Cam.mdb data being
Autotool settings, Nest settings, and Optimization settings. So, in actuality the
two databases work together but aren’t directly connected.
You can find both databases back in the following directory :
Fms\ncexpress\(your machine)\work
Cam.mdb- stores data for each material code and thickness. This helps
automate the software. For example, when a lead setting is changed for a
particular material code and thickness it is saved in the database to be used at a
later time.
Laserprm.mdb- Stores data relating to cutting conditions within the machine.
Used to determine types of material codes and thickness set within as well as
time information within NC Express. Comes with standard material codes and
thickness created by Finn-Power. Any additional codes and thickness desired
are the responsibility of customer.
2.5.1 Material Types
Shown on the next page is a screen shot of material code and thickness
selections. When a part or nest is created the material code and thickness needs
to be correct for each particular part or nest in order to properly run at the
machine. For each code type there may be one or more thickness set. When
clicking on each material code the thickness will change within the thickness
dialog pertaining to each thickness set for the selected code.
15

Description of European codes:
ALMg3: Aluminum
C15: Steel with a content of carbon
DC01: Cold Rolled Steel
DC01+ZE25/25 – APC: Electrolitical Zinc Coated Steel
DX51D+AS120 – A-O: Aluminum coated steel
DX51D+AZ150 – A-C: Aluminum zinc coated steel
DX51D+Z275-N-A-C: Thermical zinc coated steel
S420MC: Hot Rolled Steel
X5CrNi18-10: Stainless Steel
The codes:
(N2-5): Nitrogen cutting with 5” lens
(N2-7.5): Nitrogen cutting with 7.5” lens
(O2-5): Oxygen cutting with 5” lens
(O2-7.5): Oxygen cutting with 7.5” lens
Thickness:
The different size of material thickness.
2.5.2 Updating Materials
Clicking on Update materials… on above screen shot will allow editing of
materials loading within NC Express.
16

By opening the update materials dialog user has ability to edit material names,
delete materials, or add new. Even though there is the ability to edit the code
names and delete them you still want to keep the same name as what is loaded
within the Laserprm.mdb.
• Current materials list box: Shows list of current materials in the
database.
• Delete button: Deletes current selected material from the material
database. When you delete a material, it must not be
active in the Environment. If it is, a message box will be
displayed telling you that the current material cannot be
deleted from the database.
• Material name: Allows you to enter a new material code.
• Thickness: Allows you to enter a new material thickness.
• Add button: Adds the material you entered, into the database. Settings
(Autotool, nesting, etc…) for material that is currently
selected in current materials list will be copied to the
newly added material
Remember- Code names can be edited, but should not be. Material code names
and thickness should be the same, letter for letter. When a program is created
within NC Express the code name and thickness will carry through to the NC
Code generated to be run at the machine. When the NC Code is loaded into the
machine it will read to see what type of material is being used.
There are two different ways to enter new material types and thickness into
NC Express:
2.5.2.1 Directly from Laserprm (Read Laserprm…)
By clicking on the Read Laserprm it is possible to add a new material from out
the database that is copied from the machine.
Before clicking on the button select a material type and thickness that will be
used to copy parameters within NC Express.
When Read Laserprm has been clicked the list of new materials from the
Laserprm will be displayed.
17

To enter the new material into NC Express select material within the list and
click Add. The new material will be added to NC Express. Once the material
type and thickness has been added from Laserprm list the parameters
(Autotool, Intertool, Nesting, and Optimizing) inherited from previously
selected type and thickness within NC Express.
2.5.2.2 Manually enter material
When adding a material through NC Express by copying an already existing
type, all of the parameters set will be copied to the new material type and
thickness being created. It is best to select a material that is thicker than the
new one being entered.
Type over currently
selected material name
to enter new code,
repeat as well for
thickness. Once done
click Add.
Note- Creating a new material in NC Express will copy an already existing material
loaded within the Cam.mdb. When this is done all parameters set for the material
type and thickness will be transferred to the new one being created. Select a material
thickness that is thicker than what is being created.
EXAMPLE:
You want to have Aluminum from 1,5mm
Step 1: Click on Update materials
18

Step 2: Select ALMg3(N2-5) 2mm
Step 3 Change the thickness into 1.5mm (use point no comma)
Step 4: Click on Add
Step 5: If you want to add it answer is Yes
Step 6: Click OK and you can see that the material is added to the list
Now we want to delete a material:
Step 1: Click on Update materials
Step 2: Select ALMg3(N2-5) from 1.5mm
Step 3: Click on Delete
Step 4: If you want to delete it answer isYes
Step 5: Click OK and you can see that the material is deleted from the list
3 PART PREPARATION
The following section will cover the process of preparing parts within NC
Express.
This can either be done by importing DXF files or utilizing CAD features, this
will allow the user to create a CP file (*.cp) within NC Express. A CP file is an
actual part file, CP being the file extension.
Within a CP file there are many items that are remembered, these items are as
follows:
Geometry
Tool information (used tools & locations within part)
Sorting address
Material type & thickness
Turret used to tool part
First we will see how to draw parts in NceXpress and then how to import dxf
files.
3.1 CAD FEATURES
Within NC Express there are CAD features, which allow for part creation or
geometry editing. Section 3.1.1 will explain the function of all icons within the
CAD toolbar. A separate CAD manual demonstrates the features of the CAD
system and has also some exercises.
3.1.1 CAD
The first thing to familiarize with when using the CAD within NC Express is
the ‘Allow Selection’ icon on the toolbar. This icon will de-activate itself
when a CAD feature has been activated from the toolbar or menu. Once this
icon has been de-activated the ability to select any geometry within the
screen is not possible. To activate this use the mouse to click on the icon.
Once activated the user will see that the icon will change in appearance
changing to a lighter color.
19

3.1.1.1 Selection
Allow single and rectangular selection. The icon displayed
to the left shows the ‘Allow Selection’ icon to be de-activated and to the
right is active. Once de-activated the ability to select geometry or tooling
is disabled.
Activate polygon selection. Use mouse to connect lines around a
feature or features to be selected. Hit Esc key to allow anything within
box to be selected.
Lock and unlock geometry. Once locked, geometry is
unable to be selected. Once unlocked, all geometry is allowed selection.
Lock and unlock selected geometry (allows selected
geometry to not be moved when locked)
3.1.1.2 Snap Modes
Once the ‘Allow Selection’ button is understood the next important section
of the CAD to understand is the snap functions. The snap functions have
been designed to try and avoid accidental Snapping to incorrect points. In
the Drawing area, box around tip of cursor arrow, the cursor will only find
either end points of lines or real intersections. It will only allow free
points where these are expressly requested or where the function makes it
sensible to use them, e.g. Zoom.
For any function you can either use a point in the Drawing area or you can
use the snap menu to derive an additional point, which may or may not be
real. The following will describe the snap functions within the CAD
system.
Located on the right side of the screen when CAD is activated is the snap
toolbar (shown below). Within the toolbar are functions to help determine
the best application of CAD within a part file. On the next page the snap
function toolbar is shown along with a table of descriptions for all of the
functions. Along side each snap function a shortcut key is listed within
parenthesis.
20

Snap Function Description
Current (keyboard shortcut
key- U)
Last point drawn, usually end of line or
arc. Value is shown in the status bar
after completing a draw command
Free Point (F) Allows selection anywhere in the
drawing area
End Point (E) Snap to the end point closest to the side
the cursor selected
Intersection (I) Use the intersection of two points as
snap location or if two entities don’t
exist the location of the two clicks will
determine the intersection
automatically
Centre (C) Snap to the center of an arc or circle
Absolute (A) Snap to X and Y value in reference to
the 0,0 origin point
Relative (R) Snap to X and Y value in accordance
to the current point
Indirect (D) Coordinates relative to a point in the
drawing area. A window will pop up
asking for X and Y location. A point
will be asked for by clicking anywhere
in the drawing area. (Snap functions
not used after enter X and Y values)
Tangent (T) Draw tangent to an arc or circle from
the current point
Middle (M) Mid point of an arc or line
Horizontal (H) Draw a line horizontal to an arc or line
from the current point extended to
nearest element
Vertical (V) Draw a line vertical to an arc or line
from the current point extended to
nearest element
Perp. (Perpendicular) (P) Draw a line perpendicular to an arc or
line from the current point extended to
nearest element
Angle (G) Draw a line at a designated angle from
current point extended to nearest
element or snap point
21

Snap Functions (Con’t…) Description
X(p1)Y(p2) (Y) Within the Drawing area the X value from the
first cursor click location and Y value from the
second cursor click location are used to
determine the snap point. (Snap functions are
not used when this function is active)
Circle Axis (X) Quadrant point of an arc or circle nearest the
cursor
Polar (O) Calculates coordinate at a distance R and an
angle Theta from the current point (dialog box
will appear asking for both R and Theta)
Nearest (S) This is the point on the line or arc nearest to the
cursor
Fraction (N) Derives a point as being a certain fraction of the
way along from one point to the other.
< 0 Before first point e.g. –1 would
be the same distance back as that
between the 2 points
0 = First point
0.5 Midpoint
Second Point
1 After second point e.g. 2.0 would be same
distance forward as that between the two points.
Along (L) This derives a point as being a certain distance
along from the end of the line nearest the cursor.
A window will pop up asking for the distance.
Negative distances will be off the line
Construct (Z)- Allow the creation of construction line instead of drawing
geometry for selected draw feature.
Lock (K)- Lock a certain snap function on.
Hide- Hide the CAD toolbar.
22

3.1.1.3 Use of construction lines
Construction lines provide means of a Construction layer in which lines
are projected to some boundary, which the user can specify. Construction
lines can be saved within the drawing. The construction layer can be
hidden, locked or deleted like any other layer.
Construction lines are drawn to define an point on a part. With the correct
use of the snap points construction lines are sometimes unnecessary.
3.1.1.4 Numerical input (Evaluator)
A keypad is provided to allow numerical input using the mouse and/or the
keyboard.
C clears the input line

3.1.1.5 Selecting Elements for Using Copy/Move Functions
Under normal circumstances ‘Allow Selection’ is de-activated. The system
is by default set to specify what you want done and then ask to which
element(s) the function applies. However, when you want a function to
apply to a set of elements e.g. Copying, Mirroring you can set Selection on
by clicking on ‘Allow Selection’ icon, select the elements you want and
then invoke the requisite copy/move function
Three kinds of selection are provided when ‘Allow Selection’ is active:
Single elements Select an element. Clicking on something other than the
element deselects the selected element.
Multiple elements To collect individual elements hold the Shift key down
and select each element.
Rectangular selection Use the mouse to draw a box around the elements.
The elements must be wholly within the box if drawing box from left to
right. If drawing box from right to left any element touching inside the
box will be selected.
Polygon selection Draw a polygon around elements.
3.1.1.6 CAD Functions
These can be accessed either from the menu or via Toolbar buttons. The
Toolbar operates on a two level system – Column 1 is the main function
(Lines, Arcs, etc.), Column2 is the sub function of the selected main
function. The majority of functions remain activated until you choose
another function. The current function and the prompts are shown in the
status bar
Whenever a point is asked for it is asked
for in the bottom right corner of the status
bar. Points can be defined by clicking in
the drawing area or by choosing a snap
function.
On the following pages each of the CAD functions along with the icons
will be described.
24

3.1.1.6.1 Lines
Line between 2 Points. Prompts are for Point1 and Point2. If the
layer is construction the line will be projected to the bounds. A rubber
band line will be shown.
Line to End Point. Set first snap point and second will automatically
ask for end point of line.
Line parallel to a line at a given distance. Touch the line on the
required side and then give the distance
Line parallel to a line through a point. Select the line segment and
then define distance via snap function and exact line will be duplicated
parallel from the distance entered.
Two lines parallel to a given line. Touch the line and input the
distance
Common tangent to two circles. There are 4 possible tangents.
Depending on where the circles are touched determines which tangent is
drawn. To create an Obround draw two circles and 2 Common tangents
and then use the Cut 2 points function to remove parts of the circles.
Extend a line to the boundary.
Angle to line
Draw the bisector of an angle. If the layer is construction the line
will be projected to the bounds
25

3.1.1.6.2 Arcs
Note that the radius is positive in all cases. Where there is ambiguity the
system will display all the possible solutions one at a time
You can cycle through the solutions. Click OK when you have the one you
want.
Cancel rejects all solutions
Arc defined by 3 points
Semicircle defined by 2 points. *Note that there are 2 possible
solutions.
Arc specified by centre and 2 points. *Note that there are 2 possible
solutions.
Arc specified by 2 points and radius. *Note that there are 4 possible
solutions.
Arc specified centre radius and 2 angles. *Note that there are 2
possible solutions
Arc specified by centre, Start Point and Subtended angle. *Note that
clockwise angles are negative, counter clockwise are positive.
Arc Specified by Start Point, Start Angle, Radius and subtended
angle
Parallel arc at a given distance. Touch the required side and input the
distance. If on the inside the distance must be less than the radius.
26

Parallel arc through a point
27

3.1.1.6.3 Circles
Circle specified by centre point and diameter
Circle specified by 2 points that are on the diameter
Circle specified by 3 points
Circle specified by centre point and point on circumference
(diameter)
Circle specified by 2 points on the circumference and radius.*Note
there are 2 possible solutions
Circle through 2 points tangential to a line
Circle through a point with a given radius, and tangential to a line or
arc. *Note there may be 2 solutions
Circle with a given centre tangential to an arc or a line
Circle tangential to 2 elements with given radius. *Note there may be
2 solutions
Circle tangential to 2 elements with given radius. *Note there may be
up to 8 solutions
Circle tangential to 3 lines
Concentric circle. Touch side of circle and give distance
Ellipse defined by centre, Major Axis, Minor axis and angle of major
axis to the horizontal. The ellipse is immediately replaced by 12 arcs
28

3.1.1.6.4 Rectangles
Rectangle specified by 2 points
Rectangle specified by one point, and then Length and Width
Rectangle with radius corners specified by 2 points and radius
Rectangle with radius corners specified by one point, Length and
height and radius
Rectangle specified by centre point, and then length and width
Rectangle with radius corners specified by centre point
3.1.1.6.5 Notches
In each case you specify the side of the line and the point at which the
notch should go.
Rectangular notch Input width and height
V Notch Input Width and height
Angular V notch Input Width and angle
U notch Input Width and Height
Rectangular Corner Notch, touch two lines and specify the distance
along each line. First click represents Distance 1 and second represents
Distance 2.
Corner Loop
29

3.1.1.6.6 Trims
Trim 2 lines
Trim one element against another. Click on the part of the element to
keep. There are two possible cases
-If the second element intersects (or would intersect) the first, the first
element will be shortened.
-If the second element does (or would )not intersect the first, the first
element will be lengthened.
Extend an element to a point. The point must lie on the extension of
the element. This can be used to close gaps where appropriate but if this
condition is not met then either use or insert a line or replace the
element.
Cut an element between 2 points both of which must lie on the
element. Click on the part of the element to delete.
Split an element at a point. The point must lie on the element
Fillet, touch the 2 elements inside each and specify the radius.
Element lines do not have to intersect.
Chamfer, specify two lines and the distances from the intersection
point. The two lines do not have to intersect
3.1.1.6.7 Move
Here elements must be selected first
(see Select).
Move items from one point to another
Mirror in Y direction – specify a point to indicate where the mirror
axis is
Mirror in X direction – specify a point to indicate where the mirror
axis is
Mirror about an axis defined by 2 points
30

Rotate selected items from defined snap point
Move origin
Scale selected in X and/or Y
3 .1.1.6.8 Copy
Here elements must be selected first (see Select).
Copy selected item to defined location
Make a copy of the original mirrored in the Y direction – specify a
point
to indicate where the mirror axis is.
Make a copy of the original mirrored in the X direction – specify a
point
to indicate where the mirror axis is.
Make a copy of the original mirrored about an axis specified by 2
points
Grid copy
Polar copy around a point
Linear Copy along a line
31

3.1.1.6.9 Measurement
Measure Angle between two intersecting points
Measure Distance between two points. Gives angular distance (D),
X-axis distance, and Y-axis distance
Verify geometry.
With arcs the radius is shown, with circles the diameter. You can change
the diameter of a circle but not any other values.
Activates Evaluator (Calculator)
32

3.1.1.6.10 Modify Commands
Undo the last element create. There may not be a one to one
correspondence
between a function and an element e.g. Double parallel
lines. Each undo will step back another element.
Redo last undo function.
Activate this button and delete items by clicking on them.
Delete selected elements
Delete construction lines
Turn construction lines to real geometry.
33

3.2 IMPORT DXF FILES
The following section will cover how to import a DXF file. Along with
importing DXF files, problems will be shown that may occur when importing.
Problems that are shown will help in fixing DXF files when these problems may
occur. At the end of the section exporting a DXF will briefly be covered.
If the part you are going to use exists as a DXF file and you want to modify or
create a cp file from the DXF, you will have to import the DXF from the folder
where it is stored. In NC Express, under C:\fms\ncexpress directory, there is a
folder called ‘geomdir’. The ‘geomdir’ folder is the default location for DXF
files. The default DXF directory will automatically change to the last directory
where a DXF file was imported.
3.2.1 Import a good dxf file
To import a good DXF file is very simple.
Step 1:
1. File menu | Select Import…
2. Click on toolbar
Both of these options will bring you to the Open dialog box with the ‘geomdir’
folder. If the DXF is not located in the ‘geomdir’, navigate to where the DXF
is located on your machine or on a network.
Select DXF file through Windows directory : DXFOK\Drawing 1
Step 2: Once you have found the DXF, click on it and click the Open button
in the dialog box. The DXF should now be displayed on the screen.
Note – If there are other layers (numbers, letters, or other characters) on the DXF,
they will be disposed of later when Autotooled, leaving only the part geometry.
34

In the case where a DXF file is being imported from the flat, NC Express will
import all layers of the DXF file. It is important that all part geometry
(internal & external contours) is on it’s own separate layer(s) when doing this.
All unwanted layers (ex. Dimensions) can be filtered out of the file when
Autotooling the part. Picture below shows a part that would be imported with
many different layers within.
To save part either go to File menu | click Save, or click on toolbar.
Once saved directory where the part resides and name of part will appear on
top of the screen.
Now the part is saved as a cp file in the partdir from your machine. See for
more explanation at Storing CP files.
Note- When saving part the DXF file name will now be the part name. If part
will be named differently click Save as… in File menu.
3.2.2 DXF files that are not OK
When importing DXF files into NC Express they are checked to see if there
are any open contours or duplicate lines. The following explains how open
contours are found and what defines an open contour.
3.2.2.1 Duplicate lines
For the following exercise create a new part, material type and thickness does
not matter.
Import DXF file from- dxf nok/duplicate contour dado.dxf
The error message below will appear:
35

What this means is that there are unclosed contours found. It can be one of
two things: unclosed contour or duplicate lines.
To view what is wrong in this drawing go to View menu | select Display →
DADO end points. This will give user the ability to see where the problem
area is. Below shows circles with crosses through them to display the
problem.
For this particular part there are two different duplicate lines found. Select the
duplicated lines and delete them. When there is a duplicated line that is the
same length NC Express will delete this line automatically. When there is
duplicate lines partial length of another it needs to be deleted manually.
3.2.2.2 Duplicate lines (automatically taken out)
Import DXF file- training/dxf nok/duplicate contour non.dxf
For this particular DXF file there are duplicate lines that will automatically
taken out, but NC Express will warn that there are duplicate lines to be
automatically removed.
36

The duplicate lines were ignored here when importing. When file is saved and
reopened the duplicate lines are gone.
3.2.2.3 Open contour
The following demonstrated an open contour found within a part. The error
message shown below is displayed when this occurs:
Go to View menu | Display → DADO end points
As seen in picture shown there is an unclosed contour that needs to be
trimmed to make corners meet. To trim go to Edit menu | select Trim.
Trim- click first vertical line and then the diagonal line but click it on the side
that can not been cut.
NC Express uses a tolerance value to check for open contours when importing
DXF files. This tolerance value is set at a default value 0.0025. The value set
for the tolerance can be found in the Environment dialog shown below:
37

3.2.3 EXERCISE
Import the following DXF files and determine the problems within:
Training/dxf nok/troubles.dxf
There are many different problems here. Fix all the problems and save the
part with no error messages.
3.3 CP FILE (PART FILE)
In NC Express to create a part file you are able to import a DXF file, or by using
the CAD functions create a new part and save it as a CP file. There is also the
ability to export a CP file as a DXF file. A CP file is how a part’s information is
stored within NC Express. CP file is stored in ASCII text format and holds part
profile and tooling information. Information stored within a CP file is as
follows:
Part name (ID) Geometry
Material type and thickness Sorting type & Address
Revision Level Tooling
Once a CP file is created from DXF or from CAD features it is then ready to be
tooled, either automatically or interactively.
When creating a new DXF or cp file, there are part properties to take into
consideration. Many of the properties a part retains are listed above, in the bullet
list of the opening paragraph of this section. NC Express will use, throughout
the application, the properties that are set in the Part properties dialog box.
3.3.1 Create New Part
Each time a new part is created within NC Express there are important settings
that need attention when starting. Below describes the settings of creating a
new part within NC Express.
Step1 : Create a new part and fill in the properties
1. Go to File menu | New → Part
2. Click Icon on toolbar
Both times next screen will appear
38

Description of all fields on the New Part dialog.
Nesting:
• Common line- Allows the part to be commonlined in the nest. Only
select Commonline for parts that will be commonlined.
Default the commonline option is set on Yes, so if we want a part that is
not common lined on nesting level then we have to disable this option.
• Allowed Nest rotation (Grain direction)- Defines grain direction for
laser parts. Initial part is imported at 0° rotation unless otherwise declared.
For example, selecting 0/180 will keep grain direction moving side to side
on part. If grain direction is not applicable for a part than both options can
be selected. This applies rotation within the nest. This can be turned off
also when nesting parts, but is declared for each part.
• Initial rotation- Tells what the initial rotation of the part is during nesting.
Information:
• Turret- Not applicable in FPL.
• Sorting- Not applicable in FPL.
Material:
• Code- Allows you to select the material type for the part.
• Thickness- Allows you to select the material thickness for the part.
• Update materials button- Clicking this will open a dialog box
allowing you to add or delete material from the database
Defined in earlier section Material Types
39

• Note- Ability to add remarks for a part. Allows you to type in
information about the part for later use or output into a report.
• Alias- Regular part name
• Revision value- Revision number of the part
• Quantity- Number of regular parts
Step2 : Click the OK button. The NC Express screen will now be blank. You
are ready to create a new part.
Note – Part properties for a part that were set in the New Part dialog can be viewed
by going to Settings menu | Properties. Ex. If a part was created and part properties
were set for that part, when you open the part in NC Express, you are able to view the
properties from the Settings menu | Properties.
Once we have created the new part or the cp file we can start drawing the part
or we can import the dxf file into NCeXpress.
3.3.2 Storing CP Files
Part files (CP Files) are stored, by default, in the PARTDIR folder under the
machine being used. When you click save on the toolbar, the file is saved with
a .cp extension in the PARTDIR folder under the current machine being used
(C:\fms\ncexpress\’machine name’\PARTDIR).
There is the ability to have multiple folders under the PARTDIR folder. (Ex.
You may have a folder for each material type under the PARTDIR folder. In
each of the material type folders, you may also have a folder for each material
size). It is important that parts are stored properly within the default part
directory because when nesting the nest engine searches the default part
directory for the parts being nested. The default part directory set is the base
of the tree hierarchy, nesting will search through all folders within the default
part directory until the part(s) is/are found.
The default part directory can be changed to a different location either on the
PC or Network. The following will demonstrate how this is done:
3.3.2.1 Exercise- Changing Default Part Directory
Step 1: Go to Settings menu | Machine Parameter | Environment.
The Environment dialog box will now be displayed. (See picture below).
Select the second TAB-Page : Directories
40

Step 2: Click the Browse button next to the Part directory text box. This will
display the Open dialog box allowing you to change to a different directory.
Step 3: Navigate to a different folder either on your computer or on a network
where the cp files are located or will be saved.
Note – When changing to a different part directory, a cp file must exist in the
directory you will be changing to
Step 4: Click on one of the cp files and then click the Open button. The Part
directory text box will now display the path that you have selected.
(Ex. \\SERVER\TURRET\CPFiles)
Step 5: Click the OK button in the Environment dialog to accept the changes.
Note – As described before, you may have several folders under the PARTDIR folder.
Ex. C:\fms\ncexpress\LASER_MM\PARTDIR\CRS\030. When you click the Open
button on the toolbar, the Open dialog box appears displaying the contents of the
folder that you set in the Environment. As shown in the path location example above,
the contents of folder 030 will be displayed
Remember – When working with multiple folders, make sure to save the cp file in the
correct folder. This is easily done by going to File menu | Save As and navigating to
the folder where the cp file is to be saved. Once you have done this, every time you
want to save the file again, you can use the save icon on the toolbar and the file will
be saved in the same location.
3.3.2.2 Networking Part Directory (Sharing)
The ability to change the default part directory location is the same as sharing
amongst multiple users. The PARTDIR folder can be transferred to a desired
location (Ex. network or Main PC) to be shared amongst one to many users.
Sharing the PARTDIR folder is useful if there are changes made quite often or
if many parts need to be added to the system. To share the PARTDIR folder,
copy the PARTDIR folder to a shared location (Ex. on network or Main PC).
If the part directory will be stored on the network it is a good idea to make
sure the network administrator is involved with this process. Once parts are
stored correctly on the network (or Main PC) the process to set the default part
directory is the same as the exercise 3.3.2.1 in the previous topic. Please
follow the steps of the exercise for each user that will be attached to the part
directory.
41

Remember - Each time a part is modified by a user, any other user working on the
same part should re-open the part. This will refresh any changes or new editions
made to the part.
3.4 PARTS DATABASE
Used to efficiently display part information pertaining to how parts were
programmed. Parts database is used to library parts from one or many part
directory(s) of one or many machine(s). The part information has the ability to
be sorted by machine or even by each field. Information stored within the Parts
database is listed below:
Field Description
Part ID ID # of part within database, ID # will
change if part is removed & added again.
Name Part name
Machine Machine part is programmed for
Material Material type
Thickness Material thickness
“CP” File Directory in which part is stored
Sorting Type Sorting type applied to part
Sorting
Sorting address applied to part
Address
Turret Turret used when tooling part
Slug Hole Ash hole used (LP combination only)
Revision Revision level of current part
Comments Notes entered by programmer
When a part ID is selected within the Parts database the part geometry is
displayed in a viewer next to the Parts database dialog.
3.4.1 Adding Parts to the Database
When NC Express is first used the Parts database is empty. Adding parts to
the database can be done three different ways: save part, Add part through
dialog, or Load from part loading directory.
Save Part- When a DXF file is brought into NC Express and saved as a CP
file it will automatically be added to the Parts database. Part property
information for the file is read and input into the database. This is done for
each part that is saved and not already in the database.
Add Part- When the Parts database is opened there is a button on the bottom
of the dialog, Add. Clicking this button will allow the user to add parts from
any directory where parts are stored. This process can only add parts on a
part-by-part basis. Part properties that can be changed when adding a part:
Machine, Material type and thickness, Revision, and Comments.
42

Load Parts- In the case where the Parts database is empty because it was
cleaned or is new to an already existing user, there is an option to load many
parts from a selected part directory at once. To Load multiple parts at once the
‘Part loading directory’ needs to be changed to the location of desired parts.
Once ‘Part loading directory’ is set click Load on Parts Database dialog and
all parts within will be loaded within. All part property information will be
loaded automatically for each part. Each part directory will need to be loaded
separately.
3.4.1.1 Editing Parts within the Database
Any part within the Parts database can be modified within. There are only
certain fields that can be modified. These fields include: Machine, Material
type and thickness, Revision, and Comments. To edit a part within the
database, highlight the part and click Edit to view and modify fields available.
Edit dialog is the same as Add dialog, with the exception of Select part option.
Reasons to edit, if a part is needed on another machine then it was
programmed for. Part machine would be changed as well as respective
material type and thickness. Comments or revision level can be changed for
parts by highlighting parts and clicking Edit.
3.4.1.2 Sorting Part Information within the Database
Information within the Parts database has the ability to be sorted to easily
display what the user is looking for. All fields displayed can be sorted by
clicking in the header (field name) within the dialog. Parts for specific
machines (if multiple machine user) can be sorted by machine by selecting the
desired machine from Machine drop down box.
43

3.4.2 Super Part Reporting (Grid Parts Feature)
Super Part defined is a grid (multiple parts) of one single part. Within
Drawing menu | Features is a feature Grid Parts that will create a grid of parts
using one single geometry external contour to be processed within NC
Express. When the Grid of Parts uses the main part, the original part name
(Alias) and how many parts created (Quantity) is added to the Part properties
page automatically for the new Super Part (Grid of Parts part).
After a Grid Part is created the part properties can be opened through the
settings menu to view the original part name as well as how many parts will be
created within the Super Part. The original part name is found in the ‘Alias’
field and quantity of parts within Super Part is found in ‘Quantity’ field.
When the Super Part is nested the Alias part name will be output in the report
as well as the Super Part name. More report information will be found later in
this document for Super Part reporting.
44

4 TOOLING PARTS
Once the dxf is imported or the part has been drawn then we can apply tooling
on the part so that all information is in the cp file.
The following section will cover the processes within the system to apply
tooling to a part whether it is automatically applied or manually applied. The
first two sections will cover the use of the automated tooling of NC Express.
The next Section will cover the use of manual tooling.
4.1 AUTOMATIC (AUTOTOOLING)
The Autotooling function is a fully automatic tooling system that works with the
existing CAD database (Cam.mdb). Autotool breaks the part geometry into
predefined features (geometric entities). It then proceeds to tool these geometric
entities according to tolerance settings and priority of tools. Autotool requires
minimum input from you. At the same time, it gives you enormous flexibility in
tooling the parts. Nibbling and punching priorities are used here to distinguish
which tools are used first. Tolerance levels are used to set tolerance limits for
each type of geometric shape.
The information within this section is tailored to the application of tooling parts
for a Finn-Power Laser machine utilizing the Autotool feature within NC
Express. Below are hyperlinks to jump to different sections that will explain
settings as well as how to apply Autotool to different applications:
CAM Database
Settings
Single part
Presheared parts
Commonline parts
4.1.1 CAM Database
Autotool has a variety of settings (Autotool, Nesting, Optimization, and Post
processing parameters) that can be edited for each material type and thickness
loaded for a particular machine. In order to remember each of the settings per
material type and thickness there is a database in the background that stores
the settings within for each type and thickness.
The database that holds this information is named CAM.mdb.
Each time a part is created or opened, the material type and thickness settings
are then accessed from the database. When Autotool is opened the settings
that were saved to the database last are then opened and loaded in Autotool
dialog. Settings for each material type and thickness are saved when
switching between them or closing NC Express
A suggestion is to first find settings that will work for the material type,
thickness, and machine. Once these settings have been established they will
not have to be changed by the user, unless for unique parts. The Cam.mdb
given with the machine install is a starter database with values
45

for the materials within that is set as a base. It is up to the customer to add
new materials and set settings for all of their materials.
For the FPL/L6 machine there is a Laserprm.mdb that goes along with NC
Express. The Laserprm.mdb is stored in the Work directory inside the
machine specific folder. This Laserprm.mdb is setup at the machine. NC
Express checks the Laserprm.mdb to see if a material exists. If an NC Express
user is creating a new material type in the software and the Laserprm.mdb has
not been updated, NC Express will give an error message stating the material
does not exist in the Laserprm.mdb (see creating new materials). If the
operator at the machine is entering new material into the Laserprm.mdb (at the
machine) this file needs to be copied to the Work directory of NC Express to
update new materials for the software.
4.1.1.1 Saving Settings to CAM Database
When a setting within NC Express (ex. Autotool parameter) has been changed
that is stored within the CAM database NC Express will ask if the user wants
to save the settings for the material type and thickness that was being used.
NC Express will ask to save when material type and thickness is being
changed within the system or when NC Express is being closed. Below is a
screen shot of the message that will appear when the system will ask to save
settings.
The goal in using a CAM database is to find settings that will work for overall
use for each material type and thickness. For example, a specific material
requires certain size parts to be tabbed into place, you would set the
microjoints to be applied each time for that specific part geometry dimensions.
If a parameter is for a one-time use then when the system asks to save settings
click ‘No’.
Again, a suggestion is to first find settings that will work for each material
type and thickness. Once these settings have been established they will not
have to be changed by the user, unless for a unique case. The Cam.mdb given
with the machine installation is a starter database with default materials loaded
within. It is up to the customer to add new and set parameters for all
materials.
46

4.1.2 Settings
1. Go to Tooling menu | Autotool
2. Click Icon on toolbar
By clicking this button the following dialog will appear
4.1.2.1 General tab
General tab gives the user the ability to set all major functions of Autotool,
when Autotool is first opened. Functions Machining mode, tooling
(alternative & where tools are used from), and Sorting applied are found here.
DXF file CAD layers can be filtered from parts here.
• Machining mode- select the type of tooling to be placed on part. For
turret punch press machines only punch and nibble can be selected.
• Laser- used to tool a part with shear tooling.
• Preshear- tools only interior geometry
• Use taught cycles- enables the use of taught cycles that have
been created.
• Laser cutting mode : We can select different settings for this option.
- Normal mode
- High speed cutting mode
This option makes it possible to have an optimized nesting with different
cutting modes on one plate.
47

Alternative Tooling – Allows user to tool part with variational tooling
(tooling a part with 1 or more rotations).
o Use only 1 tooling- only tools part at 0° orientation. Part can
then be nested only at 0° rotation.
o Use 0° & 90° tooling- tool parts only for 0° & 90° rotation for
nesting.
o Use 0° & 180° tooling- tool parts only for 0° & 180° rotation for
nesting.
o Create 4 tooling orientations- tool parts in all orientations (0°,
90°, 180°, and 270°).
Tool this orientation only- tool only selected orientation with Autotool
again.
CAD Layer Filter- used to filter layers of dxf files and DADO lines and
points.
o Closed Contours- closed geometry used by system for offset
cutting. This variable can be alphanumeric or “ALL”. Layers
from imported dxf file that are desired layers to be tooled are
entered exactly as NC Express sees them. (Layers defined can be
viewed by going to Settings menu | CAD then select layers…)
o DADOS- open geometry used by system for centerline cutting.
Cannot be “ALL”. Enter DADO for DADO lines to be tooled.
4.1.2.2 Microjoint tab
Microjoints (tabs) are applied when a piece of material will be left within the
sheet or within a part. When a microjoint is applied there is a small gap
between two punch hits or in the corner of a part, allowing the material to stay
in place. Microjoints can be applied to either internal or external contours.
Settings within Autotool allow the user to set restrictions on which line
segments will have microjoints applied. The size of the gap (joint width) or
microjoint tools can be used also. All values here can or will change
depending on material type and thickness.
48

External/Internal Contour properties-
• Min. segment length- Minimum length of segment to microjoint.
• Microjoint length- distance of microjoint.
• Max Microjoint distance- max. distance between microjoints.
• Lead-in settings- See Lead-in settings in this Appendix.
• Lead-out settings- See Lead-out settings in this Appendix.
• Microjoint tools- Option to allow the use of a special tool as a
microjoint tool when using punching only. (Not applicable for FPL)
49

4.1.2.3 Path/Leads tab
Controls laser lead-ins/outs and technologies that will be used per line
segment dimensions. Pilot holes, Fillets, lead’s length & angles are some of
the items controlled within the Path/Leads tab.
Set Contour defaults here along with lead-in and lead-out settings.
Commonline cutting parameters are set in this tab as well.
• Contour types- Set dimension limits for each contour type within the
Autotool settings. Notice how each value is placed in-between both contour
types. Contour types are defined in the machine parameters of the Settings
menu. Default they are set as High Speed, Large, Medium, Small. Defining
the two values will allow Autotool to distinguish what dimensions of
geometry within a part will be tooled with which type of contour. The above
example states that any
dimension of a contour greater than 50 will use the High Speed
dimension of a contour between 50 and 8mm will use the large contour
dimension of a contour between 8mm and 4 mm will use the medium contour
dimension of a contour less than 4mm will use Small contour.
• Pierce point- We can also fill in a value for Pierce point , this value can
not be more then the minimum dimension for small
contour. (in this example not more then 2.7) If we put the
value to 1.5 mm then all contours between 0 and 1.5 mm
will not be cut only pierced in the middle of the contour.
Exercise on Pierce Point
50

• Lead-in settings See Lead-in settings.
• Lead-out settings - See Lead-out settings.
• Auto Cycling- Enable auto cycling of laser cutting. Used for faster
cutting sequencing (high speed).
Common Line Cutting-
• Minimum width of internal common line contour- Allows
for cutting head to not drop down any large holes within a nest of
commonline parts. Any cutout larger than this value disables laser from
cutting continually.
• Laser beam width (IMPORTANT)- Sets beam width to
check for radius’ less than half the beam width, to avoid problems at the
machine. If a tooled part has a radius/line less than half the beam width
the machine stop and give an error message telling operator that there is
a problem with the nest.
• Lead-in & Lead-out lengths- Sets lead-ins and lead-outs for
inside and outside edges of commonlined parts.
4.1.2.4 Lead in – Lead out settings
1. Lead-ins settings
If we click following button then we get following dialogbox :
51

Straight Lead-in
L1- Initial length of lead-in.
L2- Secondary lead-in length.
Ability to split lead-in into two section, to change technology for one and
remain same as contour for second.
A1- Angle of lead-in. Measured perpendicular from the contour.
T1- Change technology for L1 lead-in.
T2- Change technology for L2 lead-in.
Back and forth
Pierce point Intermediate point
Start point of contour
52

At the pierce point a piercing is made through the material. Optional, there can
be chosen to first make all the piercing points and then return in the pierce hole
to continue.
Then there will be a cut in a straight line from the pierce point to the
intermediate point. The length is set by value L2 and the technology used in this
by T2. When the intermediate point is reached, we return to the pierce point,
using the same technology as before, set by T2.
When we reach the pierce point, we return again to the intermediate point, still
using the same technology as set with T2.
When we then reach the intermediate point for the second time, we switch to
technology as set in T1, this can of course be the same technology as used in T2
but it does not have to be.
We then cut in a straight line to the start point of the contour, the length of this
segment is set with L1, after reaching the start point of the contour we switch to
the technology set on the contour (different dialog in NCeXpress) and continue
cutting the contour.
Arched Lead-in
L1- Length of Lead-in.
A- Angle of Lead-in. Measured perpendicular from contour.
R- Radius of Lead-in.
T1- Change technology of R Lead-in.
T2- Change technology of L1 Lead-in.
53

Lead-in with hole
R1- Radius of lead-in
R4- Radius of hole
A1- Angle of lead
L1- Length of Lead-in, not including arc
Spiral Lead-in
R1- Radius at entry of lead entry on contour
R3- Radius end of spiral
R4- Radius of spiral
N- number of spiral lines
L1- Length of lead
54

Add loops to corner
Enable- Enables (activates) corner loops.
Value 2.2- Radius of loop.
Value 1.2- Length of lead line to radius of loop.
Value 20- Any corner with an angle less than
(x) angle will have corner loops applied.
Fillets
Enable- Enable (activate) fillets to be applied to
corners.
Value 2- Radius of fillet.
Value 91- Any corner with a angle of 90 or less
will have fillets applied.
Overlap
Value 1- Amount of overlap between
lead-ins and lead-outs. Maximum value
for overlap is set as default 3mm
in machine parameters | misc tab
(Max. overcut).
T1- Change technology for overlap.
Enable- Enable (activate) overlap.
Minimum distance to contour
Sets minimum allowable distance for end of lead to
be from contour of part. If pilot hole distance
measured from closest outside edge of tool. If no
pilot hole distance is measured from center of
pierce point.
If this distance in combination with the desired length of a lead-in gives a
conflict then the lead in will be shortened.
55

Hole size for pierce in center
If we fill some kind of value in this parameter then we
will pierce in the center from every geometry from
0mm until this value.
For example 6 mm : we will pierce in the middle of
each contour that is not larger then 6mm.
If we fill in a value at the lead in settings for Large contour, then this value
will automatically be filled in at the settings for Small and Medium contour.
Important- Settings for Lead-ins are saved in the Cam.mdb database for each
material type and thickness, so each time that material is used the settings will
be re-used each time that material type and thickness is used. When settings
are changed for a material type and thickness and user exits to another type
system will ask to save settings, click Yes to save and re-use. Settings for
microjoint lead-ins is different from normal lead-ins.
Piercing type (only for L6 with Controllink)
For each contour type we define also a piercing
type.
In thin materials we don’t use piercing so then
the option No pierce is enabled.
In thicker materials we will use the fast,
medium and fine pierce according to the contour
type we use.
This means if necessary we can choose another
piercing type when using when of the contour
types (or technologies).
56

Lead-out settings
When we click on following button - the lead out dialog box will appear
:
For lead outs there are no different types :
L2- Lead-out length. Maximum lead-out length set in machine parameters |
Misc tab (Max. Leadout).
R2- Radius of Lead-out. Set to zero (0) to make straight lead-out.
A2- Angle of Lead-out. Measured perpendicular from contour.
T1- Change technology for R2.
T2- Change technology for L2.
57

Minimum distance to contour- Sets minimum
allowable distance for end of lead to be from
contour of part. Measured from end of lead-out.
Important- Settings for Lead-outs are saved in the Cam.mdb database for
each material type and thickness, so each time that material is used the settings
will be reused each time that material type and thickness is used. When
settings are changed for a material type and thickness and user exits to another
type system will ask to save settings, click Yes to save and reuse. Settings for
microjoint lead-outs is different from normal lead-outs.
Technology settings
For every lead-in type we can set the length and technology per segment by
pressing T1 or T2 (to select the technology) you get the following screen:
Mostly we choose a technology: ‘As contour’.
When we cut thicker material it can be necessary to let the process start
slower, so then we can choose another technology (small or medium contour).
Push ‘Apply’ button and the technology will be set for the lead-in.
4.1.3 Single Part
Using Autotool is a very simple task. The thought is to create your geometry
either through NC Express CAD or by importing a DXF file. Once you have
geometry on the screen you are ready to use Autotool. Single part is the
basic processing of a part. In section 9 you will find back some exercises.
58

4.1.4 Presheared Parts
Presheared relates to parts that will be nested on a plate that has the same
dimensions as the part. Parts are tooled using ‘Preshear’ machining mode
through Autotool to be processed into NC code.
To be able to explain this we first have to go through the nesting and
optimizing. This will be explained with an exercise.
4.1.5 Commonline Parts
Commonline parts are parts that will share geometry of their outside contour.
Important thing to know when this geometry is shared on the outside of a part
when cutting with a laser is that there is a compensation for the beam width
added to accommodate for loss of material on the part. This way the part will
not have smaller dimensions.
There are 2 ways to handle the commonline cutting:
4.1.5.1 At part level
When you handle the common cutting on this way then it is only possible to
create a common cut between one and the same part.
This means that you will create a large part that contains x times the original
part. To do this we have to use Grid Parts from the Drawing menu | Features.
There is an exercise at the end of this manual demonstrating the procedure of
how to create commonline parts at part level.
4.1.5.2 At nesting level
When we create a common line on nesting level then this means that we can
create a common cut between different parts.
To do this the parts should be prepared (tooled) as usual, use the standard
database settings. A leadin/out will be created on the outer contour, but when
the part is nested commonlined, the optimiser will delete the leads and replace
them with commonline cuts
There is an exercise at the end of this manual demonstrating the procedure of
how to create commonline parts at nesting level.
59

4.1.6 Exercise- Autotool Parts
In the following pages there are a few exercises demonstrating how to apply
tooling through Autotool. DXF’s will be imported and tooled in a specific
fashion to show the uses of Autotool. As well as tooling the parts, the
following exercises will give insight on how parts should be tooled for the
FPL.
Create new part and import DXF file: Training FPL\DXFOK\Drawing 1
To start Autotool function go to Tooling menu | select Autotool. Or select
from the toolbar.
Once Autotool is started a dialog box will appear.
First tab (General) allows editing common tooling as well as CAD layer
filtering. For this exercise don’t edit any fields on this tab.
Second tab (Microjoint) will add tabs to parts.
60

Microjoints are placed on a part when thin material is used and there is a
possibility that the part can fall through holes of table during cutting. So,
microjoints are placed to keep the part in place. If part happens to fall into
table it may be partially sticking out of the sheet. If cutting head hits part it
will stop the program from running. It is possible to place microjoints on the
external and internal contours.
First we have to enable the type of microjoint we want to place.
For each type of material (also different thickness) the settings for the lead in
and lead out will be different but we are able to edit the lead-in and lead-outs
from the microjoint tab by pressing the following buttons:
For the external microjoints:
For the internal microjoints
Lead In Lead Out
Lead In Lead Out
NC Express will never put microjoints on a part if we didn’t enable the
microjoints. But NC Express will set the lead-in and lead-out settings for the
microjoint and these settings are depending from the material that we are
using. Until the user has saved new settings within Autotool for a material
type the settings will be default until settings are changed and saved.
61

Once Microjoints have been set and established move to the Path/Leads tab.
Path/Leads tab allows setting of contours, leads for each contour, and
commonline settings.
Dimension limit
Everything > 8 is a large contour; this means that every contour larger then
8mm will be cut with the large contour technology.
Everything between 8< >4 is a medium contour, this means that every contour
between 8mm and 4mm will be cut with the medium contour technology.
Everything < 4 is a small contour, this means that every contour smaller then
4mm will be cut with the small contour technology.
Don’t change the large contour value to be a smaller value; it is bad for the
axis from the FPL machine. When cutting a large contour the cutting head is
moving with a speed that is faster then we are cutting medium or small
contours. So if we change the value for large contour to 1mm this means that
everything bigger then 1mm will be cut with this faster speed. This is not good
for the axis from the FPL.
62

Pierce Point
If we put a value for the pierce point then this means that all contours between
0 and that value will not be cut only pierced in the middle of this contour.
This value can not be more then the minimum value for small contours.
Let us first continue this exercise and then make a new exercise on Pierce
point.
Leads
For each type of material (also different thickness) the settings for the lead in
and lead will be different. Also the other features like : loops, fillets and
overlap will be automatically set when it is needed for that kind off material if
saved this way.
But it is possible to change the settings for every type (large, medium, small)
of contour.
Lead in
Lead out
The selection for Lead-in and Lead-outs is the same for each type of contour.
Each Lead-in setup is the same for each contour. As well as Lead-out.
As seen above there are the same four types of lead-ins, but now there are
three new features added for the Lead-in. Microjoints don’t use these
additional features. The additional features are used for:
For every corner smaller then 90 degree we will make a loop.
You can also change the 90-degree in a smaller or larger corner.
63

For every corner larger then 110 degree we will make a fillet.
You can also change the 110-degree in a smaller or larger corner.
There will be an overlap of 2mm of lead-in and lead-out depending on which
contour this feature is activated for.
(large or medium or small contour)
Tooling part
Once lead-ins have been set click apply, then OK on Autotool dialog. Part
will now be tooled.
Finished part
64

4.1.7 Autotool Example 1- General
The following will use examples of Autotool to help understand how features
of Autotool can be applied.
Step 1: Start by drawing a part:
a. New part: Aluminum 8mm
b. Draw a rectangle 40mm x 40mm.
c. Draw circles with the following
diameters:
16.5mm
8.5mm
5.5mm
Step 2: Autotool part with settings below:
General tab: no changes
Microjoint tab: Microjoints disabled
Path/Leads tab: Enable lead-ins and lead-outs use settings from Lead-in
screenshot below for Lead-ins.
65

Step 3: Click OK to Autotool part.
The part will be tooled with a pilot hole being cut before starting into
contours. Auto cycles are applied to all leads for each contour.
Step 4: Go back to Autotool and go to Path/Leads tab:
Edit Dimension limits to change technology applied to each contour. Also, go
to Lead-ins to add Loops to each contour by enabling loops.
Click OK to apply new tooling to part.
Step 5: Go back to Autotool and go to Path/Leads tab:
Edit Lead-ins, disable Loops and enable Fillets as well as overlap. Values can
be changed to edit outcome.
Step 6: Enable microjoints to be placed on part.
4.1.8 Autotool Example 2 – Pierce Point
In this example the meaning of the pierce point will be explained :
1. Go to File menu | New → Part OR
2. Click Icon on toolbar
3. Take as material Aluminium 2mm
4. Create new part and import DXF file: Training FPL\DXFOK\Drawing 2
In this dxf file we have holes with diameter 3.1mm , 4mm and 5 mm
66

5. Go to Tooling – Autotool and go to the tab page Path/Leads
Fill in the value 3.5 for Pierce point.
This means that all contours between 0 and 3.5 will not be cut only pierced in
the middle of the contour.
If we now press the OK button then we get following tooling for this part :
These holes have a
diameter from 3.1mm
67

As you can see there is no technology on the contour so this will not be cut. We
will only have a piercing in the middle of the contour.
If want to have this also for the holes with a diameter of 5mm then we have to
change or values from the small contour :
You can see that all inside contours will not be cut only be pierced.
Diameter 3.1
Diameter 4
Diameter 5
Now we will see what we have to do if we don’t want to have the holes from 4
diameter to be pierced.
First we do the same as above and make the autotooling.
Now we can select the holes with a diameter of 4mm one by one and holding the
SHIFT button down.
68

When we now are going to run the autotooling then this will only be applied on
the selected geometry.
Go to tooling – Autotool
Put the parameters again on the original values : 8 – 4 – 0
Push the OK button and let autotool run.
You can see that the holes will be
cut as a medium contour
69

4.1.9 Autotool Example 3 - AutoCycling
The following example will use a different part to demonstrate the
applications of Auto cycles. Auto cycles are applied in the Path/Leads page of
Autotool.
Autocycling
The cycling will be done in such a way that the cutting head doesn’t move
over a cut part. This means that cycling will replace the lead-ins off the
geometry so that it can be optimized. When the cutting head moves over
pieces that already have been cut then there is danger that those pieces have
skipped/tilted and you can get a nozzle touch.
If Autocycling is disabled then the lead-ins will be placed all in the same
direction and if desired a manual cycle would need to be created:
Autocycling will always give the fastest way and the most secure way of the
cutting process.
Step 1: Import dxf: cycling.dxf
Step 2: Autotool with Auto cycles enabled.
View the sequence and how the leads are placed.
Step 3: Now Autotool with Auto cycles disabled.
View how the leads are placed in the same direction.
A manual cycle can be created and will be seen in Manual tooling section for
this part.
70

4.2 MANUAL TOOLING
Interactive tooling (manual tooling) is used to tool intricate part designs.
Sometimes Autotool will not tool the part in the desired fashion. Through
Interactive tooling you can have the freedom to tool/edit the parts manually.
Interactive tooling feature
o Text Marking
o Manual Cycling
Modify tooling/part features
o Piercing technology
o Process technology
o Tabs
o Leads
o Break laser path
o Direction
o Loops
o Fillets
The following subsections will describe and show how to use the interactive
features of NC Express.
4.2.1 Text Marking
Feature used to add text to a part using laser or a scribe tool, if scribe tool is
available. Text can be entered into dialog box; font size can easily be
changed. Once entered text will be applied as tooling in the middle of the part
to be moved to desired location. There is currently only one type of font. This
feature can be found by going to Tooling menu and select Text marking.
Text: Fill in the text you want
Font size: Fill in the size off the font
(mm)
Clicking will automatically fill in as the
text to be added to the part. is used in conjunction with
nesting.
71

When the part that has is nested, the text from the work
order field (nest- part setup) is automatically used as the text on the part
instead of . This allows the part to be stored in the part
directory and used for many different orders.
There is only one type of text used within NC Express. Any other types of
text will need to be imported from the DXF file and tooled interactively with
any of the text marking tools.
4.2.2 Manual Cycling
Manual Cycling gives the user the ability to create or edit cycles. Cycles are
the order in which each contour will be cut by laser. Manual cycling can be
used when a specific order of lasering is needed, or if a cycle created needs to
be rearranged. When using Auto cycling in Autotool it applies an order that
allows for fast cutting. Do not confuse the two functions of manual cycling
and auto cycling. Auto cycling looks for the next closest hole/contour to cut
without passing over cutouts.
Using Manual cycling when there is no cycling applied:
Step 1: Open part cycling.cp. Autotool this part but make sure the create auto
cycle paths is disabled. See previous section about tooling.
Step 2: Go to Tooling menu | select Cycling or click on toolbar.
Step 3: Adding Laser tooling to cycles:
-Click on bottom right circle to highlight, and then right click to add to list.
-Next, click top right circle to highlight, and then right click to add to list.
-Continue adding the rest of the contours to the list in the same fashion.
72

Order of cycle can be changed by selecting a ‘No.’ and clicking SwitchUp.
Step 4: Click Save, and then select Create then click OK.
Cycle has been created.
Remark : It is not so that all geometry from the part have to be in the manual
cycle. If you make a cycle and not all parts are integrated then this means that
you can not predict what geometry that will be cut first the only thing that you
know is that once the first geometry of your cycle is cut that then the whole
cycle will be cut.
You can also create more then one cycle for one part.
Using Manual cycling when there is cycling applied:
Step 1: Open part cycling.cp. Autotool the part with Create Auto Cycle paths
ON !
Step 2: Go to Tooling menu | select Cycling or click on toolbar
You have the same screen as before but now you can load the cycle that has
been created by autotooling into the cyclingbox.
Step 3: Double click on the dashed line from the cycle
73

Before you can start change the cycle you need to click the right mouse button
to confirm.
Now you can start changing the cycle with the switchup button.
Step 4: Select No.004 in the list and push the switchup button until this line is
on top of the list. Now you can see that the geometry that you were cutting as
last is now the geometry that you will cut first.
Step 5 : Click now on Save and you get following box
74

Create
When selecting this option then you are saving the cycle that you just have
made in the manually cycling.
Breaking/Rejoining a Cycle
Break is defined as splitting a cycle into two separate cycles. The following
will demonstrate how to break a cycle into two separate cycles, as well as how
to rejoin them after the fact.
Break the cycle
Step 1: Open cycling from toolbar.
Step 2: Double click on cycle and right click to add to dialog.
Step 3: Select hit No. 3 in the list, click Save, select Break from three items,
and then click OK. Cycle will be split into two different identities.
Rejoin the cycle
Step 4: Double click on one of the two cycles and then right click to add to
the list.
Step 5: After adding the first split cycle, left click on the other cycle and right
click to append to then end of the list.
The order in which the cycles are added back into the cycling dialog will
determine how the cycle will be carried out.
Destroy
Destroying a cycle will delete the cycle all together. Select Destroy when
Save is clicked to destroy a cycle.
Remark- Sync settings means synchronize actions, means force the optimizer to do
the cycle exactly in this way. For FPL this makes no difference, because we have only
one tool. Also Nibble Path Reverse is not for FPL machine.
75

4.2.3 Delete Tooling
Tooling can be deleted from a drawing by selecting tooling and simply delete.
The geometry must be locked before deleting tooling; otherwise geometry
segments would be deleted if selected.
Unlocked geometry- Geometry can be selected
Locked geometry- Geometry will not be selected.
Delete tooling- Delete selected tooling/geometry.
4.2.4 Tooling Modify Features
The following features are within the tooling menu in the Modify menu.
These features can be used to edit some of the smallest or largest details of a
part.
4.2.4.1 Piercing Technology
Piercing Technology is the manual function of changing
the technology for the piercing on a part. As seen to the
right these are the basic piercing type selections used in
NC Express. The way this works is to select a piercing
to be edited, the current piercing type will be
highlighted, select new desired piercing type and then
click apply.
4.2.4.2 Process Technology
Process Technology is the manual function of changing technologies (cutting
types) for a selected contour. All cutting types loaded within
NC Express can be edited through this feature. As seen to
the right these are the basic cutting type selections used in
NC Express. The way this works is to select a contour to be
edited, the current cutting type will be highlighted, select
new desired cutting type and then click apply.
Note- Marking Contour is to be used for a technology
(cutting type) when marking (etching) with laser will be
utilized.
To use Technology go to Tooling menu | Modify → Process
Technology or select from toolbar.
76

4.2.4.3 Tabs
Tabs will give the ability to add microjoints to a contour of a part. When
adding tabs to a part externally or internally they will follow settings from the
Autotooling dialog. Tabs can easily added & deleted on a contour by selecting
Add on dialog and clicking desired position, or to delete select Delete on
dialog then click microjoint (tab) to be removed.
4.2.4.4 Break Laser path
This function is very useful as a manual function
when working with lasers. The break laser path
gives user ability to break a portion of a laser
contour. Lead-ins and Lead-outs are easily applied, as well as
pilot hole (which will be used from Autotool
settings | Path/Leads tab). To utilize this function:
Highlight contour to be broken, right click where
the break will be placed, then the system will
ask ‘Do you want to break path on the
closes point?’ and click Yes.
Laser path is then broken into two separate
laser paths.
4.2.4.5 Leads
Leads function is used to change the lead in settings or to
relocate the lead-ins & lead-outs within a contour.
If we enable the option No relocation then we are able to
modify the lead in / lead out settings without changing
the position.
If we disable this option then we are able to move both
leads, at the same time, to a new location on the same
contour. To use this function click the new location on
the contour where you would like the leads to be placed,
both will be moved.
When we click on the button on the left bottom side we
can change from Lead in to Lead out.
If we put all the values for the lead out to zero then this
means that we won’t create a lead out.
77

When we want to change the lead in type then you first click on the wanted
icon. Then you can zoom in on the contour where you want to change the lead
in and click on the lead of this contour.
Or if you want to replace it at the same time you can click somewhere on the
contour.
4.2.4.6 Direction
Modify direction function gives flexibility to lasering process. This option
will change the direction the laser path will follow on any given contour.
When opened each laser path will have an arc with an arrow through it
towards the center of its contour. To change direction of a laser path, right
click on the laser path that will need direction changed.
4.2.4.7 Loops
Modify loops will add loops to any selected corner. Loops
can be used when working with very tight angled corners,
especially used on external contours. To use this function
select Loops from the menu, then click any corner that
would need a loop applied.
4.2.4.8 Fillets
Fillets are added to a part on the edges of corners, to round
out the corner versus having a sharp edge. To add fillets,
select Fillets from menu. Select Add from dialog, click on
any corner that requires a fillet to be applied. To delete
select Delete from dialog, click unwanted fillets that have
been added.
Note- Delete will not delete fillets that have been saved to the part already.
78

5 NESTING
Proper nesting yields savings in material. The NC Express nesting engine will
automatically layout the most complex part onto your sheets in the most
efficient manner possible using True Shape Nesting. You provide the
information about the sheet, such as size, material type, and thickness; and then
tell it where you want to place the clamps. NC Express will then determine the
optimum placement of the part on that sheet. You can also choose to place
multiple parts on one sheet.
The goal of nesting is to provide an efficient arrangement of shapes within the
context of the machine on which the part is to be produced and the preferences
of the user. To assist the user many parameters are available for modifying the
nesting process. Varying these parameters will significantly affect the outcome.
The following will cover the process of nesting parts to produce NC code.
In order to get started nesting parts the setup of the nest environment is
important. There are a few things that are needed to keep in mind when nesting:
material type according to parts, plate size, amount of parts, and most important
the run folder in which the nest will reside. The run folder is where all the
information for the nested and optimized plate resides, at the same time this is
where the NC code is also created. These folders are very important to keep
organized. You can find these folders in the following directory
C:\fms\ncexpress\(your machine)\work. Each time you want to run a new nest
you can reuse the old folder just by re-nesting or nesting new parts, or you may
create a new run folder. A benefit of having the run folders is the ability to go
back, at any point, and reopen an old nest of parts taking into account the run
folder and parts for that nest still exist.
Reminder- If a part has been nested and you would like to change laser tooling on it
before optimizing and do not want to re-nest the plate; the tooling can be changed
without having to re-nest all parts. Part must be opened to change tooling, and then
nest can be reopened from run folder, and then optimized.
5.1 NC EXPRESS NESTING THEORY
Plate size, material type and thickness, and plate definitions are the main items
required to create a nest. NC Express gives the ability to store this information
to be retrieved automatically when nesting. NC Express, in its entirety, is solely
based on material type and thickness from start (part creation) to finish (NC
file). Multiple plate sizes (raw material) are defined within a database for each
material type and thickness setup within NC Express; in addition to plates
defined, parts are stored within a parts database. When nesting, parts and plates
that have been defined with a specific material type and thickness are only
available within the current nest according to the nest properties. Plate
definitions (clamp information and plate margins) are set accordingly to create a
working area within a given plate.
79

Overall, the ultimate goal is to allow easy setup when creating a nest. The
following three sections will explain the application of features within NC
Express to produce an optimal level of efficiency during the nesting process.
5.1.1 Plates Database
Before nesting, plate information can be stored within a database to be
retrieved when creating nests. Stored plate information, within the Plates
Database, is the actual raw material on hand. Within the Plates Database, a
plate is setup according to dimensions, quantity on hand, material type and
thickness, priority as well as more useful information. When a nest is created,
NC Express searches the Plates Database for stored plate information
containing the nest’s material type and thickness. If a plate(s) is found that
shares the same material type and thickness, the plate(s) is entered into the
Nest dialog plate list automatically.
Additional information is available for use within the plate setup- Utilization,
Cost, CS storage address. Utilization percentage is entered to display the
desired utilization value. Cost is the cost of a single sheet, once parts are
nested material used for the part is calculated from the cost defined. If a CS
storage tower is present within the Finn-Power system, CS storage address can
be stored for each plate to be output within the code accordingly; this allows
quicker and less hassle program loading at the machine. Finally, if a plate is
stored within the Plates Database as a remnant may be defined here.
Plates defined within the Plates Database do not actually need to be on hand
(raw material). Plates Database can be used to load plate sizes for material
types and thickness’ that are typically used. This feature is used to save time
when creating nests.
80

5.1.2 Parts Database
When parts are created within NC Express, necessary information is stored
within the CP file. Therefore, each separate part has it’s own properties which
are used throughout the entire system. The most important information stored
within a part for nesting is the material type and thickness, part rotations, and
turret used. Why this information is important is to allow for quick part
selection and processing, meaning that all three of these pieces of information
can be sorted or modified when selecting parts in nesting.
In addition to the three items mentioned, more items are available to help
select parts. Within the nest dialog information from the Parts Database is
viewable. The following items can be viewed: part name, file location, sorting
type and address, turret used, slug hole (laser) and revision level. Part name,
sorting device, turret used and slug hole can be sorted within the Parts
Database list to allow grouping of similar parts. These items are used to save
time when nesting parts.
5.2 CREATING A NEST
When creating a nest there are a few parameters that are needed to set the
properties of the nest: Run ID (can be name or number) and Material type and
thickness.
Creating the nest properties:
Start by going to File menu | New → select Nest.
81

5.2.1 Run ID
Run number is the ID of the nest; a folder named as the run number is created
and can be found in the following directory C:\fms\ncexpress\(your
machine)\work. The run folder is where all plate information for the nested
and optimized part(s) resides. These folders are very important to keep
organized. These folders are stored on the local PC of the NC Express setup.
The folder can be named with alphanumeric values up to 18 characters.
A benefit of having the run folders is the ability to go back, at any point, and
reopen an old nest of parts using the same exact environment that was set at
time of creation.
Edit Run ID to create folder in background to store information pertaining to
nest. Select Material type (code) and Thickness by highlighting them. Click
OK.
If there is already a folder that exists with that runs id there will be a warning
message that appears on the screen (shown below).
Click YES to overwrite the folders information.
Click NO and NceXpress will look for the next free number.
(Note- You may switch back to an older run folder by going to File menu | Open
Plate, then select correct run folder to open old nest.)
5.2.1.1 Re-using/Overwriting Run Folders (Dynamic Nesting)
In the case that dynamic nests are created the reason to save old nests is very
minimal. Dynamic nesting is the ability to create nests on the fly. A run
folder is created and parts are scheduled as needed and the nest is created to
liking. When dynamic nests are used the use of old run folders is very
minimal, meaning that run numbers can be re-used or overwritten. To
overwrite a run folder all that is done is the old run folder name is entered as
the run number when creating a new nest. When OK is clicked a warning
message will appear and ask if it is okay to overwrite the old folder.
82

5.2.1.2 Keeping old Run Folders (Static Nests)
In the case that nests that have been created in the past and will be ran over
and over at the machine, this means that static nesting will be utilized and old
run folders will need to be saved. Run folders are perfect for static nests, but
the only thing that is needed is to remember which run folder is the actual old
nest. This can be done two ways- rename the run folder or write down the run
number in a log.
The actual run number folder can be renamed within the windows
environment to either a customer name or Order ID. When adding this folder
back into NC Express, the folder will need to be renamed back to it’s original
run number ID. The original ID of the run folder can be found by opening the
renamed folder and viewing the .nst file name, the first three numbers are
always the original run folder name.
A log can also be kept to track run numbers per customer nest or Order ID.
5.3 NESTING PARTS
To nest parts the nest dialog must be opened.
The settings can be found back in the AppendixB Nest parameters
Go to Process menu | select Nest or click on toolbar.
83

5.3.1 Global Parameters
Plate definitions are defined within the nest dialog in the Global Parameters
tab. Clamp information and plate margins are used to define the working area
of the selected plate(s).
5.3.1.1 Plate Margins
Setting the plate margins is in essence setting the working area within the
plate. Size of plate margins generally varies from company to company, but
never is too small to where parts are very close to the plate edge. Parts being
removed too close to plate edge will create a flimsy skeleton, which can cause
problems at the machine or even cause problems for parts.
Plate margins can be set to a default value by clicking on ‘Use as default’
button on bottom left of dialog.
5.3.1.2 Nesting Theory Summary
Overall, the theory of nesting is to push the user to reach a state of automation
when creating nests. All together, the items that are used to make a nest work
correctly are easy to set or edit. Plates database stores information for plates
and can be done in a one-time setup with many plates, only modifying
quantities of plates or adding a new material type or thickness if needed. Parts
database is used to sort the parts that have been created and stored in one or
more part directories, allows easy access to part information. Plate definitions
can be either used automatically or modified to liking, either way they are easy
to set.
Once the above items have been setup the ability to nest parts should be an
easy task. The rest of the settings within the nest dialog are available to
modify the outcome of a nest.
5.3.1.3 Part Separation
Part separation is set both in the X-axis and the Y-axis. The values used
within the nest dialog will be used to add spacing between tooling on parts.
When a part is tooled within NC Express the geometry is no longer the outside
of the part, the nest engine considers the outside edge of the tooling is to be
the actual outside perimeter of the part. Within NC Express this is termed as
“tooling envelope”. When tools are placed on the outside of the part, the
amount of distance the tool is outside the external geometry of the part forms
this imaginary envelope (window) around the outside of the part. For FPL we
talk here about the beam width.
This allows the parts to be nested as close as possible, but still not allowing
tools to overlap onto other parts. True shape nesting is still used depending on
the shape of the parts or tools used.
84

5.3.1.4 Nest Accuracy
Adjustments made to nest accuracy edit the step size for nesting parts. The
value is an adjustment made by the end user. Increasing the accuracy will
allow the nest engine to produce a nest much faster; also, using a large value,
the part spacing may be larger than actual values entered. Decreasing the
accuracy will make the nest engine run much slower, but will increase the
potential for a higher quality nest. To achieve acceptable nest accuracy the
end user should experiment with this value.
5.3.1.5 Nest Direction
Nest Direction determines the starting position of placement of parts in a
sequence. When nesting parts, the parts are placed on the plate one at a time.
So, the nest direction position chosen within the dialog will determine the
starting point of the nest and work its way from the specified location to fill
out the plate. For example, if upper left is chosen the first part will be placed
in the upper left corner of the plate and will fill out the rest of the sheet from
there.
Typically for all Finn-Power machines upper left corner is used because this is
the side closest to the sheet removal when plate is being processed at the
machine. Other directions can be utilized to find a more suitable nest
outcome.
5.3.1.6 Grid Nesting
Grid Nesting is used to nest parts in a grid like manner. The parts are arranged
within the plate in a uniform fashion. When using this option the part
quantities may change within the plate. Grid Nesting will allow for a better
looking nest and is generally well suited for use with square or rectangular
parts.
5.3.1.7 Nest by Work Order
If parts are nested using a work order number the parts can be sorted within
the plate(s) by the work order entered. Work order’s can be used in nesting by
either entering the work order when adding the part to the part list or by
utilizing Orders database.
5.3.1.8 Nest in Holes
Within NC Express’ nesting engine Nest in Holes allows parts to be nested
within a cutout of another part. If a nest has small parts that will be nested
along with large parts with cutouts big enough for the small parts to fit, Nest in
Holes activated will nest the small parts within the cutouts. Requirement of
Nest in Holes is that the cutout is to be microjointed (tabbed) into place
85

5.3.2 Part list
Part List will determine which and how many parts will be nested onto the
plate(s). Few other options to change parameters of nesting included in part
list.
On the left side you find back all the parts that are in the part database for that
kind of material and that thickness.
With the button you can move the parts to Scheduled parts, this means that
those parts will be nested.
If the parts that you want to nest are not in the parts database (in the directory
fms\ncexpress\(your machine)\partdir) then you can change this by clicking on
the Parts Browse button. Then you get the open dialog.
86

Modify
Once the parts are in the Scheduled section we can edit the properties of each
part by double clicking on the part or by selecting the part and press on the
Modify button. Following dialog will be opened :
Name- Displays name of part selected.
Work order- Work order number from the orders database.
Due date- Set a due date for part being nested.
Quantity- Amount of parts that will be nested in current nest.
Priority- (Values 0-9, 9=highest) Set priority, similar to tools, parts
with higher priority will be nested earlier in the nest.
Grid nesting- Turn on or off by placing check mark. Depicts whether
or not grid nesting will be turned on for part.
Part orientation-
Initial rotation- Rotates parts automatically in nest to value
entered (0°-360°). Set to default changes Initial
rotation back to original part configuration.
Allowed rotations- Sets parts to give ability to rotate freely in
the nest.
Delete
Select part to be removed from nest and click Delete, part will be removed
from current nest.
Due date
Due date set to current date when creating a new nest. When opening an old
nest Due date will remain the same as the date it was nested.
87

5.3.3 Plate list
In the plate list we get the plates out of the plate database for that kind of
material and that thickness that we have selected for the nest.
Switch Up
Highlight plate, click Switch Up to move plate a single line at a time. Top
plate is used for nest.
New
Clicking new will bring up Plate record screen. This plate that you create here
will not be saved into the Plate Database. This plate is only once used for this
nesting. When you will create a new nest you will not find back this plate size.
Plate ID- Enter name of plate.
Reserved- Quantity of plates being used.
Cost per sheet- Input price to be calculated in post process.
X and Y- Top line equals X coordinate line on right equals Y
coordinate.
88

Modify…
Highlight plate, click Modify to edit plate.
Delete
Highlight plate, click Delete to remove plate from current nest.
Square last plate
Last plate in nest squares all parts in order to use maximum utilization for
parts nested.
Use in listed order
This option will make the nesting on the plates like they are put in the list.
This means if we have 3 times a sheet of 3000x1500 and 6 times a sheet of
2000x1000 and 1 time a sheet of 2500x1250 then we will get the nest in the
same order. (if all plates are needed)
Use smallest
With this option the nest will be made on the smallest plate out of the list.
Use only the first plate size
With the switch up button we can put any plate on top of the list and then
NceXpress will use this plate to make the nest.
Set plate limit
Sets a limit of nest patterns NC Express will create when nesting parts.
Example of this being used is if you wanted to generate only nest pattern to
run out a large amount of parts that need to be nested. Activate this function
and enter a value of 1 to create only one nest pattern. A possibility of this
being used when making a static nest and the additional sheet is then
eliminated.
5.4 NESTING EXAMPLE
Create a nest with run number 100 in AluMg3 with thickness 2mm.
Step 1: Click on toolbar.
Step 2: Go to Part list tab, add a part to scheduled parts
(alu_2mm_medium)
Step 2a: Edit quantity of parts (110)
Step 2b: Enable allowed rotation for both.
Step 3: Go to Plate list tab,
Step 3a: Move plate 2000x1000 to top of list by highlighting the plate and click
Switch Up until on the top of the list.
Step 3b: Make sure the right option is set to use the selected plate for the
nesting.
89

Step 4: Go to Global parameters tab
Step 4a: Edit part separation- 5mm
Step 4b: Direction- top left
Step 4c: Beam width- 0.3mm
Step 4d: Margins all at 10mm
Step 4e: Commonline : no
Step 5: Click OK.
Step 6: Put on the option grid nesting
Step 7: Try now different direction angles for the nesting
90

5.5 MODIFYING PART’S/TOOLING (FOR PARTS THAT ARE
ALREADY NESTED)
If a part within a nest requires a change to tooling and re-nesting is undesired;
the tooling can be changed without having to re-nest at all. The part can be
opened to modify the tooling. Once the changes are saved to the part, the nest
(*.nst file) can be re-opened from the run folder to be processed. When the nest
is opened from the run folder it loads (reads) the CP file from the default part
directory. If the part(s) doesn’t exist in the default part directory NC Express
will issue a warning, and the default part directory should be checked.
Nests can only utilize this function. Optimized files will need to be re-opened
from the nest to change tooling.
91

5.6 PRESHEARED PLATE NESTING
NC Express allows the user to nest a part onto a plate, which shares many of the
same dimensions. For nesting Preshear, a part is tooled through Autotool (see
Preshear Autotool) and then ready for optimization directly after. When
programming presheared parts through NC Express there is no nesting involved
the part goes directly to presheared optimization (See Presheared Optimization).
5.7 INTERACTIVE NESTING
After nesting process is completed, the first of the nested plates is displayed on
the screen and is immediately available for interactive editing. Selected parts
can be moved around, deleted or copied. If more then one nested plate was
created, parts can be copied and pasted between plates. New parts can be added
to the nest via the File menu | select Add Part menu selection. The full list of
nested plates is displayed in the Nest Explorer dialog.
At the end of interactive editing, user will save the modified nest by going to
File menu | select Save. At this point the system will check the nest for part and
plate boundary violations and if necessary issues a warning. After a modified
plate is saved, the system automatically updates the nest report.
Interactive Nesting features:
Drag and drop parts within plate
Copy parts from plate to plate or within plate
Move selected by giving the X an Y values
Add tooled parts from Part directory
5.7.1 Drag and Drop Parts
Parts can simply be selected in nesting screen and moved around the plate
according to users needs. Parts will only be able to be moved within
parameters set for plate margins and clamp settings. If moved in illegal area
an error will occur. Save after moving parts. Parts cannot be rotated manually
in the nest because tooling may not be able to be used in that orientation.
5.7.2 Copy Parts
When viewing a nest of parts, parts can be copied either within a nest or from
plate to plate. There are two ways to copy parts within the plate. First, is to
select and copy and the second is to use the Move Selected feature.
To copy a part within a plate select the part to be copied, hold down control
(ctrl) key, and drag part to desired location. Save after copying. To copy to
another plate highlight part to be copied, select copy from either toolbar or edit
menu, open destination plate by double clicking in Nest Explorer. To paste
part, select paste and click in plate desired location. Once part has been pasted
in nest it may be moved to fit where needed. Save after copying.
Note- Using shift + ctl key at the same time when copying a part will allow the part
to be moved only in horizontal or vertical movement (0°, 90°, 180°, and 270°)
92

5.7.2.1 Move Selected
Move selected allows parts to be moved using an exact value, either absolute
or relative value. When copying parts Keep selection must be enabled to
actually copy the part. Click Specify to enter an X and Y value. Once the X
or Y value are entered, depending on which way the part will be moved, click
Move to move part. Save after moving part.
5.7.3 Add Part
Add part gives ability to add part manually to an existing nest. Open plate in
which a part will be added, go to File menu | select Add Part, and then select
tooled part from Partdir. When part is added to nest it is added outside the
bottom left corner of the plate. Part can be moved to desired location, then
copied however many times needed. Save nest after adding part.
93

6 OPTIMIZATION
In a typical environment, you can use the automatic Optimizer. For more
complex parts, or if you want greater control, you can choose to interactively
optimize the parts. Once parts have been nested onto a plate in NC Express they
are ready to be run through the Optimizer. This step determines the most
efficient path for the machine to process and produce all parts on the plate. This
section of the program is the most important because it is where you will be
programming the laser to be most efficient. The following section will cover
items including Automatic optimizing, and Interactive optimizing.
Detailed description of settings for Automatic Optimizer can be found in
Appendix C.
Automatic Optimizer
Interactive Optimizer
6.1 AUTOMATIC LASER OPTIMIZER
Parts will be nested onto a plate and must be optimized to run NC code. The
automatic optimizer will create packages of tooling which will give the best path
for the tooling to be used. Changing settings within Automatic Optimizer will
drastically change the outcome of the final result.
6.1.1 Exercise- Optimization
The following exercise will demonstrate the use of Automatic Optimizer. The
nested plate from exercise in nesting will be used for this exercise. This
exercise will demonstrate how to adjust settings in the automatic optimizer
create different outcomes for this nest.
First part of the exercise settings will be adjusted to create a finished nest
where the parts will be cut in a horizontal fashion from left to right and right to
left order stopping in the top right of the sheet. The second part of the
exercise will optimize parts vertically finishing in the top right then the bottom
right of the sheet.
94

Step 1: Nest Drawing1.cp with a quantity of 45 on a sheet size of 2000mm x
1000mm.
Step 2: Open Optimizer by going to Process menu | select Optimizer or click
on the toolbar.
Cutting Destination- Destination point of the last part of the nest. Select the
corner in which you want the machine operation to terminate.
Swath- Creates zones either horizontally or vertically. Choose to cut in
horizontal or vertical direction.
95

Generate-
Crop line- Create a laser path to the right of parts nested. Used to cut off
unused material.
Outside lead- Creates leads on the outside of parts, if not already created.
Inside lead- Creates
leads on inside contours, if not already created.
Smooth Cutting- Generates a smooth path with limited axis moving.
Calculates
the end point of cut and start point of next cut then make smooth
transition to next cut.
Clamps No Fly Zone- If we enable this option and we put the size to 100 then
this
means that the cutting head will be lifted straight up with ping-pong
disable when we ‘fly’ over parts with a X and/or Y size smaller than 100mm.
Reason for this function is that we can eliminate the danger to hit a part which
is possibly fallen halfway between the slats when we start the ping-pong
motion. Recommended size is 100mm!
Also new is that we will move around the clamps with the head up.
For
example we stop cutting on the left side of a clamp and we need to start a
new contour on the right side of the clamp, both coordinates below the
Y
value of the clamp safety area, we will now at the end of the 1 st contour lift the
head straight up, move to Y of clamp safety, move to the new X and then
move down to the Y value of the next contour start point. Clamp safety area’s
are set in the machine set-up
Prepierce – Adds prepierce cut
to lead-ins (not for FPL)
Use G41/G42 command in normal cutting – activates the
beam radius
compensation
on machine side.
Head down- (Used only in high speed mode) Setting will tell optimizer
how long the head can be down after cutting until it must be picked up.
Common Line-
T hese parameters are explained in the commonline exercise .
Scrap cut- (Skeleton cutting) Create scrap cutting for parts. Will create a
grid
outside the parts to remove the scrap. X and Y coordinates will tell the
optimizer where exactly you would like this grid to be created.
Post cutting- outputs the scrap cuts to be cut after all parts have been cutout.
96

Temporary High Temperature Area - This option is a
solution to optimize the heat dissipation during the
cutting process of thick materials.
With these parameters, which are different
for each kind
of material and thickness, we are able to minimize the
influence which the heating up of the material has on the
cutting process.
When
we cut out a contour with the laser beam, we know
that the material is warming up during this process.
(powerpoint Heat Dissipation).
The area that is warming up around
this contour we call :
THTA (Temporary High Temperature Area).
To have an optimal cutting process this area and
its boundaries are unaccesable
for any cutting operations until it has cooled down.
We can do this already when optimising the cycle from
the nesting but these
parameters will calculate how long the area around the contour is overheated.
Delay Before Growth – (sec) This
parameter tells us when this area will start to
heat up. In most cases this parameter will be
zero because at the moment we activate the
beam and start to cut the material, the
material is already warming up.
Offset
Growth Speed – (mm/sec) This is
the speed with which the Temporary High
Temperature Area grows.This depends on
the kind of material and the thickness.
Maximum
Offset Size – (mm) this is the max. distance around the contour that
will warm up during the cutting. This value will determine the maximum size of
the Temporary High Temperature Area.
Once the boundaries of this area have been
reached the material will start to cool
down
Delay
Before Fall – (sec) This parameter will tell us when the temporary high
temperature area will start to shrink, to cool down.
Offset Fall Speed – (mm/sec) This is the speed with which the warmed up area
shrinks.
This parameter
allows us to calculate how long it will take until the area around
the cut part is again safe for usage.
Max
Delay in Post – (sec) When jumping around from contour to contour to
avoid these High Temperature Areas there can be a moment where we have to
wait until everything is cooled down.This parameter allows us to set the
maximum waiting time.
97

Step 3: Setting optimizer to do horizontal cutting and ending in top right
Step 4: Click OK.
Step
5: Go back to optimizer and put Swath to Vertical. Click OK
START
Step
6: View simulation of parts being cut.
HORIZONTAL
VERTICAL
START
98
END
END

Open simulator by going to Process menu | select Simulator
C lick to start simulation.
Increase speed (move speed bar to the right or click F until increased)
Will move to next part.
Simulator
will show parts being processed from both sides of plate in snake
like motion horizontally finishing in top right corner.
Step
7: Close Simulator.
6.1.2 Exercise- Optimization (scrap cutting and crop line)
The following will demonstrate how scrap cutting is applied to a nest, as well
as adding a crop line to end of the parts. The scrap cut will cut the remnant of
the skeleton into sections for ease of handling. Crop line will be used for plate
not completely filled with parts.
Step
1: Use same nest as last exercise
Step 2: Optimizer settings:
99

The outcome of the optimized nest will have vertical scrap cuts throughout the
plate 500mm apart to split skeleton into section. Selecting Post cutting will
allow skeleton scrap cutting to be done after all parts are cut.
Step
3: Go back to optimizer and make now also a scrap cut in Y direction
for each 250mm
This
will be the optimized nest :
100

Step
4: Go back to Nesting and change the quantity of the nested parts to 10.
And make the nesting direction in the left down corner.
Step
5: Go back to Optimizer and enable the crop line (disable all scrap
cutting)
The outcome
of the optimized plate will cut the remnant from the skeleton
allowing the rest of the sheet to be used for another job.
101

6.2 INTERACTIVE OPTIMIZER
Interactive Optimizer gives user freedom to manually manipulate the optimized
data. This function can be found by going to Process menu | Interactive
Optimizer. Using Interactive Optimizer a user can delete a part from a nest
and/or reorganize order processing parts. Reorganizing parts can either reverse
order or set a customized order of parts processed.
How Interactive Optimizer works is that NC Express creates tooling packages to
be placed within the Interactive Optimizer. These tooling packages can be seen
as soon as the Interactive Optimizer is opened (as seen on next page showing
tool name). A tooling package is similar to a folder in your Windows system
holding a specific order of parts for the current plate being viewed. When a
tooling package is opened (by double clicking on a tool package) all parts are
shown in the current order, as they will be done at the machine. Interactive
Optimizer is giving the user the freedom to alter the order the laser will be
making. Interactive Optimizer comes in two forms:
Modify
View Only
6.2.1 Modify
Functions of Interactive Optimizer can either be done directly in the dialog
box or by graphic selection mode. Switching hits up a row, move selected hits
to bottom, Reverse hit orders or when using graphic mode selecting the
specific tool hit directly and changing hit order on the screen are many uses of
the Interactive Optimizer.
.
The following exercise will use the same optimized file from last exercise
(Optimizing). This exercise of Hits only is to demonstrate how to utilize the
feature of Interactive Optimizing parts. This will simply demonstrate how hits
are moved around to change the order.
6.2.2 View Only
View Only is similar to Modify but doesn’t have the capabilities to edit the
tooling packages. View Only is used to view motions of the carriage between
tooling hits (Head up), repositions (pad placement), and sorting. View Only is
used in the same fashion as Modify to view tooling packages, but remember it
is to just view motions throughout the operation. Below are definitions of
terms:
102

6.2.3 Exercise- Interactive Optimizer
The following exercise will demonstrate the ability to edit the order the parts
will be processed at the machine. The following exercise will reverse the
order of parts being processed. The parts will be processed from the top and
finish at the bottom. The process will be done two ways: graphic mode and
non-graphic mode.
6.2.3.1 Modify (without Graphic Mode)
Step 1: Open optimized file that we have last created with the cropline.
Step 2: Go to Process menu | Interactive Optimizer → Modify.
103

Step 3: Double click on laser (No. 1):
Now you can start changing the sequence with the buttons :
Move to Bottom :
Select the first line and click on the button Move to Bottom. You can see that
the first part will now be cut as the last part.
Switch Up :
Select the last line and click on the button Switch Up. Select then the fourth
line and switch up again. Do this until the last part is again the first part to be
cut.
Reverse :
Select two lines with the Ctrl button and click then on the reverse button. You
can see that the two selected parts have switched places.
Split :
This button will split the sequence into different packages. As you could see
when we opened the interactive optimizer there were two packages : Laser and
cropline.
If you now select for example line 3 and you click on the split button then you
will create a second package Laser.
If you now click on the button Next Package you can see that there are three
packages :
104

Step 4: Click Close and Yes to confirm changes.
Modify (Graphic Mode)
Step 1: Rre-run Automatic optimizer to reset original optimized nest.
Step 2: Open Modify and double click on laser tool package.
Step 3: Select Graphic Mode.
-Select Part 5 on the nesting and there will be a dialog that appears:
105

Chosen No.- displays the part chosen.
After No.- displays where in the screen order the part will be placed.
Don’t show this…- enables the ability to click each part thereafter After No.
in a progressive order.
Step 4: Leave zero (0) for After No.
Click then on part 5 and leave the After No. set at 1
And go on until you have reversed the whole cycle
Step 5: Click Close and then Yes to confirm changes.
6.3 BATCH OPTIMIZATION (AUTO-PROCESSING MULTIPLE
SHEETS)
In the case that a nest of multiple parts, or even single parts, has created multiple
sheets it may be time consuming to go through and process each plate if they
will be processed the same for each. NC Express offers the ability to process all
sheets nested (that are listed in the Nest Explorer) with a click of a button.
Batch Optimization requires a few items to be setup as well as options to be set
within the Optimizer.
Options to be set: Generate report PDF file…(optional), Print report
automatically after… Show report picture with tooling (optional). (Settings
menu | Options)
Post Processing: Set the correct output folder for NC, fms, and report files.
To start: Make sure that settings above are set correctly.
Step 1: Create a nest that will have more than one sheet within the Nest
Explorer.
Step 2: Setup Optimizer with desired options then click ‘Use as default’.
Step 3: Highlight all the sheets (999001-999004) within the Nest Explorer.
106

Step 4: Click Process on the Nest Explorer. This will allow all plates to be
optimized and then post-processed automatically with a click of a button.
Step 5: When finished and everything has optimized and post processed
correctly the Status will display ‘Post Processed’. The plates are ready to be
Accepted. Click Accept and the reports will be printed automatically as well as
plate quantities (used for the sheets within the Nest Explorer) will be subtracted
from the Plates Database.
Note- If there were any errors when optimizing or post processing the selected sheets, a
log is displayed showing the sheet name as well as the error. If the Plates Database
doesn’t have material loaded within for the particular nest an error message will
appear stating that the material is not loaded within the Plates Database.
Remember- This process can be done on a portion of the sheets listed. It doesn’t have
to be done for all sheets within the Nest Explorer. Meaning that certain sheets can be
selected within the Nest Explorer.
The ability to Batch Optimize nests is an option within the software to increase
the level of productivity when creating nests within NC Express.
107

7 CREATE NC CODE
Once the steps of tooling a part, nesting, and optimizing have been done the
final optimized plate will be ready to simulate and create NC Code. The
following section will inform how to simulate the actions of tools throughout a
plate and create NC code.
7.1 SIMULATION
Open optimized file from the last exercise using Interactive zones. Run
simulator by clicking on the toolbar.
Speed is increased by moving speed bar, or
by pressing F on keyboard. Speed is
decreased by moving speed bar to the left,
or by pressing S on keyboard.
Run simulator on the optimized file to see
how the tooling is being punched and laser is cutting out parts to be removed.
7.2 NC CODE
The files is ready to create
code. With the optimized plate
on the screen press on the
following button on the toolbar
Post processing dialog will
appear. Here you will see the
Tech tables, these are used to
output the correct value for
each technology used within
the software. The technology
values must match what is
loaded within the machine
database. Also, the name of
the NC file that will be
prepared and NC file location
to save to alternate location. Click Save as to save NC file to any location on
either the network or local hard drive. This is useful to store newly prepared NC
files for operator to use.
108

The Parameters tab allows for editing settings to be output for cutting. These
values are easily edited to suit the material type and thickness. Once the code is
created any values entered within are saved in the Cam.mdb for the current
material type and thickness to be used again.
In Appendix D you can find a detailed description of the settings.
Parameters set for each material type and thickness are originally set by Finn-
Power from experienced user. These values generally do not need to be
edited.
Focal length and Focus point
These are the parameters from the cutting lens that come from the database
Cutting head mode
The quickness of response off the sensor in the cutting head.
1=fast motion of the cutting head
2=slow motion of the cutting head
Acceleration
[10..100%] The acceleration setting during the processing. The percent value
from maximum vector acceleration
Smooth pos
[10..100%] The speed and acceleration of the positioning. The percent value
from maximum vector speed and acceleration
109

Laser beam selection
The different setups for laser beam diameter and focal length compensation
Foil processing
When there is a foil on the plate we have to activate the foil cutting. Then put
this parameter on 1. This can not be done in high speed cutting.
Sheet probing
When we want to do a sheet probing (determine how the plate is place on the
table) then we have to activate this parameter by putting to 1.
When we have a automatic loading table or when we put the plate in our
clamps then this is not necessary to do.
Prepunch probing
If we put a prepunched plate into the machine then we have to activate this
parameter so it will measure the prepunched holes or other contours before
starting the cutting.
Focus pierce
Here we can do a repositioning of the lens while piercing. This is only for
thick material and the values will be filled in automatically
Cutting head position
[mm]The cutting head distance from sheet to upward direction during
positioning
Cutting head position type
0=reclinear cutting head motion during positioning,
1=Ping-Pong cutting head motion during positioning
Corner function
This parameter will be activated automatically when it is necessary. This
corner pulse will make it able that the corners are cut nice, just before a corner
we will cut slower and with pulses.
Output m01
After every part there will be generated a code that will make the laser stop.
Nozzle calibration
The calibaration of the distance control sensor in the beginning of the NCprogram
Scrap cut parameters
When we have a cropline then on 5mm before the end off a plate the cutting
head will disable his sensor, go 3mm outside the plate starts cutting and after
5mm activates the sensor again goes to the other side off the plate and there
5mm before the edge the sensor will be disabled again to go 3mm outside the
plate.
110

7.3 REPORTS
When NC code is generated reports are created to inform programmer what was
done in the nest. The report shows all information pertaining to one plate nested.
The following information is included in the report: machine tool, nest ID/nc
code file name, Material type and thickness, Sheet utilization, picture of parts
nested, part order identification, and time estimation info. Programmer will
have the option to export this report as an HTML file, PDF, or keep as text
format.
Reports can easily change between efficiency reports, time reports, or entire
report of nest.
111

8 HIGH SPEED – NORMAL CUTTING MODE
When you go to Settings | Machine parameters | Environment
Then you can see next to the material type and thickness the HSP type and the
default cutting mode.
This is for Mild Steel 1mm
This is for Mild steel 2mm
This is for Mild steel 5mm
112

As you can see we can have different HSP types :
And two different cutting modes :
8.1 HIGH SPEED CUTTING MODE
High speed cutting mode will be default selected for all materials that are cut
with Nitrogen with a thickness from 0 – 3mm.
8.1.1 High speed cutting mode for 0mm – 1.5mm
In the thickness from 0mm to 1.5mm the HSP type will be 2.
This means: allow tech 5 and multiple technologies.
When we autotool a part in these thickness then we get next screen :
113

On the path/leads tab-page we can see that all contour types will be used
according to the dimensions of the contours.
So after tooling our part can look like this :
We use the High speed technology
number 5 and all the other technologies
on one and the same part.
The High speed technology uses a higher
speed then the other technologies but also
more gas pressure.
For example in mild steel 1mm we are
cutting at 18m/min with the large contour
technology and with the new high speed
technology this will be at 25m/min.
For the smaller contours we will use the
Large, medium or small contour
technology.
114

8.1.2 High speed cutting mode for 1.5mm – 3mm
In the thickness from 1.5mm to 3mm the HSP type will be 3.
This means: allow only tech 5 for High speed cutting.
When we autotool a part in these thickness then we get next screen :
On the path/leads tab-page we can see that only the High speed contour type is
enabled:
We use only High speed technology
number 5 on the same part.
In this material (1.5mm until 3mm) the
High speed technology does not uses a
higher speed then the large contour
technology but it allows us to cut the part
without piercing.
115

So after tooling our part can look like this :
8.2 NORMAL CUTTING MODE
The Normal cutting mode will be default selected for all materials that are cut
with Nitrogen with a thickness from 3.5mm and higher and for all materials cut
with Oxygen.
8.2.1 Normal cutting mode for 3.5mm and higher (and O2)
In the thickness from 3.5mm and higher the HSP type will be 0.
This means: No High speed cutting allowed.
When we autotool a part in these thickness then we get next screen :
116

On the path/leads tab-page we can see that only the High speed contour type is
disabled:
So after tooling our part can look like this :
We don’t use the High speed technology
number 5 in these thickness anymore.
117

8.2.2 Normal cutting mode for 0mm – 3mm
The
cutting mode for materials that are cut with Nitrogen and have a thickness
between 0mm and 3mm uses the High speed cutting mode by default.
But if necessary we can also make these parts in normal cutting mode.
This means that we will not use the High Speed technology on the parts in these
thin materials.
When
you go to
part.
autotooling for the part you can change the cutting mode for the
Select the normal cutting mode to tool
the part. This means that we will not use
the high speed technology nr 5.
On the path/leads tab-page we can see that only the High speed contour type is
disabled:
118

This means that we can tool parts from 0 until 3mm in High speed cutting mode
(default selected) or in Normal cutting mode.
So this means on one plate we can have parts that we cut with the High speed
mode and the high speed technology or parts with the Normal cutting mode.
9 ORDERS MANAGEMENT SYSTEM (MRP NESTING)
The Orders Management System (OMS) is a feature within NC Express that
allows a user to process production requirements in a more accurate and
efficient manner. OMS (Orders Database) can be used to nest parts from text
file created that contains all the part information to be nested. By having an
order file of parts, the file can be imported into the Orders Database to be nested
instead of manually adding each part to the nest dialog each time a nest needs to
be created for an order. Once an order is imported and ran from the OMS run
folders pertaining to material type and thickness are created automatically. This
also allows integration with an MRP system to achieve more accurate and
efficient nesting of parts.
The following section will explore the Database Orders dialog
as well as how to
operate.
9.1
DATABASE ORDERS DIALOG
Go
to Database menu | select Orders. The Database Orders dialog will be
displayed.
Tab Selection
Active Tab: Displays ordered parts as well as unfinished parts
ordered. If parts were not completely nested the remaining orders will
stay in the active side until nested.
Completed Tab: Once ordered parts are nested they will need to be
optimized and post processed in order to be ‘completed’. After the
parts are optimized and post processed the nests will need to be
Accepted through the Nest Explorer. The acceptance will move parts
that are active to the ‘Completed’ tab.
119

Sorting
Machine combo-box: Allows user to select the machine that will be used.
By selecting the machine from the Machine combo-box, orders for the
selected machine, active or completed, will be displayed in either the Active or
Completed grid.
Sort by:
General
o Order: Sort part orders by Order ID.
o Assembly: Sort part orders by assembly name (kit).
o Material: Sort part orders by material and thickness.
o Machine: Sort part orders by NC Express machine name.
Add…:
Add a new part to the order. A New Order dialog box will be
displayed. (See New Order dialog picture below)
Edit…: Opens the selected part for editing. (Edit dialog will be displayed.
similar
to the New Order dialog)
Re move: Removes the selected part(s) from the order. The check box for
the part(s)
must be checked.
Export…:
Exports the orders in the list to an XML or ASCII-file (text
file). Import…: Imports a part order file from an XML or ASCII-file (text
file).
Nesting [x]…: Transfers the selected part(s) to nesting. Multiple items
can be selected by clicking [x] column,
or by clicking the white area of the
first f ield li sted (ex. if sorted by Order click on the order name under the
Order fi eld) . All the rows having an [x]-check will be nested.
If the orders
are of the dissimilar material or are going to different machine tools
multiple
run folders
will automatically be created for each type.
Close: Closes the dialog box and saves any changes that have been made.
120

9.2 ADDING/MODIFYING PARTS IN ORDERS DATABASE
Orders Database is setup to integrate with an MRP system in order to process
ordered
parts by importing a text file. The Orders Database also gives the
opt ion to manually add parts to be ordered. When the Add button is clicked the
New Order dialog will be displayed, which allows for parts to be added one by
one. Or a part is selected and Edit button is clicked the Edit Order dialog will be
displayed.
The information below describes the settings that appear in both of
the dialogs (both dialogs have the same information).
Header
Order name: Order ID for the part or parts that are to be nested.
Machine tool: Select the machine that will be used to nest the part(s)
ordered.
Assembly: Enter a name for an assembly name. A previous entered
assembly name can be selected from the drop down. Assembly name can
be used to sort parts belonging to the same assembly (kit) together. This
field can be left empty.
Part name: Type in a part name or select the part by pressing ‘Select…’button.
Parts being nested in this fashion must reside in the default part
directory defined within the environment.
Select: Allows user to select a part file. Order can’t created if the part file
doesn’t exist. When the Select button is clicked, depending on the Option
button selected in the Additional Information frame, the Open dialog will
display: cp files, dxf files, or scripting files. (ex. if ‘Use existing part file’
is selected within Additional Information [bottom right corner of dialog]
only the .cp files will be displayed within the Open dialog.)
Amount
Ordered quantity: The original ordered quantity of the parts.
Nested quantity: Quantity of parts nested. The amount of parts that are
accepted with ‘Accept’ button in ‘Nest explorer’.
Manufactured quantity: The real manufactured quantity. This field will
display zero if there is no feedback from PowerLink.
Extra parts allowed: This is the amount of extra parts allowed to
manufacture if using part as a filler. Increasing this
value will, in turn, increase the sheet utilization
percentage.
121

Scheduling
Due date: Displays a calendar
dialog allowing user to set the due date of
this order.
Manufacturing window: Manufacturing window tells how many days
before or after the due date this part order can be
manufactured. You can still
force this part order to be manufactured earlier in ‘Part orders’-window simply
by selecting this order to be nested. Increasing this value helps you raise a
sheet utilization factor. Any part nested that is outside the manufacturing
window will be nested as a filler part.
Next phase: Tells the next phase number of this part. This field can be
used to keep such parts together that are going to the same next phase.
Priority: Sets the priority of the order. 1 is the least urgent and 9 the most
urgent.
Process this order immediately: By setting the ‘forced priority’
on, you
can make this order be manufactured as soon as possible. It will bypass all the
other orders.
Additional Information
Status: Shows the current status of the order. Status can be changed for
any part(s) at any time.
The choices are:
o New order: None of the parts are nested yet.
o Order split: Some
of the parts are nested, but not all.
o Nested: All the parts are nested.
o Manufactured: All the parts are nested and manufactured.
o Program missing: Part program (.cp-file) is missing.
Material code: Allows user to select the material to be used for the order.
Material listed
comes from the Environment (CAM.mdb). This is modified
when importing from DXF or utilizing part scripting.
Thickness: Allows user to select the material thickness to be used for the
order. Thickness’ listed comes from the Environment (CAM.mdb). This is
modified when importing from DXF or utilizing part scripting.
Use existing part file: The order will use the cp part file from the default
part directory when nested. When the Select
button is clicked in the Header
frame, cp files will be shown in the Open dialog.
Autotool part from DXF: The order will use the dxf part file from
default DXF directory when nesting. When you click the Select button in the
Header frame,
dxf files will be shown in the Open dialog.] When using this
option the DXF file will be imported and create a CP file utilizing the material
and thickness defined. Part will then be Autotooled using parameters set:
Parameters:
The parameters dialog will display parameters that Autotool
will use.
122

This is a scripted part: This option tells NC Express that the part will be
created from a script. Material and Thickness will need
to be selected. When
the Select button is clicked in the Header frame for Part name, scripted files
(.js or .vbs files only) will be shown in the Open dialog. If the ‘This is a
scripted part’ option is selected and the Parameters button is clicked,
the
following dialog will be displayed:
From this dialog, the user is able to set the scripting parameters for the part that
will
be created when the order is ran.
123

9.3 EXERCISE- USING ORDERS DATABASE
The
following section will describe how to utilize the Orders Database (OMS)
feature.
Orders Database can be used to increase productivity level when
nesting
parts. The following steps will show how to add parts manually within
the
Order Database, nest the parts, and then accept (complete) the order. Once
the
order is completed a text file will be exported to display parts that have been
processed.
Step
1: Open Orders Database by going to Database menu | select Orders.
Step
2: Select the machine that will be used from the Machine drop down
menu.
Step
3: Before adding order make sure the Active tab is selected.
Step
4: Click Add on dialog to open New Order dialog.
Step
5: Enter part order information for three parts listed below (for
unidentified
fields below leave the fields untouched in the New Order dialog):
For
this exercise we will use the cp files : alu2mm_a_small / alu2mm_b_small /
alu2mm_c_medium
/ alu2mm_d_large from previous exercises.
Alu2mm_d_large
Order name: TEST
Machine Tool: ‘use current machine’, select from drop down menu.
Part name: Click Select to open default part directory. Select
alu2mm_d_large.cp from previous exercises.
Priority: 6
Ordered Quantity: 20
Extra parts allowed: 50
Click OK
Alu2mm_c_medium
Order name: TEST
Machine Tool: ‘use current machine’, select from drop down menu.
Part name: Select alu2mm_c_medium.cp by clicking Select and
finding
within the default part directory.
Priority: 5
Ordered Quantit y: 27
Extra parts allowed:
0
Click OK
124

Alu_2mm_b_small Order name: TEST
M achine Tool:
‘use current machine’, select from drop down menu.
Part name: Select NESTPART2.cp
by clicking Select and finding within
the default part directory.
Priority:
5
Ordered Quantity: 8
Extra parts allowed:
0
Click
OK
Step 6: After parts have been entered into the Orders Database they are now
ready to be nested. Sort parts by machine name
by clicking Machine in Sort by.
Select all parts to be nested (parts input from
step above) by clicking on the
machine name within
the grid (white area). Once parts are selected click
Nesting [x]…
Step 7: Once the parts are nested from the Orders Database the system will start
nesting from run folder 800. If run folder
800 has already been used the system
will
ask if it is okay to overwrite the existing folder, click OK to overwrite or
Cancel to continue to next number.
Note- run folders created before
NC Express was currently opened will be asked
if it is okay to overwrite, and run folders created while NC Express is currently
opened
will automatically be skipped.
Once the run folder(s) is created the nest dialog will appear. The dialog is set
the same way as normal nesting.
125

Step 8: Once parts have been nested they will need to be optimized and post
processed. The nested sheets can either be batch processed (all at once) or
optimized and post processed one by one.
Batch Process (all at once)
Open the Optimizer and set the options within to create a desired output. Once
options
are set click ‘Use as default’, and then click Cancel to close the dialog.
Highlight all sheets within the Nest Explorer and click Process to start
optimization and post processing of the sheets in the nest.
Processing One by One
Open
the Optimizer and set the options within to create a desire output. Click
OK
when options are set. Open Post Processor dialog and set location and file
name
of the nest, click OK to process sheet. Select the next sheet and click
Open (or double click on the selected sheet to open). Process in the same
fashion as the first, continue for each sheet listed in the Nest Explorer.
Step
9: Once sheets within the Nest Explorer display Postprocessed they are
ready to be accepted. Accept will move all nested parts within the Active tab of
the Orders database to the completed tab. If some parts or a portion of the parts
ordered were not nested or processed they will remain in the Active tab.
Highlight all sheets within the Nest Explorer and click Accept.
Note- if an error message appears that
the raw material is not available this
means that the material sheet
size that was nested was not input into the Plates
Database. This error is okay and files are still created.
126

Once the sheets are accepted the Nest Explorer will display Accepted.
Step 10: Open Orders Database from Database menu. Once the sheets were
accepted the parts that were nested are now moved from the Active tab to
Completed tab. Click on ‘Completed’ to view the parts.
Step 11: To create a report (text file) that will display parts that have or will
been
processed through NC Express click Export on Orders Database dialog.
This
will bring up the Windows Save As dialog. Find a directory to output the
text file, type in the name of the file, and click Save. This file will store
information for parts that are both Active and Completed. Part quantities as
far
as how many have been nested or ordered is stored within this file. This file can
be
used to track what has been processed for the day.
127

10 CREATE PARTS
10.1 CREATE PART3
128

10.2 CREATE PART4
129

10.3 CREATE PART5
130

10.4 CREATE PART6
131

11 AUTOTOOL SPECIAL PARTS EXERCISES
The following pages of section 8 (Autotool Exercises) has explanations of what
to do in each case. Read explanation and repeat process to create expected
outcome.
Exercise 1:
Step 1: Create a new part: ALMg3 (2mm)
Step 2: Import dxf file: Drawing1.dxf
Step 3: Change settings for Autotool as follows:
Large contour- lead in with a straight line and a arc off 2mm diameter
Make loops for every corner equal or smaller then 90 degree.
Medium contour- lead in with a pilot hole with a diameter of 0.5mm
Small contour- straight lead in off 2mm
Step 4: Autotool part and save.
Exercise 2:
Step 1: Open parts drawn before: Part1.cp and Part2.cp
Step 2: Change settings for Autotool as follows:
Apply microjoints to parts internally and externally.
Autotool the parts in different kinds of material and thickness to
see the different settings.
Exercise 3:
Step 1: Parts: Part1.cp and Part2.cp
Step 2: Autotool parts by changing values within leads tabs to view outcome.
(change lead-in type, lengths, technology types…)
132

11.1 COMMONLINE CUTTING AT PART LEVEL
If you want to use commonline cutting in NC Express for punch/laser, it must be
prepared at the part level.
1. Open the
single part file and check that the geometry of the part is
correctly represented (for example, that all closed contours really are
closed and so on). Remember to save
the
part.
2. Select Drawing | Features | Grid Parts from the menu.
3. In the n (part per column) and m (part per row) fields set the amount of
parts in a commonline.
4. Click on the Laser Commonline radio button and check that ‘Beam
Width’ is the correct value.
5. Click on the Prepare button.
6.
Click on the Save As button and enter a name for this commonline part.
7.
Review on the screen the outside contour presented with a red pen and all
commonline cuts with a yellow pen. If your part doesn’t have corner
notches,
it is normal to have tiny red squares in an intersection point of
four parts. These small squares will not be cut.
8. Close the Grid of Part dialog.
9. Select Tooling | Autotool from the menu. Click on the General
tab assure
that you have selected Laser in the Machining mode area.
10. Click on the Path/Contours tab. Check the values
for lead-in and lead-
outs of commonline cuts. Note
the following restrictions:
Outside lead-in length for a commonline cut is actually hard-coded to a
half beam
width. If you give zero for a lead-in length of commonline cut in
inside contours, the program will
create lead-in lengths of a beam width.
11. Click OK to close the Autotool dialog, and then review the results.
12. NOTE: Commonline parts are prepared so that if the part is longer than its
height, it is released with a horizontal cut. High
parts are released with a
vertical cut. Exceptions: If you have only one column of parts, they are
always released by a horizontal cut. If you have only one row of parts, a
vertical cut always releases them.
13. Nesting and optimizing works the same way for commonlined parts as for
any other parts.
133

11.1.1 Commonline Example 1
Step 1: Open part: common1.cp: Training FPL\common cut\common1.cp
Step 2: Save the part in the part directory
Step
3: Go to Drawing –Features – Grid parts
Step 4: Fill in the n-
and m- parameters
Step 5: Click on the button Show Grid
Step 6: If you now zoom in on the parts
you
can see that we still have two separated
lines.
Step 7: Click now on the prepare
button
Step 8: if you now zoom in on the
part you
can see that there is now one line.
Step 9: Save the part as a common
part
Step 10: Close the grid part window
Step 11: Autotool the part
As you can see the inside contours will be
cut first and then the common lines and as
last the outside contour
134

Finished Part
11.1.2 Commonline Example 2
Step 1: Open part: common2.cp
Step 2: Save the part in the part directory
Step 3: Go to Drawing –Features – Grid parts
Step 4: Fill in the n- and m- parameters
Step 5: Click on the button Show Grid
Step 6: If you now zoom in on the parts you can see that we still have two
separate lines.
Step 7: Click now on the prepare button
Step 8: if you now zoom in on the part you can see that there is now one line.
Step 9: Save the part as a common part
Step 10: Close the grid part window
Step 11: Autotool the part
Step 12: On the tab page Path/Leads you can find back the parameters for a
common cut line.
135

Minimum width of internal common line contour
If the inside of the common line contour is more then 5 mm then this inside
contour will be cut into pieces and will stay attached with microjoints. But,
when the common lines are cut then the microjoints will be cut to.
Finished Part
136

11.1.3 Commonline Example 3
Step 1: Open part: common3.cp
Step 2: Save the part in the part directory
Step 3: Go to Drawing –Features – Grid parts
Step 4: Fill in the n- and m- parameters
Step 5: Click on the button Show Grid
Step 6: If you now zoom in on the parts you can see that we still have two
separated lines.
Step 7: Click now on the prepare button
Step 8: if you now zoom in on the part you can see that there is now one line.
Step 9: Save the part as a common part
Step 10: Close the grid part window
Step 11: Autotool the part
Now we made the inside common contour smaller then 5mm so now the
inside contour will be cut into pieces with the common lines:
137

11.2 COMMONLINE CUTTING AT NESTING LEVEL
To be able to make this exercise you have
to make a nesting.
See
chapter about nesting.
11.2.1 Commonline with same parts
To make it easier to explain how this is working we will start by making a nest
with the same part.
Now we have an normal nesting, when we go back to the global parameters from
the nesting then we have to enable the commonline cutting :
NOTE: Make sure that the
right value for the beam
width is filled in !
For Normal and fast cutting we
have the beam radius
compensation in the machine
but for COMMON LINE is
NOTE: Set your desired commonline
nest option here. Note that sides of
the parts which can be commonlined
less than 30% will be nested with the
normal component spacing for that
particular side.
Circles will never be commonline
nested.
138

After changing the nesting parameter for common line we can see how the
parts are rotated to have a good common cut.
But when we zoom in we can still see that the parts are still separated. It is
only after optimisation that the common line will be created.
Now we can optimize our nesting. To create the common
line we have to
enable
the common line parameters and fill in the values:
To be able to explain the values from the common line you have to know how
the laser
is going to cut these parts :
On
the drawings we are using different
names for the values:
Leadin
length = X1
Leadout
length = X2
Precut length = X3
Back
overcut = X4
Forward
overcut = X5
139

Step1 : First the inside contours will be cut
Step2 : Starting at the first outside contour with the lead in length = X1
140

Step3 : Cutting the outside contour until the first point where we have a
common line + the precut distance
Here you see that we don’t stop on the intersection but that the laser cuts a
little bit longer = Precut distance. Never take this value to small
At the end of distance X3 the beam is put off and the cutting head is moving
back to the point where you can see the arrow.
To understand what is happening you can follow the drawing but be aware
that this drawing is enlarged. The distance of the precut is 4mm !!
Step 4:
First the laser cuts until the end
of the precut (x3) then the beam
is put off for the distance X3-
X4.
At the point where length X4 or
the back overcut begins the
beam is put on again and the
laser is continues to cut the
outside contour.
141

Step 5: Continue to cut the outside contour
On each intersection you can see that the laser cuts
a precut :
Step 6: Then we come on the end of our part and there we cut a lead out
distance
= X2
142

Step 7: After the first part we start with the inside contours off the second part
Step 8: Because of the common line we don’t make new lead in but we start at
the at one of the precuts :
The distance X3 was
already cut so we start
cutting at the beginning of
X5.
We start the cutting in the
laser curve !
This way we continue for
all the parts…
At each intersection we
have the precut distance
and then we always start
our cut in this laser curve.
143

11.2.2 Commonline with different parts
Step1 : Create a nest with different parts:
Step2 : In the Global Parameters from the nesting you can select the options
for common line. Here you can choose between a common line for all parts or
a common line for only the same parts .
144

Step3 : Common line for all parts
Step4 : Common line for only the same parts
If you look close then you can see that the only the same parts are put in
common line.
145

11.3
PRESHEARED PARTS
The process to create a presheared part is totally different :
For nesting Preshear, a part is tooled through Autotool then ready for
optimization directly after. When programming presheared parts through NC
Express there is no nesting involved the part goes directly to presheared
optimization.
With this option it is possible to make a part from which we only will cut the
inside contours.
Let say that we have somewhere a left over from 200 by 150 and we want to cut
a rectangle with those dimensions with some inside contours. Then we will
handle this as follow :
Step 1: Draw a rectangle from 200 by 150 and the inside contours
S tep 2: Go to autotooling and make sure that the option Preshear is enabled on
the tab page General.
You
will see that only the inside contours are being tooled.
146

Step 3: Go now straight to optimizer.
You can see that the nesting is made on the rectangle that was drawn.
Only the inside contours will be cut.
147

12 NESTING EXERCICES
Here you have two nesting files. Try to make the same nestings.
The dxf files are in the directory DXF exercise.
You will need to import the dxf files and tool them.
To be able to make the nesting you need to check how many parts you need.
12.1 NESTING 1
148

12.2 NESTING 2
149

APPENDIX A- AUTOTOOL SETTINGS
General tab
Machining mode- select the type of tooling to be placed on part. For turret punch
press machines only punch and nibble can be selected.
o Laser- used to tool a part with shear tooling.
o Use taught cycles- enables the use of taught cycles that have been created.
o Preshear- tools only interior geometry
• Laser processing mode – depending on material and thickness the parts will be tooled
with a different mode. In the chapter high speed and normal cutting mode you can find
back more explaination.
CAD Layer Filter- used to filter layers of dxf files and DADO lines and points.
o Closed Contours- closed geometry used by system for offset cutting. This
variable can be alphanumeric or “ALL”. Layers from imported dxf file that
are desired layers to be tooled are entered exactly as NC Express sees them.
(Layers defined can be viewed by going to Settings menu | CAD then select
layers…)
o DADOS- open geometry used by system for centerline cutting. Cannot be
“ALL”. Enter DADO for DADO lines to be tooled.
150

Microjoint tab
Microjointing places gaps between tooling internally and/or externally.
External/Internal Contour properties-
Min. segment length- Minimum length of segment to microjoint.
Microjoint length- distance of microjoint.
Maximum
Microjoint distance- max. distance between microjoints.
Minimum
Corner-micros- (external only) Used for punch only. Allows for corner
tabs to be placed at a minimum selected.
Lead-in settings- See Lead-in settings in this Appendix.
Lead-out settings- See Lead-out settings in this Appedix.
Microjoint tools- Option to allow the use of a special tool
as a microjoint tool when using
punching
only.
(Not applicable for FPL)
151

Path/Leads
Set Contour defaults here along with lead-in and lead-out settings. Commonline cutting
parameters are set in this tab as well.
Contour types- Set dimension limits for each contour type within the Autotool
settings. Notice how each value is placed in-between both contour types. Contour
types are defined in the machine parameters
of the Settings menu.
Lead-in settings- See Lead-in settings.
Lead-out settings- See Lead-out settings.
Auto Cycling- Enable auto cycling of laser cutting. Used for faster cutting sequencing
(high speed).
Common Line Cuttingo
Minimum width of internal common line contour- Allows for cutting head
to not drop down any large holes within a nest of commonline parts. Any
cutout larger than this value disables laser from cutting continually.
o Laser beam width (IMPORTANT)- Sets beam width to check for radius’
less than half the beam width, to avoid problems at the machine. If a tooled
part has a radius/line less than half the beam width the machine stop and give
an error message telling operator that there is a problem with the nest.
o Lead-in & Lead-out lengths- Sets lead-ins and lead-outs for inside and
outside edges of commonlined parts.
152

Lead-ins settings
Straight Lead-in
L1- Initial length of lead-in.
L2- Secondary lead-in length. Ability to
split lead-in into two section, to change
technology for one and remain same as
contour for second.
A1- Angle of lead-in. Measured
perpendicular from the contour.
T1- Change technology for L1 lead-in.
T2- Change technology for L2 lead-in.
Arched Lead-in
L1- Length of Lead-in.
A- Angle of Lead-in. Measured
perpendicular from contour.
R- Radius
of Lead-in.
T1- Change technology of R Lead-in.
T2- Change technology of L1 Lead-in.
Lead-in with hole
R1- Radius of lead-in
R4- Radius of hole
A1- Angle of lead
L1- Length of Lead-in, not including arc
153

Spiral Lead-in
R1- Radius at entry
contour
R3- Radius end of spiral
R4- Radius of spiral
N- number of spiral lines
L1- Length of lead
of lead entry on
Add loops to corner
Enable- Enables (activates) corner loops.
Value 2.2- Radius of loop.
Value 1.2- Length of lead line to radius
of loop.
Value 20- An y corner with an angle less than (x) angle
will have corner loops applied.
Fillets
Enable- Enable (activate) fillets to be applied to
corners.
Value 2- Radius
of fillet.
Value 91- Any corner with a angle of
90 or less will
have fillets applied.
Overlap
Value 1- Amount of overlap between lead-ins and leadouts.
Maximu m value for overlap is set as default 3mm
in machine p arameters | misc tab (Max. overcut).
T1- Change technology for overlap. Enable- Enable (activate) overlap.
Minimum distance to contour- Sets minimum
allowable
distance for end of lead to be from contour
of part. If pilot hole
distance measured fro m closest outside edge of tool. If no pilot
hole distance is measured from center of pierce
point.
Important- Settings for Lead-ins are saved in the Cam.mdb database for each
material type and
thickness, so each time that material is used the settings will be reused each time that material
type and thickness is used. When settings are changed for a material type and thickness and user
exits to another type system will ask to save settings, click Yes to save and reuse. Settings for
microjoint lead-ins differ from normal lead-ins.
154

Lead-outs settings
L2- Lead-out length. Maximum
lead-out length set in machine
parameters | Misc tab (Max.
Leadout).
R2- Radius of Lead-out. Set to zero
(0) to make straight lead-out.
A2- Angle of Lead-out.
Measured
perpendicular from contour.
T1- Change technology for R2.
T2- Change technology
for L2.
Minimum distance to contour- Sets minimum allowable
distance for end of lead to be from contour of part. Measured
from end
of lead-out.
Important- Settings for Lead-outs are saved
in the Cam.mdb database for each material type
and thickness, so each time that material
is used the settings will be reused each time that
material type and thickness is used. When settings are changed for a material
type and thickness
and user exits to another type system wi ll ask to save settings, click Yes to save and reuse.
Settings for microjoint lead-outs differ from
normal lead-outs.
155

APPENDIX B- NEST PARAMETERS
Nest settings
Global parameters
Run number- Displays run folder number. Run folders are stored in the NceXpress
file system. Run folders store all data related to nesting, optimizing and NC code.
Part separation- Defined as minimum skeleton distance between parts. This value
changes the distance that parts are placed in a nest. In machine parameters there is a
field for separation factor which is looked at by Part separation. This value is
multiplied by the thickness of the sheet to result in a minimum part separation for the
parts. 0 may also be used.
Grid nesting- A grid option is used rather than a normal method of nesting. Grid
nesting is used to create automatic shear nesting. This will create a grid of parts
automatically.
Plate margins- The distance on each of the four edges of the plate not included in the
nest.
Direction- The nesting program places one part at a time on the plate. The direction
factor determines the position of placement of the parts in sequence. The center
selection means that the first part is placed at the geographic center of the plate and
each succeeding part is placed around all the proceeding nested parts until the plate is
full as dictated by the nesting algorithm. Similarly selecting the upper left point will
cause the first part to be placed at the upper left corner of the plate and the process
proceeds from there. Each selection determines a different starting point.
156

Clamp informationo
Locations- The center of the clamps along the x-axis of the machine. The
default location is determined by formula based on the travel of the punch
head as defined in the machine file. All locations
are user modifiable.
o Nest under clamps- Enables the ability to nest parts around or under the
clamp avoidance zones.
Part List
Part List will determine which and how
many parts will be nested onto the
plate(s). Few other options to change
parameters of nesting included in part
list.
New
Above right
is a screen shot of the new part record. Click on new to select parts that will be
input into the current
nest.
Name- Displays name of part selected.
Work order- Work order number from the orders database.
Due date- Set a due date for part being nested.
Quantity- Amount of parts that will be nested in current nest.
Priority- (Values 0-9, 9=highest) Set priority, similar to tools, parts with higher
priority will be nested earlier in the nest.
Grid nesting- Turn on or off by placing check mark. Depicts whether or not grid
nesting will be turned on for part.
Part
orientation-
157

Initial rotation- Rotates parts automatically in nest to value entered (0°-360°).
Set to default changes Initial rotation back to original part configuration.
Allowed rotations- Sets parts to give ability to rotate freely in the nest.
Before checking rotation on these, tools used must be indexable to these
angles in order to be ran or parts need to be tooled with Variational tooling.
Modify…
Clicking
on Modify… brings up the same screen as New Part Record (clicking new). Modify
gives
ability to edit parts inserted for nest.
Delete
Select
part to be removed from nest and click Delete, part will be removed from current nest.
Due
date
Due
date set to current date when creating a new nest. When opening an old nest Due date will
remain
the same as the date it was nested.
Plate list
Plate list identifies plate
sizes and quantity of
plates per size. This tab
configures all of the
parameters for plates
involved in producing
parts.
In the plate list we get the plates out of the plate database for that kind of material and that
thickness that w e have selected for the nest.
158

Switch Up
Highlight plate, click Switch Up to move plate a single line at a time. Top plate is used for nest.
New
Clicking new will bring up Plate record screen.
Plate ID- Enter name of plate.
Reserved- Quantity of plates being used.
Cost per sheet- Input price to be calculated in post process.
X and Y- Top line equals X coordinate line on right equals Y coordinate.
Modify…
Highlight plate,
click Modify to edit plate.
Delete
Highlight plate, click Delete to remove plate from current nest.
Square last plate
Last plate in nest squares all parts in order to use maximum utilization
Use in listed order
This option will make the nesting on the plates like they are put in the list.
This means if we
have 3 times a sheet of 3000x1500 and 6 times a sheet of 2000x1000 and
1 time a sheet of
2500x1250 then we will get the nest in the same order. (if all plates are needed)
Use smallest
With this option the nest will be made on the smallest plate out of the list.
Use only the first plate size
With the switch up button we can put any plate on top of the list and then NceXpress will use
this plate to make the nest.
Advanced
????????
Set plate
limit
? ???????
for parts nested.
159

APPENDIX C- OPTIMIZER SETTINGS
Cutting Destination- Destination point of the last part of the nest. Select the corner in which
you want the machine operation
to terminate.
Swath-
Creates zones either horizontally or vertically. Choose to cut in horizontal or vertical
direction.
Generate-
Crop line- Create a laser path
to the right of parts nested. Used to cut off unused material.
Outside
lead- Creates leads on the outside of parts, if not already created.
Inside lead- Creates leads on inside contours, if not already created.
Smooth
Cutting- Generates a smooth path with limited axis moving.
Calculates the end
point of cut and start point of next cut then make smooth transition to next
cut.
Clamps
No Fly Zone- If we enable this option and we put the size to 100 then this means that
the
cutting head will be lifted straight up with ping-pong disable when we ‘fly’ over parts with a
X and/or Y size smaller than 100mm.
Reason
for this function is that we can eliminate the danger to hit a part which is possibly fallen
halfway
between the slats when we start the ping-pong motion. Recommended size is 100mm!
Prepierce
– Adds prepierce cut to lead-ins
Use
G41/G42 command in normal cutting – activates the beam radius compensation on
machine
side
Head down- (Used only in high speed mode) Setting will tell optimizer
how long the head can be down after cutting until it must be picked
up.
Common Line-
These parameters are explained in the commonline exercise
.
160

Scrap cut- (Skeleton cutting) Create scrap cutting for parts. Will create a grid outside the parts
to remove the scrap. X and Y coordinates will tell the optimizer where exactly you would like
this grid to be created.
Post cutting- outputs the scrap cuts to be cut after all parts have been cutout.
Tempory High Temperature area
Delay Before Growth – (sec) This parameter tells us when this area will start to heat up. In
most cases this parameter will be zero because at the moment we activate the beam and start to
cut the material, the material is already warming up.
Offset Growth Speed – (mm/sec) This is the speed with which the Temporary High
Temperature Area grows.This depends on the kind of material and the thickness.
Maximum Offset Size – (mm) this is the max. distance around the contour that will warm up
during the cutting. This value will determine the maximum size of the Temporary High
Temperature Area.
Once the boundaries of this area have been reached the material will start to cool down
Delay Before Fall – (sec) This parameter will tell us when the temporary high temperature area
will start to shrink, to cool down.
Offset Fall Speed – (mm/sec) This is the speed with which the warmed up area shrinks.
This parameter allows us to calculate how long it will take until the area around the cut part is
again safe for usage.
Max Delay in Post – (sec) When jumping around
from contour to contour to avoid these High
Temperature Areas there can be a moment where we have to wait until everything is cooled
down.This parameter allows us to set the maximum waiting time.
161

APPENDIX D- PARAMETERS NC CODE
Parameters set for each material type and thickness are originally set by Finn-Power from
experienced user. These values generally do not need to be edited.
Focal length and Focus point
These are the parameters from the cutting lens that come from the database
Cutting head mode
The quickness of response off the sensor in the cutting head.
1=fast motion of the cutting head
2=slow motion of the cutting head
Acceleration
[10..100%] The acceleration setting during the processing. The percent value from maximum
vector acceleration
Smooth pos
[10..100%] The speed and acceleration of the positioning. The percent value from maximum
vector speed and acceleration
Laser beam selection
The different setups for laser beam diameter and focal length compensation
Foil processing
When there is a foil on the plate we have to activate the foil cutting. Then put this parameter
on 1. This can not be done in high speed cutting.
Sheet probing
162

When we want to do a sheet probing (determine how the plate is place on the table) then we
have to activate this parameter by putting to 1.
When we have a automatic loading table or when we put the plate in our clamps then this is
not necessary to do.
Prepunch probing
If we put a prepunched plate into the machine then we have to activate this parameter so it
will measure the prepunched holes or other contours before starting the cutting.
Focus pierce
Here we can do a repositioning of the lens while piercing. This is only for thick material and
the values will be filled in automatically
Cutting head position
[mm]The cutting head distance from sheet to upward direction during positioning
Cutting head position type
0=reclinear cutting head motion during positioning,
1=Ping-Pong cutting head motion during positioning
Corner function
This parameter will be activated automatically when it is necessary. This corner pulse will
make it able that the corners are cut nice, just before a corner we will cut slower and with
pulses.
Output m01
After every part there will be generated a code that
will make the laser stop.
Nozzle calibration
The calibaration of the distance control sensor in the beginning of the
NC-program
Scrap cut parameters
When we have a cropline then on
5mm before the end off a plate the cutting head will disable
his sensor, go 3mm outside the plate starts cutting and after 5mm activates the
sensor again
goes to the other side off the plate and there 5mm before the edge the sensor will be disabled
again to go 3mm outside
the plate.
163