21.08.2020 Views

Programmer V5 EN

This is a multi-channel programming system for turning / milling machines with 3D machine room simulation. ● You create NC programs on the basis of an NC editor with machine macros and an integrated 2.5D CAD / CAM system. ● Templates are stored for different types of processing (bar / chuck ...). ● Program structures are generated automatically. ● The 3D machine space simulation shows the real machining process simultaneously. ● The actual implementation of the NC program is simulated. ● In the event of a collision, the relevant machine components and the associated NC blocks are displayed. What are the extensions of the V5.1 programmer? ● Project history and additional windows for further machine conditions ● Main and subprogram names are displayed in the simulation ● 3D blank (prismatic, rotationally symmetrical) is to be read in the STL format into the simulation ● The current workpiece is to be generated from the simulation as a 3D blank in the STL format ● Gaps can be measured in three dimensions ● NC block run times can be displayed as an EXCEL table

This is a multi-channel programming system for turning / milling machines with 3D machine room simulation.
● You create NC programs on the basis of an NC editor with machine macros and an integrated 2.5D CAD / CAM system.
● Templates are stored for different types of processing (bar / chuck ...).
● Program structures are generated automatically.
● The 3D machine space simulation shows the real machining process simultaneously.
● The actual implementation of the NC program is simulated.
● In the event of a collision, the relevant machine components and the associated NC blocks are displayed.

What are the extensions of the V5.1 programmer?
● Project history and additional windows for further machine conditions
● Main and subprogram names are displayed in the simulation
● 3D blank (prismatic, rotationally symmetrical) is to be read in the STL format into the simulation
● The current workpiece is to be generated from the simulation as a 3D blank in the STL format
● Gaps can be measured in three dimensions
● NC block run times can be displayed as an EXCEL table

SHOW MORE
SHOW LESS

Create successful ePaper yourself

Turn your PDF publications into a flip-book with our unique Google optimized e-Paper software.

www.dmgmori.com

Turning technology

DMG Programmer 3D Turning V5

Programming

Training – The decisive know-how advantage

Training Manual

CONTROL

DMG Programmer V5


A-D821UK-1

Programmer 3D Turning V5

Programming and Operation

DMG MORI Academy GmbH

Gildemeisterstraße 60, D-33689 Bielefeld, Phone: +49 (0) 52 05 / 74 - 25 01,

Fax: +49 (0) 52 05 / 74 - 25 02, training@dmgmori.com, www.dmgmori.com

Disclaimer of warranty:

The information in this document has been compiled to the best of our knowledge.

However, we do not assume any responsibility for possible errors and consequential damage.

© 2020 DMG MORI Academy GmbH, Bielefeld

All rights reserved, including photocopies, filming, reproduction through image and sound carrier of any kind and

partial copies. According to the copyright law, it is prohibited to reproduce copyrighted works or part of them, even

for teaching or training purposes, except after consent from the publisher and, if applicable, against payment of a

fee for the use of foreign intellectual property. According to the copyright law, "those who reproduce a work without

the beneficiary's consent in cases other than those legally allowed" will be penalised with a prison term of up to one

year or with a money fine.

2


Dear customer!

Quality is our program.

We guarantee a high training standard by constantly optimising the course structures and regularly updating the

documents used for teaching.

The present teaching document has been designed to complement the machine's operating instructions and the

programming instructions of the control unit manufacturer. It does not and cannot replace them!

This document was didactically-methodically elaborated by the DMG MORI Academy. Its contents are oriented

towards your requirements, so that you hold in your hands an accompanying working tool during the course with

us and later on in your job.

In order to save what you have learned, write down your own notes on the margins provided for that purpose. This

will provide you with a useful way to brush up your knowledge.

We hope you are satisfied with our course and wish you the best possible success on your job.

Bielefeld, February 2020

3


Table of Contents

1 Table of Contents

1 DMG Programmer 3D Turning 8

1.1 Basic menu 9

1.2 Program management 10

1.3 New project 10

1.3.1 Defining a new project 11

1.3.2 Entering setting data 12

1.4 Defining operations 16

1.5 Defining a tool 17

1.5.1 Defining a new tool 18

1.6 Executing a tool change sequence 20

2 Simulation 26

2.1 Simulation toolbar 27

2.2 Zooming, rotating and moving using the mouse buttons 28

2.3 Simulation settings 29

3 Operation plan manager 32

4 CAD/CAM operations 36

4.1 Plane definition 36

4.2 Computer-aided design (CAD) 37

4.2.1 Setting the intersection snap function 38

4.2.2 Creating a new contour 38

4.2.3 Form elements and undercuts 39

4.2.4 Deleting elements 40

4.3 Generate operations in CAM 41

4.3.1 2D simulation 45

4.3.2 3D simulation 46

4.3.3 Generating an NC code 46

4.4 Turning cycles 48

4.4.1 Hiding elements 50

4.5 Operation on counter spindle 51

4.5.1 Generating the contour for counter spindle 52

4.5.2 Construction lines 53

4.6 Recesses 55

4.7 Generating an operation in channel 1 with B axis 57

4.7.1 Recess machining 58

4.8 Thread definition 59

4.9 Milling operation 61

4.9.1 Chamfering face contours 66

4.10 Face drilling 68

4.11 Milling using mechanical Y axis 70

4.12 Pocket milling using the CAM function 73

4.13 Y-axis machining – direct programming on turret machines (recess) 76

4.13.1 Y-axis machining – programming on turret machines using CAD/CAM (circular pocket) 79

4


Table of Contents

4.14 Cylindrical interpolation 84

4.14.1 Groove without macro 87

5 Machining with tailstock on the 4A TWIN machine model 92

5.1 Case 1 Machining on long zero point 92

5.2 Case 2 Short zero point 96

6 4-axis machining 100

7 Defining the raw part 108

7.1 Creation of the raw part in the CAD/CAM module 111

7.2 Reading in the raw part as STL 113

7.2.1 Loading of the STL file as raw part 114

9 G codes 124

9.1 Syntax explanation 124

9.2 High-level language and G codes relating to Programmer 125

9.2.1 Commands not supported (examples) 127

5


6


B

78

E

30°

F

36

32

0

1

45

57

14

25

20

M 42

32

31

40

18

R5

2

28

0

3

B

4

E

F

1 2 3

4

A

51,8

100±0,05

72,1

76,9

94,5

A

22,5°

DIN 76 - A

1,6x45°

2x45°

18 -0 ,05

- 0,01

x1,5

70 ±0,05

R 2,5

C

6± 0,05

C

6

2

D

48H7

D

167°

DIN ISO 13715

DMG-TA

36,5±0,02

+0,4 -0,4 Allgemeintoleranz ISO 2768-m

Verantwortl. Abt. Technische Referenz Erstellt durch Genehmigt von

DMG-TA

Dokumentenart

Fertigungszeichnung

Rohmaterial : Rd 80x102

Alle Kanten gebrochen

Nicht bemaßte Radien/ Fasen 1 mm

Dokumentenstatus

freigegeben

Titel, zusätzlicher Titel Material

Änd. Ausgabedatum

Übung 4

M 1:1

EN AW-Al Cu 4 PB Mg

Spr.

de

Blatt

1

1

Chapter

3D Preparation programs


1 | DMG Programmer 3D Turning

Memo

1 DMG Programmer 3D Turning

This training document shall be used in conjunction with a training course provided by

DMG MORI Academy only and makes no claim to be complete.

It describes the complete step-by-step programming procedure from the entry of a

new workpiece to the finished machining program.

To make yourself familiar with the steps described, we recommend reading the individual

topics page by page and then repeating them by hands-on experience at Programmer

3D.

8

A-D821UK-1_200420


1 | DMG Programmer 3D Turning

1.1 Basic menu

Most operations can be executed by means of appropriate icons. In addition, menu

sequences are available (e.g. FILE, BASIC MENU instead of the respective icon).

Memo

DMG Programmer 3D Turning

1

9

Projects - e.g. definition of a new workpiece

Waitmarks manager (for 4-axis machining only)

ISO converter - conversion of the programmed sequences into Siemens high-level

language

Simulation - 3D simulation with collision monitoring

Tool setting sheet - management of the tools for the current (selected) workpiece

Workpiece settings - zero points, chuck data, raw parts, etc.

Operation plan manager - definition of a new tool based on the Gildemeister work

plan

Macros catalogue

Tools catalogue - all tools stored are listed here. Program management

A-D821UK-1_200420

9


1 | DMG Programmer 3D Turning

Memo

1.2 Program management

Programmer automatically opens an overview window that comprises 4 individual windows.

On the left, you will find a list of all workpieces and of the installed machines.

In Channel 1 and Channel 2, the operations (=programs) are displayed while the part

of the program that has just been clicked in Channel 1 or Channel 2 is shown on the

right. Here, the NC code can be edited directly.

1.3 New project

In the following sections, you can learn step by step how to define and generate

a project with its machining processes.

To make the procedure valid for all machines, the workpiece of this first project is

manufactured at spindle 4 with channel 2 only.

As an example, the first exercise from the Annex is used.

10

A-D821UK-1_200420


1 | DMG Programmer 3D Turning

1.3.1 Defining a new project

To define a new project, select the tab "Projects" from the basic menu.

Then select the appropriate machine and open the pop-up menu using

the right mouse button.

Memo

1

11

DMG Programmer 3D Turning

The following window appears for the entry of further data.

Here, you can enter global project information.

The minimum input requirements are the project name and the model. In this dialogue,

a model can only be entered once.

After the data have been entered in the required fields, close the window using

"OK".

A-D821UK-1_200420

11


1 | DMG Programmer 3D Turning

Memo

1.3.2 Entering setting data

Next, you should specify the setting data such as fixtures, workpiece,

jaws and transfer parameters. To do so, click the icon for entry of

workpiece settings.

All the parameters being relevant for the workpiece are transferred into the loading

program for variables via the workpiece settings function. Moreover, the clamping

and workpiece data are entered for 3D simulation. In detail, this refers to the following

data:

Base body of the

clamping device

Clamping elements

such as jaws

Define workpiece or

read in STL file

RG738 = raw part diameter

RG725 = finished part length

Minimum Ø = hole diameter

Add-on Z - Rear = allowance on left side (SP3)

Add-on Z - Front = face allowance on right side (SP4)

Send to other spindle

Delete

Save data

Design your own chuck

Accept the settings by pressing OK.

12

A-D821UK-1_200420


1 | DMG Programmer 3D Turning

If data shall be entered for all the spindles, you can select the appropriate tab to

change over to the desired spindle. Similar data are entered for the spindles 3 and 4.

Memo

1

13

Tabs for change-over

Base body of the

clamping device

DMG Programmer 3D Turning

Clamping elements

such as jaws

Some parameters may not apply and others may be added depending on the machine

options.

If you want to define one of the fixtures or the raw part as a contour, this can be done

as well here in the setting manager (design your own chuck). You still need to set the

parameters for zero-point definition and transfer position in the "Parameter" tab.

A-D821UK-1_200420

13


1 | DMG Programmer 3D Turning

Memo

RG720 = dimension between front edge of jaw / collet and workpice zero point

RG712 = cut-off width + allowance

RG724 = jaw overtravel length sp.3

RG713 = machining compartment length sp4. to sp.3

14

A-D821UK-1_200420


1 | DMG Programmer 3D Turning

Memo

1

15

DMG Programmer 3D Turning

The appropriate parameters can be taken from the Help screen.

After the completion of setting data input, the sequence of operations can be defined.

Make sure the two channels contain the same number of machining processes. Operations

that do not contain machining processes are designated as NOP-OP and must

be defined accordingly.

A-D821UK-1_200420

15


1 | DMG Programmer 3D Turning

Memo

1.4 Defining operations

Each operation is stored in a separate program. In general, the first operation is defined

after the start program.

To do so, select the start program and open the pull-down menu by clicking the right

mouse button.

In this menu, select "New Operation".

The following screen form appears.

Depending on the machine type,

it is important to set the correct

operation templates

and planes.

RG720, RG722 (short part)

RG730 (X3 top)

RG823 (Z3 front)

The same applies when working

with the counter spindle and with

the tailstock.

Assign a name of your choice to the operation, e.g. Schruppen_sp4.

Check any further fields and adjust their contents if necessary.

16

A-D821UK-1_200420


1 | DMG Programmer 3D Turning

1.5 Defining a tool

The next input window requests a tool for the new operation.

Select the appropriate tool from the tool management list or define a new one.

Memo

1

17

DMG Programmer 3D Turning

Copy

tool

Delete tool

Import tool from

catalogue

Save selected tool

in file

Read in selected tool

from file

3D display

New

tool

Edit

properties

Move

tool

Tool

export

Tool export

Export all tools into

Excel file

channel/spindle specification

A-D821UK-1_200420

17


1 | DMG Programmer 3D Turning

Memo

1.5.1 Defining a new tool

Upon clicking "New Tool", the selection screen shown below appears.

3 4

1

2

5

6

Item

Description

1 Tool type selection

2 Cutting edge geometry

3 Prepare kit or use available kits

4

3D view of the selected tool. By selecting one of the radio buttons Cutter, Holder

or Clamp below the view, you can display only the view concerned. All selected =

entire list

5 Input of cutting edge geometry data

6 Input of tool parameter data

When all the parameters have been set, the tool is defined with OK. The newly

defined tool must now be selected. (Mark and select with OK.)

18

A-D821UK-1_200420


1 | DMG Programmer 3D Turning

Finally, the tool offset can be defined under "Tool correction".

Memo

1

19

DMG Programmer 3D Turning

A complete operation always consists of machining process and tool that are combined

to nodes which can be expanded using the "+".

Accept the entries by pressing OK.

A-D821UK-1_200420

19


1 | DMG Programmer 3D Turning

Memo

1.6 Executing a tool change sequence

The new operation has now been defined with the appropriate tool.

In the NC Code field, place the mouse pointer to the position where the tool

change process shall be inserted. (Here: block 11 - red cursor)

Select the tab "Common Macros".

Here, you will find common macros for turning and drilling operations as well as for

the insertion of tool changing processes.

Select the "Tool change" macro.

The following tool change screen appears.

20

A-D821UK-1_200420


1 | DMG Programmer 3D Turning

You can confirm the subsequent queries using the ENTER or TAB key.

Memo

1

21

DMG Programmer 3D Turning

With each confirmation with the Enter key, the appropriate program line (marked in

blue) is inserted in the lower field.

Finally, click "FINAL" to display the result which is inserted in the NC code by pressing

"OK".

A-D821UK-1_200420

21


1 | DMG Programmer 3D Turning

Memo

The NC code is inserted at the position selected beforehand.

Manual entry in NC editor

In the NC editor, data can also be entered manually. This e.g. may be helpful to face a

workpiece at high speed. To do so, go to the NC editor, select the desired position and

enter the NC code.

Example: Inserting a cutting cycle

Go to the Macros area.

Select the subitem Turn Cycles.

Select the cutting cycle CYCLE95.

The screen form for parameter definition appears.

22

A-D821UK-1_200420


1 | DMG Programmer 3D Turning

Memo

1

23

DMG Programmer 3D Turning

Define the values for the cycle and go to the next parameter using the ENTER key.

When the "FINAL" point has been reached, the cycle is inserted in the editor by

confirming with "Yes".

The NC code will then look as follows:

Finally, the contour must be defined.

Place the cursor at the positions between Begin and End labels and press the

common macro "Countour Definition".

A-D821UK-1_200420

23


1 | DMG Programmer 3D Turning

Memo

The displayed NC code is transferred to the editor and inserted between the Begin

and End labels by pressing OK.

The Contour elements Point, Line or Lines at an angle are used to define the contour.

At the end, the entire program can be renumbered using the "Numbering of lines"

macro.

24

A-D821UK-1_200420


2

Chapter

Simulation


2 | Simulation

Memo

2 Simulation

Select the Simulation item in the basic menu.

Simulation is loaded upon confirmation with "OK".

1

2

3

4

5

Item

Description

1 Toolbar used to control simulation

2 Status display per channel

3 Main simulation window

4 Program run display

26

A-D821UK-1_200420


2 | Simulation

2.1 Simulation toolbar

Memo

2

27

Single block F6

Fast forward F8

Reload Crl+R

Focus on collision

(active only in case of

collision)

Simulation

Start F7

Break F5

Focus on workpiece

Focus on machine

Feedrate and rapid

speed setting

Change detail degree

Measurement ON/OFF

Change view

Set contour

mode

Hiding mode ON/OFF

Half section ON/OFF

Insert

new view

A-D821UK-1_200420

27


2 | Simulation

Memo

2.2 Zooming, rotating and moving using the mouse buttons

Keep the left mouse button pressed and move the mouse in circles to the left:

rotating the simulation to the left.

Keep the left mouse button pressed and move the mouse in circles to the right:

rotating the simulation to the right.

Keep the right mouse button pressed (same function as the scroll wheel) and move

the mouse upwards: zooming in simulation.

Move the mouse down: zooming out simulation.

Scroll wheel: turn upwards -> zooming in simulation

Turn downwards -> zooming out simulation

Keep pressed -> Rotating around the machine axis to the right

or left.

Positioning of the mouse pointer and left double-click will move the point clicked towards

the simulation centre.

Keep both mouse buttons pressed: moving the machine to the right or left or up or

down.

28

A-D821UK-1_200420


2 | Simulation

2.3 Simulation settings

Memo

Simulation settings are stored related to the project When clicking the "Sensitivity"

item, a drop-down menu appears in which User-defined can be selected. Parameters

can now be enabled or disabled if desired.

2

29

Simulation

A-D821UK-1_200420

29


2 | Simulation

Memo

30

A-D821UK-1_200420


3

Chapter

Operation plan

manager


3 | Operation plan manager

Memo

3 Operation plan manager

The Operation plan manager is used to schedule operations and assign them to channel and

spindle.

The procedure is the same as described above for manual generation of operations -

with graphical channel and spindle display.

Procedure:

New workpiece

Workpiece settings

Operation plan manager

Creating operations

Create a new operation using "New".

Confirm with "Yes".

Define the channel.

As already described in the previous sections,

define the required settings. (Basic settings

and tool) Optionally, select NOP_OP for an

empty operation at this spindle/in this channel.

32

A-D821UK-1_200420


3 | Operation plan manager

Memo

3

33

The new operation is now defined in the operation plan designer. The synchronous

operation can be moved using the drag&drop function. By clicking the Edit icon, it can

be defined.

Operation plan manager

Define the synchronous operation by clicking the "Edit" icon.

You will be automatically enquired whether you want to define an empty operation. If

your answer is No, you will return to the known basic settings menu.

Icon

Description

Insert a new operation after an operation already programmed.

Delete operation

Insert a new line above the selected one with a simultaneous NOP_OP synchronous

operation.

Edit

A-D821UK-1_200420

33


3 | Operation plan manager

Memo

Define the entire workpiece operation and finally press "OK". The operation plan manager

is solely used to define the sequence of operations. Then, the appropriate cycles

and parameters for the machining process must be created.

Define the machining processes as described in the previous chapter.

34

A-D821UK-1_200420


4

Chapter

CAD / CAM


4 | CAD/CAM operations

Memo

4 CAD/CAM operations

4.1 Plane definition

The sequence of operations has been defined (through operation plan manager or

manually).

Open the first machining operation by double-click.

Select the geometry item.

A window appears in which the machining plane "Create new worlds" can be selected.

Operation

Rotation

Front

C/Y Surface

B/Y Axis

Y Front

Plane

Plane of rotation (G18)

Face milling, creates a TRANSMIT_S4 or S3 (G17)

Cylindrical interpolation, creates a TRACYL_S4 or S3 (G19)

B axis (G17)

Mechanical Y axis (G17)

36

A-D821UK-1_200420


4 | CAD/CAM operations

4.2 Computer-aided design (CAD)

Memo

For a turning contour, select the Rotation field. The following design screen appears.

1

2

3

4

37

CAD/CAM operations

Item

Description

1 Design toolbar

2 Design and machining sequence

3 Drawing plane

Icons

Description

Geometry generation:

Generation of auxiliary designs by means of

• Point definition

• Line definition

• Circle definition

Generate a contour:

• New contours, contour expansion, holes

• Macros: Undercut, recess, groove, circle and rectangle

• Point, line, arc, chamfers, radii

• Join with line, join with arc, close

Change a contour:

• Chamfers/radii, delete element, change radii, elongate

• Factor, offset, shift start / end, join/separate contour

• Working direction, soft on contour, attribute,

restore geometry elements

Edit:

Contours: Copy, mirror, shift, set zero point, rotate, delete

Measurement:

Contours: Measure distance, display element, measure

perimeter

A-D821UK-1_200420

37


4 | CAD/CAM operations

Memo

4.2.1 Setting the intersection snap function

Select the design surface by clicking the right mouse button. You can now select the

desired intersection snap options. This is always possible during the design process.

4.2.2 Creating a new contour

Select Contour new.

There are several ways of generating a contour.

By means of direct entry of the dimensions using F9.

By means of the Line contour definition.

Use Point definition to define the start point first

and then define the next contour point.

With the "Linie" contour definition, you can promptly verify the entered values since

they are immediately displayed. (green)

38

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

39

CAD/CAM operations

4.2.3 Form elements and undercuts

Form elements such as radii or chamfers are inserted once the actual contour has

been generated.

Press the Chamfer/Radius softkey and select the contour.

Then select the adjacent elements.

The information bar at the bottom of the screen contains accurate instructions about

how to execute the selected operation.

Press the Undercut softkey and select the shape.

Select the appropriate corner.

A window for data entry appears.

A-D821UK-1_200420

39


4 | CAD/CAM operations

Memo

Define the parameters and press

"OK".

4.2.4 Deleting elements

There are two possibilities to delete programmed elements:

Delete element

Delete it using the "Eraser".

Procedure

Select the contour.

Select the element to be deleted.

To delete the entire contour, select the eraser. Select the contour and confirm with

Enter. The contour is deleted.

40

A-D821UK-1_200420


4 | CAD/CAM operations

4.3 Generate operations in CAM

Memo

After the contour has been generated, the machining process must be defined

in the CAM area.

To do so, select the CAM tab.

The following screen appears.

4

41

CAD/CAM operations

Select the "CAM" item in the toolbar.

The screen form for raw-part definition appears.

If all the parameters have been correctly defined in the machine setting sheet beforehand,

they are automatically entered in the screen form for raw-part definition and

can be accepted.

A-D821UK-1_200420

41


4 | CAD/CAM operations

Memo

The defined raw part is laid over the programmed contour and highlighted by hatching.

Select "New Operation".

Select New Operation and assign

a name.

Confirm the selection with OK.

42

A-D821UK-1_200420


4 | CAD/CAM operations

A tool selection screen for the operation defined in the operation manager (here: drilling)

appears.

Memo

4

43

CAD/CAM operations

Select the appropriate tool and confirm the selection with "OK".

A pop-up menu appears. Here, the tool change process must be selected.

Confirm the selection with OK.

The tool change menu, that has already been described above, appears.

The tool change process is now displayed under the CAM operation "Drilling".

A-D821UK-1_200420

43


4 | CAD/CAM operations

Memo

Since the toolbar depends on the currently selected operation, only the cycles shown

here are enabled.

Drilling cycle

Approach/retraction cycles

Loading a

defined macro

Free movement and storage of the paths

Select a drilling cycle. The menu shown here appears:

Define the parameters and confirm the entry

with "OK". The cycle will also appear in the

tree structure below the defined tool.

The NC code function can be used to

show the selected cycle as NC code in

the side menu.

If you select the topmost operation, the entire

NC code for this operation is displayed.

44

A-D821UK-1_200420


4 | CAD/CAM operations

The 2D or 3D simulation function can be used to simulate any cycles already programmed

or the selected operation.

Memo

To do so, press 2D or 3D Simulation. The screen shown here

appears.

4

45

4.3.1 2D simulation

CAD/CAM operations

4

1

2 3

Item

Description

1 Simulation window

2 Start / Stop, Forward / Backward

3 Speed regulation

4 NC code moving along. The current block is highlighted (green).

A-D821UK-1_200420

45


4 | CAD/CAM operations

Memo

4.3.2 3D simulation

2

1

3

Item

Description

1 Simulation window

2 Select view X, Y, Z, Coordinate plane ON / OFF as well as various views

3 Start / Stop, Forward / Backward, speed regulation

4.3.3 Generating an NC code

Finally, the NC code must be generated. To do so, press the softkey for NC

code generation. A preview window containing the generated code appears.

If the NC code is ok, it can be entered

into the machining subroutine by pressing

the "Insert" button.

46

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

47

CAD/CAM operations

The operation can now be loaded into machine

simulation or displayed as an ISO file

Creating the subsequent operation:

Call the main screen and select the next operation.

Click Geometry and select the previous operation.

Upon confirmation, you will return to the CAM screen.

A-D821UK-1_200420

47


4 | CAD/CAM operations

Memo

4.4 Turning cycles

Once again, tool-dependent cycles are available. In this case,

you can select from cutting cycles for face machining and longitudinal machining.

Select Face Cut and enter the parameters in the screen form.

For roughing, start and end points on the contour must be defined first.

The selected start and end points are marked with a yellow circle. The selected contour

in between is marked in yellow as shown in the picture below. This is the selected

roughing contour.

After the selection of the end point, the parameter definition menu shown below

appears automatically.

48

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

Define the parameters and confirm the entry with "OK".

If the cycle shall be defined as Machine Cycle

(CYCLE95 in this example), check the appropriate check

box in this screen form.

4

49

When all the values have been entered, confirm the entry

with "OK". The machine cycle screen form appears.

CAD/CAM operations

You can exit the menu with "Ja" and then simulate the new operation just created.

Finally, generate the NC code. Repeat this procedure for each operation that follows.

A-D821UK-1_200420

49


4 | CAD/CAM operations

Memo

4.4.1 Hiding elements

It may become necessary to hide contour elements for a specific operation. The "Linear"

function is provided for this purpose.

Select the "Linear" option.

Call the context menu using the right mouse button and e.g. select

the "Intersection" function.

Snap the intersection.

Select the end point as the next element.

The contour to be hidden is displayed in yellow.

After the selection of the end point, the linear element just as the contour are displayed

in magenta.

Referring to the roughing cycle described above, the undercut is now hidden for the

roughing operation, i.e. undercuts are not realized.

Using "All Fade In, any hidden elements can be shown again. When

selecting a subsequent finishing cycle,

the elements that were hidden in the roughing cycle will be shown

again automatically.

50

A-D821UK-1_200420


4 | CAD/CAM operations

4.5 Operation on counter spindle

Memo

First, a tool must be defined for the B axis. See section 1.5.1.

The tool is defined in the same way as turret tools. That's why only the properties of

B-axis tools are described here.

4

51

CAD/CAM operations

Function

Tool T

Tool name

Tool offset

Milling 1 / Turning 2

Tool position

B and C

Description

Opening the tool parameters

Can be defined under the tool parameters

1-4, depending on the defined cutting edge

Definition of whether the tool is clamped (2) or not (1 = milling operation)

Definition of the B and C axis angles of the tool. Using the "Open" button

, a help window appears in which the entered data are visualized

in the form of a graph.

A-D821UK-1_200420

51


4 | CAD/CAM operations

Memo

4.5.1 Generating the contour for counter spindle

Under "Geometry", select spindle 3 and confirm the selection with "OK".

The choice of machining geometries is displayed.

Here, select the "Rotation" item and confirm the selection with "OK".

The design window for contour definition appears.

Define the desired contour using construction lines in accordance with exercise 2

in the Annex.

52

A-D821UK-1_200420


4 | CAD/CAM operations

4.5.2 Construction lines

Memo

Construction lines are used to define diameters and Z end points with the aid of vertical

and horizontal lines in order to generate intersections which are used later to define

the contour.

The function can be called via "Line" or F9.

4

53

CAD/CAM operations

In the sub-menu of the "Line" function (click the small black arrow), the functions

shown can be called directly.

Once all the construction lines have been defined, describe the contour

geometry using "New contour". First, however, select "Intersection" in the context

menu of the right mouse button.

A-D821UK-1_200420

53


4 | CAD/CAM operations

Memo

Confirm the entries by pressing OK. The defined

recess can then be picked up by mouse click and positioned

using F9 (direct specification of dimensions).

Use the intersections to define the contour. Furthermore, the direct specification of

dimensions can be enabled with F9.

At the end, define the form elements according to the drawing by means of the

"Chamfer/Radius" function.

54

A-D821UK-1_200420


4 | CAD/CAM operations

4.6 Recesses

Memo

Using the "Recess" function, you can define the recess parameters in the

called screen form.

4

55

CAD/CAM operations

The completed contour is as follows:

A-D821UK-1_200420

55


4 | CAD/CAM operations

Memo

The contour described should now be loaded into the CAM area.

Use "CAM" to load the contour into the CAM area.

Answer the enquiry "Rohteil aus bestehender Operation laden" with "Ja".

An overview of the operations already defined on the main spindle appears. Select

the last operation (Schruppen_Innen in this example) and confirm the selection

with "OK".

The operations already programmed are laid over the new contour and highlighted by

hatching.

56

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

57

CAD/CAM operations

4.7 Generating an operation in channel 1 with B axis

Select "New Operation".

Insert a tool change process.

When the tool change has been executed, the window used to define cutting edge

position, machining direction as well as clearance angle and lead angle appears

automatically.

2

1

Item

Description

3

1 Cutting edge position

2 Machining direction

3 Setting angles

4

4 Help view

Define all the machining data for the counter spindle.

Hide the recess for roughing and finishing and the undercut for roughing.

A-D821UK-1_200420

57


4 | CAD/CAM operations

Memo

4.7.1 Recess machining

Insert a tool change process.

Define a new tool orientation.

Open "Recess".

The shown selection window appears.

Here, you can select how the recess tool shall recess referring to the defined cutting

edge.

Define the start and end points of the recess in the contour.

The screen form for parameter definition automatically appears.

58

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

59

Define the contour extension mode here and

define the start and end points in the subsequent

step in the contour editor.

CAD/CAM operations

At the end, the screen form used to enter the entry and exit movements of the tool appears.

A-D821UK-1_200420

59


4 | CAD/CAM operations

Memo

4.8 Thread definition

Threads are solely defined in the editor.

Select the "Turn Cycle" macro under Common Macros. The sub-menu contains

the item Thread cutting (G97).

First, generate a tool change process.

Call the thread cutting cycle. The following screen form appears.

60

A-D821UK-1_200420


4 | CAD/CAM operations

4.9 Milling operation

Memo

Exercise 4 explains some of the usual milling operations.

Use a "New Operation" to select and define the selection dialog for the machining

plane.

4

61

CAD/CAM operations

After having entered all parameters, the ToolManager automatically appears. Here, you

can define a new milling cutter (D=20 mm) as shown in the figure.

A-D821UK-1_200420

61


4 | CAD/CAM operations

Memo

Accept the tool setting.

Define the

tool offset

under "Tool

correction"

and confirm

the entry

with "OK".

Go to the CAM module and define the machining plane.

The rectangle to be generated can be generated by means of the "Square" function.

However, it can also be designed with the aid of construction lines. Since a hexagon

remains to be generated later, the design approach shall be explained here.

Design the square as shown below.

62

A-D821UK-1_200420


4 | CAD/CAM operations

Define the square using the intersection snap function as already described above.

Memo

4

63

CAD/CAM operations

The arrow on the square specifies the machining direction. It thus defines whether

down-cut milling or up-cut milling shall be adopted, If down-cut milling is executed, as

is done in this example, it can be reverted with the "Workdirection" function.

A-D821UK-1_200420

63


4 | CAD/CAM operations

Memo

Go to the CAM module and define the machining plane.

Execute a tool change process.

Select the "Contour Milling" cycle.

Select the desired contour.

Define the start and end points. (They are congruent in our example.)

The screen form for parameter definition appears.

64

A-D821UK-1_200420


4 | CAD/CAM operations

Now define the approach and retraction movements. First, however, you should

select the contour extension method.

Memo

4

65

CAD/CAM operations

Now define the points on the contour.

The milling cycle can now be simulated.

Finally, generate the NC code.

A-D821UK-1_200420

65


4 | CAD/CAM operations

Memo

4.9.1 Chamfering face contours

Use a "New Operation" to select and define the selection dialog for the machining

plane.

Define an NC spot drill.

Enter the appropriate tool settings.

Go to CAM area.

Select the previous operation.

The square is loaded.

Call the design mode (F6).

Select the "Contour allowance" option and define the

machining side and the distance.

The offset is generated.

66

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

67

CAD/CAM operations

Go to CAM area.

Generate a new operation.

Execute a tool change process.

Select the desired tool.

Select the the milling cycle.

Define the contour and enter the parameters as shown in the figure.

A-D821UK-1_200420

67


4 | CAD/CAM operations

Memo

Define the approach and retraction movements.

Now, the simulation can be executed.

Generate the NC code.

4.10 Face drilling

Use "New Operation" to select and define the selection dialog for the machining

plane.

Define a drill with D=8.5 mm.

Enter the appropriate tool settings.

Go to CAM area.

Insert a tool change process.

68

A-D821UK-1_200420


4 | CAD/CAM operations

Select the "Drilling Front C-Axis" macro under "Common Macros".

Memo

The following screen form appears; here, enter the data specified in the drawing.

4

69

CAD/CAM operations

Accept the entries.

The NC code is inserted in the editor.

A-D821UK-1_200420

69


4 | CAD/CAM operations

Memo

4.11 Milling using mechanical Y axis

Use "New Operation" to select and define the selection dialog for the machining

plane.

Define a mill with D=50 mm.

Enter the appropriate tool settings.

Call the editor.

Insert a tool change process.

Position the C axis at 90° (G0 C4=90 M412).

The shift must be programmed next.

Open the "Shift" subroutine and jump to a vacant position in the subroutine.

Use the macro "Commands for displacement" to insert a new

shift in the editor. The input menu shown below

appears.

70

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

71

CAD/CAM operations

Assign a name to the shift and confirm the entries. Only the ATRAS and AROT

commands are inserted in the editor.

The shift values must be entered manually in the editor. When doing so, make sure that

"Z" is selected as the infeed axis.

Go to the surface milling operation.

Use the "Shift" macro -> "Shift choose" to call the shift, that has been defined

previously, in the editor.

A-D821UK-1_200420

71


4 | CAD/CAM operations

Memo

Call the already programmed shifts in the first input field by pressing the Return or

Enter key.

Confirm the entries by pressing "OK".

The shift is inserted in the editor.

Finally, the traverse movement must be programmed.

72

A-D821UK-1_200420


4 | CAD/CAM operations

4.12 Pocket milling using the CAM function

Memo

Use "New Operation" to select and define the selection dialog for the machining

plane.

Define an 8 mm mill.

Enter the appropriate tool settings.

Go to the CAM area.

Select "None" in the "Previous operation" dialog.

Select B-Axis in the "Create new worlds" dialog.

4

73

CAD/CAM operations

Assign a name to the operation. It can be changed at will, e.g. to Pocket.

In the design window, select "Circle" and enter the circle diameter.

Select the intersection function and arrange the circle with its centre at the intersection

of the coordinate axes (0/0).

A-D821UK-1_200420

73


4 | CAD/CAM operations

Memo

Since the pocket milling function is not yet available at the moment, the contour milling

cycle with allowance must be used and programmed repeatedly.

Select "New Operation" in the CAM window.

Tool selection.

Execute the tool change process.

Select the contour milling cycle.

Select the contour and define the start and end points.

Define the parameters as shown below.

74

A-D821UK-1_200420


4 | CAD/CAM operations

In the last step, set the allowance to "0" (under "Overmeasure").

Check the check box "Insert last values".

Memo

4

75

CAD/CAM operations

Apply the data and confirm the "Clamp C axis" enquiry.

Finally, simulate the operation and generate the NC code.

Then manually enter the C-axis position into the editor and define the shift.

A-D821UK-1_200420

75


4 | CAD/CAM operations

Memo

4.13 Y-axis machining – direct programming on

turret machines (recess)

Select New Operation and set the G19 machining plane (Driven surface).

Apply the entries by pressing OK.

76

A-D821UK-1_200420


4 | CAD/CAM operations

Define a new tool for lateral surface machining. Cutter head D=30.

Memo

4

77

CAD/CAM operations

Select the operation and confirm the enquiry regarding tool change by pressing

Yes.

A-D821UK-1_200420

77


4 | CAD/CAM operations

Memo

The actual machining process is now inserted below the technology. Make sure the Y

axis is returned to 0 after the machining process; otherwise, the X axis would reach the

software limit switch when it is moved to the TCP. Moreover, the C axis should be positioned

and additionally be clamped.

78

A-D821UK-1_200420


4 | CAD/CAM operations

4.13.1 Y-axis machining – programming on turret machines using CAD/CAM

(circular pocket)

Memo

4

79

CAD/CAM operations

Select New Operation and set the G19 machining plane (Driven surface).

Apply the entries by pressing OK.

A-D821UK-1_200420

79


4 | CAD/CAM operations

Memo

Define a new tool for lateral surface machining. End mill D=8.

Select the operation and answer the enquiry regarding tool change with No.

Go to the geometry settings function.

Create a new world with the following settings: Y-Surface, C=180, Dist. from centre=20

and Depth plane (absolute)=15.

Confirm both enquiry dialogs by pressing OK. The CAD/CAM view with the Surface

plane appears.

80

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

81

CAD/CAM operations

1

1 = Coordinate system for Y surface machining

Select the circle macro in the design window.

Enter the pocket radius.

Position the circular pocket with F9.

Go to CAM area.

Define the raw part.

Select tool change as new operation.

Mill the pocket.

Select the pocket and confirm it with Enter.

A-D821UK-1_200420

81


4 | CAD/CAM operations

Memo

Define the pocked based on the drawing.

Confirm the 4. Axis Clamp enquiry with OK.

Finish the procedure with a simulation with the entered data.

82

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

83

CAD/CAM operations

Generate the NC code.

Insert the NC code in the machining process.

Go to 3D Simulation and check the programming as well as the

traversing paths.

A-D821UK-1_200420

83


4 | CAD/CAM operations

Memo

4.14 Cylindrical interpolation

Select New Operation and set the G19 machining plane (Driven surface).

Apply the selection with OK.

Define a new tool for lateral surface machining. End mill D=8.

84

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

85

CAD/CAM operations

Select the operation and answer the enquiry regarding tool change with No.

Go to the geometry settings function.

Create a new world with the following settings: C Surface D=60.

Confirm both enquiry dialogs by pressing OK. The CAD/CAM view with the Surface

A-D821UK-1_200420

85


4 | CAD/CAM operations

Memo

1

plane appears.

1 = Coordinate system for C surface machining

Select "Interactive" in the "Line" menu.

Define the groove insertion point with F9.

Use the longitudinal groove to define the groove based on

the drawing.

Define the groove type.

Position the groove centre by means of the "Intersection" snap mode.

86

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

87

CAD/CAM operations

4.14.1 Groove without macro

If you want to generate a groove without macro, proceed as follows:

Define the groove insertion point, parallel lines and auxiliary circles.

A-D821UK-1_200420

87


4 | CAD/CAM operations

Memo

Define a new contour with the right mouse button and define the intersection as the start point.

Change over to the object mode.

Select contour elements.

Go to CAM area.

Define the raw part.

Select tool change as new operation.

Mill the groove.

Select the groove.

Define the insertion point (upper or lower centre point).

88

A-D821UK-1_200420


4 | CAD/CAM operations

Memo

4

89

CAD/CAM operations

Enter the cycle data based on the drawing.

Finish the procedure with a simulation with the entered data.

Generate the NC code.

Insert the NC code in the machining process.

Go to 3D Simulation and check the programming as well as the

traversing paths.

A-D821UK-1_200420

89


3 | CAD/CAM operations

Memo

90

A-D821UK-1_200420


5

Chapter

Machining with

tailstock 4A TWIN


4 | Machining with tailstock on the 4A TWIN machine model

Memo

5 Machining with tailstock on the 4A TWIN machine model

5.1 Case 1 Machining on long zero point

This section describes the generation of standard machining processes with tailstock

centre sleeve in Programmer, provided that there is still no appropriate template program.

In the first variant, we will show a structure without structure at the part advanced.

First, define a new project.

Select the model.

First, choose an appropriate model from the TEMPLATE folder. When doing so, please

observe bar loader and remnant disposal.

In addition to the usual set-up parameters, a tailstock centre and other tailstock-related

data must be input.

92

A-D821UK-1_200420


4 | Machining with tailstock on the 4A TWIN machine model

Call the workpiece settings and go to the tailstock settings.

Memo

The structure that is now available must be supplemented by the standard centre sleeve

machining processes. In general, these processes are:

Channel1: - Pre-positioning of X3 and Z3

- Machining at Sp3 or Sp4.

Channel2: - Centring at Sp4

- Centre sleeve advance at Sp4

- Machining with tailstock centre at Sp4

- Centre sleeve retraction at Sp4

RG771 = workpiece-specic centre sleeve stroke

RG772 = tolerance window

RG774 = depth of penetration of centre sleeve

into the workpiece

RG771 = feed distance

5

93

Machining with tailstock on the 4A TWIN machine model

The first machining process in

channel 1 moves the X3 axis upwards

and advances the Z3 axis

to the supporting position.

Make sure RG730 and the correct

template program are called.

A-D821UK-1_200420

93


4 | Machining with tailstock on the 4A TWIN machine model

Memo

Now, program the following machining operations in the channel.

Then advance the centre sleeve using a new template.

The first actual machining process can now be executed at the main spindle. In our example,

this is a simple roughing process. For this process, program Longitudinal Machining.

As a last standard machining process, the centre sleeve is retracted. For this process

as well, there is an appropriate operation template. Once again, the subsequent tool

selection is suppressed.

The finished operation plan for channel 2 will be as follows:

94

A-D821UK-1_200420


4 | Machining with tailstock on the 4A TWIN machine model

Memo

5

95

Machining with tailstock on the 4A TWIN machine model

Finish the procedure with a simulation of all steps.

A-D821UK-1_200420

95


4 | Machining with tailstock on the 4A TWIN machine model

Memo

The generated program can be saved as a template in the program manager. To do so,

click the program with the right mouse button and select "Create template".

The new template is then automatically saved in the Templates field.

5.2 Case 2 Short zero point

In this section, we will present a bar machining process using centre sleeve and centring

on a short part that has not been advanced yet. Topics such as positioning of X3 / Z3 or

advance and retraction of centre sleeve will not be discussed in further detail here. The

template previously created will be used as a basis for the new program.

Define a new project to be able to perform the changes; here, select the "Langer

Nullpunkt" template.

In V-INIT, define the calculation of the short zero point.

Select the short zero point (RG722) for facing and centring in the existing program.

96

A-D821UK-1_200420


4 | Machining with tailstock on the 4A TWIN machine model

Memo

5

97

Define a new operation to advance the material.

Confirm the entry with OK and select the bar stop as the tool.

Machining with tailstock on the 4A TWIN machine model

Delete the marked standard lines from the defined program.

A-D821UK-1_200420

97


4 | Machining with tailstock on the 4A TWIN machine model

Memo

Cut the marked contents from "Material in Hauptspindel" by pressing Ctrl+X and

paste them in "Material_Vorschieben".

Now, add the following NC blocks to the operation "Material in Hauptspindel"´.

Simulate the program.

Finish the procedure by saving the program as a template.

98

A-D821UK-1_200420


6

Chapter

4-axis

machining


4 | 4-axis machining

Memo

6 4-axis machining

The machining at the main spindle using slide 1 for face and longitudinal roughing operations

and slide 2 for drilling operations serves as an example.

Make sure machining is only possible with the spindle rotating in one direction!

100

A-D821UK-1_200420


4 | 4-axis machining

Tool selection for channel1:

When using a right-hand cutting drill for channel 2, we will

need the direction of rotation 3 Clockwise (CW). For TC

machines, the right-hand roughing tool is swivelled to the

correct position with B1=90 and C1=180.

Memo

!!! For the technology input, the identical rotation value and

the same direction of rotation must be used by all means.

6

101

4-axis machining

The tool for channel 2 is a drill with D=20.

A-D821UK-1_200420

101


4 | 4-axis machining

Memo

2 machining programs in channel 1 and channel 2 are obtained in this way. They are

inserted and highlighted in red; this does not indicate a fault but shall hint to the fact that

this machining is a 4-axis machining process.

First, create the machining processes in the appropriate programs, independent of each

other. Use CAD/CAM for roughing and the fixed cycles for drilling. You will obtain two

machining programs. In general, a collision will be detected during the simulation.

102

A-D821UK-1_200420


4 | 4-axis machining

Memo

6

103

4-axis machining

To avoid this collision, wait marks must be inserted to synchronize both channels.

Call the waitmarks manager in the program management screen.

First, select the two programs to which wait marks shall be assigned in the upper two

windows.

Icon

Description

From the left to the right:

Insert new wait mark, delete wait mark, indicate Wait in the other

channel, shift wait mark upwards/downwards

A-D821UK-1_200420

103


4 | 4-axis machining

Memo

Select the block behind which the new wait mark shall be inserted.

Insert a new wait mark.

Select an arbitrary wait mark and confirm the selection with OK.

The new wait mark is inserted and marked in red.

Use the same procedure to insert the wait mark in channel 2 of the respective program.

The wait mark used in channel 1 is highlighted in yellow.

104

A-D821UK-1_200420


4 | 4-axis machining

Once the insertion is finished, this wait mark as well can be seen in the program.

Memo

5

105

4-axis machining

The inserted wait marks will automatically be written into the dummy program.

Machining result with wait marks in 3D simulation:

A-D821UK-1_200420

105


4 | 4-axis machining

Memo

106

A-D821UK-1_200420


7

Chapter

Raw part definition


4 | Defining the raw part

Memo

7 Defining the raw part

Caution: This example applies to the TC machine series!

For smaller machines, use smaller values for workpiece setting..

Call the workpiece settings.

Once having defined a clamping means, select one of the raw parts highlighted in red

from the list of the specified raw parts, change its name and save it.

108

A-D821UK-1_200420


4 | Defining the raw part

Use the edit function to edit the values in Profil Editor.

Memo

7

109

Delete all existing values.

Defining the raw part

Now, enter the raw part dimensions from the drawing into the table Here, it should be

observed that the zero point must be on the left-hand side of the finished part and that

all other dimensions refer to it!! Make sure the X-axis coordinates are specified as a

radius value.

Please do not forget to adjust the RG parameters to your modifications!

The 3D representation of the raw part can be rotated using the mouse.

A-D821UK-1_200420

109


4 | Defining the raw part

Memo

Apply the dialog with OK.

Once all setting data have been input, you should check the result in the object simulation.

This procedure can also be used to design your clamping means such as chuck, collets,

jaws, tailstock centre (if available), etc. at will.

110

A-D821UK-1_200420


4 | Defining the raw part

7.1 Creation of the raw part in the CAD/CAM module

Memo

De ne a new operation under the name "Raw Part".

7

111

Defining the raw part

Uncheck the check box "Managed from main program".

Finish the procedure by loading an operation and selecting CAM.

The contour is created by CAD. Important: It must be created and saved in positive

direction.

In the menu "NC-Code erzeugen", select Transform All.

A-D821UK-1_200420

111


4 | Defining the raw part

Memo

For their application in the machine setting sheet, the NC blocks must be marked and

copied.

Call the workpiece settings.

Select a raw part marked in red, rename it and then click Edit.

Delete all values.

Click the ISO import function.

Paste the copied code.

Apply the entries.

112

A-D821UK-1_200420


4 | Defining the raw part

7.2 Reading in the raw part as STL

Memo

Workpieces with finished programming can be saved in Programmer as STL files and

continued to be used for instance as raw part.

Have the component processed in the simulation function.

7

113

Defining the raw part

By setting the camera accordingly, the finished component can be viewed - it is

located behind the machine.

File -> Export workpiece as .stl -> Selection of machining process -> Select storage

location

A-D821UK-1_200420

113


4 | Defining the raw part

Memo

7.2.1 Loading of the STL file as raw part

Call the workpiece settings.

Check the item "External Workpiece".

Load the .stl file.

Adjust the coordinate system for machining (set axis).

Confirm the entries with OK and then perform a simulation.

114

A-D821UK-1_200420


3x45˚

70˚

8

R2

R2

35

M16

25

58

DIN 76 – A

A

1 2 3

4

Übung 1

Rohteil: Ø 60x78

25

SW28

A

Übung 5

1 2 3

4

Rohteil: Ø 120x104

B

A

B

A

Übung 4

Rohteil: Ø 80x78

A

B

2 3

43

30

1 4

C

B

C

76

A

B

C

C

D

B

unbemaßte Fasen = 1x45°

D

C

unbemaßte Radien = 1

D

unbemaßte Fasen = 1x45°

unbemaßte Radien = 1

E

D

C

D

unbemaßte Fasen = 1x45°

unbemaßte Radien = 1

DIN ISO 13715

-0,4

+0,4 Allgemeintoleranz ISO 2768-m

E

E

Verantwortl. Abt. Technische Referenz Erstellt durch Genehmigt von

F

DMG-TA

DMG-TA

DIN ISO 13715

Dokumentenart

Fertigungszeichnung

Titel, zusätzlicher Titel Material

DMG-TA

E

Verantwortl. Abt. Technische Referenz Erstellt durch Genehmigt von

Dokumentenstatus

freigegeben

D

E

F

DIN ISO 13715

DMG-TA

-0,4

1

+0,4 Allgemeintoleranz ISO 2768-m

Dokumentenstatus

DMG-TA

Dokumentenart

Fertigungszeichnung

freigegeben

Verantwortl. Abt. Technische Referenz Erstellt durch Genehmigt von

F

Übung 1

Änd.

EN AW-Al Cu 4 PB Mg

-0,4

Ausgabedatum

2

3

4

EN AW-Al Cu 4 PB Mg

Titel, zusätzlicher Titel Material

Änd. Ausgabedatum

Chapter

1

2

Übung 5

3

1

Spr.

de

4

Blatt

1

F

2

+0,4 Allgemeintoleranz ISO 2768-m

Spr.

de

DMG-TA

Dokumentenart

Fertigungszeichnung

Blatt

Titel, zusätzlicher Titel Material

Übung 4

3

1

F

Änd.

Dokumentenstatus

freigegeben

EN AW-Al Cu 4 PB Mg

Exercises 8

Ausgabedatum

Spr.

de

4

1

Blatt

F

E


1 2 3

4

A

A

Raw part 115 x 70

B

B

C

C

D

D

E

E

DIN ISO 13715

-0,4

+0,4 Allgemeintoleranz ISO 2768-m

Verantwortl. Abt. Technische Referenz

Erstellt durch

DMGMORI AC

DMGMORI AC

Genehmigt von

F

1

2

Dokumentenart

Fertigungszeichnung

Titel, zusätzlicher Titel

Exercise 1

3

Dokumentenstatus

freigegeben

Material

EN AW-Al Cu 4 PB Mg

Änd. Ausgabedatum Spr.

de

4

Blatt

1

F

116


1 2 3

4

A

Raw part 160 x 78

A

8 H7

B

B

8

117

C

C

Defining the raw part

Exercise 2b

∅110x78

Raw part 110 x 78

8 H7

D

D

E

E

DIN ISO 13715

-0,4

+0,4 Allgemeintoleranz ISO 2768-m

Verantwortl. Abt. Technische Referenz

Erstellt durch

DMGMORI AC

DMGMORI AC

Genehmigt von

F

1

2

Dokumentenart

Fertigungszeichnung

Titel, zusätzlicher Titel

Exercise 2

3

Dokumentenstatus

freigegeben

Material

EN AW-Al Cu 4 PB Mg

Änd. Ausgabedatum Spr.

de

4

Blatt

1

F

117


1 2 3

4

A

Raw part 115 x 70

A

B

B

C

C

D

10 tief

D

E

E

DIN ISO 13715

-0,4

+0,4 Allgemeintoleranz ISO 2768-m

Verantwortl. Abt. Technische Referenz

Erstellt durch

DMGMORI AC

DMGMORI AC

Genehmigt von

F

1

2

Dokumentenart

Fertigungszeichnung

Titel, zusätzlicher Titel

Exercises 3 and 4

3

Dokumentenstatus

freigegeben

Material

EN AW-Al Cu 4 PB Mg

Änd. Ausgabedatum Spr.

de

4

Blatt

1

F

118


1 2 3

4

A

A

7.5 tief

B

B

8

119

C

C

Defining the raw part

4 tief

D

D

E

E

DIN ISO 13715

-0,4

+0,4 Allgemeintoleranz ISO 2768-m

Verantwortl. Abt. Technische Referenz

Erstellt durch

DMGMORI AC

DMGMORI AC

Genehmigt von

F

1

2

Dokumentenart

Fertigungszeichnung

Titel, zusätzlicher Titel

Exercises 4b and c

3

Dokumentenstatus

freigegeben

Material

EN AW-Al Cu 4 PB Mg

Änd. Ausgabedatum Spr.

de

4

Blatt

1

F

119


1 2 3

4

A

A

B

B

C

g

C

D

D

E

E

DIN ISO 13715

-0,4

+0,4 Allgemeintoleranz ISO 2768-m

Verantwortl. Abt. Technische Referenz

Erstellt durch

DMGMORI AC

DMGMORI AC

Genehmigt von

F

1

2

Dokumentenart

Fertigungszeichnung

Titel, zusätzlicher Titel

Exercises 5 and 5b

3

Dokumentenstatus

freigegeben

Material

EN AW-Al Cu 4 PB Mg

Änd. Ausgabedatum Spr.

de

4

Blatt

1

F

120


1 2 3

4

A

A

B

B

8

121

C

C

Defining the raw part

D

D

E

E

DIN ISO 13715

+0,4 -0,4 Allgemeintoleranz Raw part 75 x ISO 78 2768-m

Verantwortl. Abt. Technische Referenz

Erstellt durch

DMGMORI AC

DMGMORI AC

Genehmigt von

F

1

2

Dokumentenart

Fertigungszeichnung

Titel, zusätzlicher Titel

Exercise 6

3

Dokumentenstatus

freigegeben

Material

EN AW-Al Cu 4 PB Mg

Änd. Ausgabedatum Spr.

de

4

Blatt

1

F

121


Memo

122

A-D821UK-1_200420


T M336 G153 G96 G95 G94 WA

NS DIAM90 DIAMON EXTERN G0 G2 G3

ET M336 G153 G96 G95 G94 WAITS WAITP TURN

G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G

RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPC

TRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS

F S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G

G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G5

OF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94

OT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G

PCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 W

40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59

SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94

AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTER

S SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G9

6 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58

POS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G

AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EX

SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95

G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G

SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G

AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMO

SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96

G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G

SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G9

T ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIA

M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153

5 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G5

N EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 D

59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55

TURN TRAORI SPOS SPCOF S

4 G17 G18 G19 AC() AROT ATRANS DIA

P TURN TRAORI SPOS SPCOF S RET M336 G153 G

G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58

TP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAIT

3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4

WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TR

70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G2

WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCO

G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS

TS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G15

63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57

AITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 W

G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3

WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN

9 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G

4 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI

RN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19

94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI

8 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5

G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI

EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19

95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI

G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5

5 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI

0 G2G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19

TP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAORI SPOS SPCOF S RET M336 G153 G96 G95 G94 WAITS WAITP TURN TRAOR

GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94

AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18 G19 AC() AROT ATRANS DIAM90 DIAMON EXTERN G0 G2 G3 G4 G17 G18

G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG94 G5G26 G40 G41 G42 G54 G55 G56 G57 G58 G59 G63 G70 G71 G90 GG

Chapter

G codes 9


9 | G codes

Memo

9 G codes

9.1 Syntax explanation

For syntax explanation, we are using the following notation.

Syntax

Gxy

X

[Y]

A|B

C/D

[X=foo]

Description

X [Y] A|B C/D (E [F|G])|H

The reference G code xy in question

a mandatory code word

an optional code word

either A or B; one of these two codes must be programmed

C, D or both of them; at least one of these two codes must be programmed

X is optional; the standard value is foo

Example:

(E [F|G])|H either H or (E and optionally, (either F or G))

This syntax notation is also used for other command types (if necessary).

The supplementary remark "without effect in simulation" refers to commands that are

ignored during simulation. If required and technically feasible, they can be implemented

later.

124

A-D821UK-1_200420


9 | G codes

9.2 High-level language and G codes relating to Programmer

Memo

AC()

AROT

ATRANS

C

D

DIAM90

DIAMON

EXTERN

G0

G1

G2

G3

G4

G17

G18

G19

G26

G41

G42

G54

G55 to G57

G58

G59

G63

G70

G74

located.

G94

Absolute programming for axes (X,Y,Z,C,...) and lengths (I,J,K,...) is not

yet supported.

Order of Z,Y,X rotations. No restriction regarding the

value range.

Zero offset for c axes restricted to the current machining spindle.

Programming with rapid speed only. DC, ACP, ACN are not supported.

Infeed always along the shortest path.

If the selected compensation has not been defined, it has the same

effect as D0 (without compensation).

Standard setting; cannot be deselected.

Is only effective for absolute programming.

Procedures are registered and reloaded from the template_twin500.tnc

file if necessary.

Rapid speed programming of linear and rotary axes is permitted within

a block but is fragmented in two blocks for simulation. In this case, the

rotary axes are fed in first, G0 B180 X100 is converted to G0 B180 \n

G0 X100. The C axis of the current machining spindle is the sole axis

that can be programmed. The same is true for the movement of the

counter spindle with Z3, provided that it is not programmed in a separate

block.

Linear interpolation of Z3 and another axis - is not supported at the moment.

Arcs can be programmed by specifying both the centre point and the

radius. Centre points are always incremental, i.e. G2 X100 I=AC(10)

corresponds to G2 X100 I10. Full circles with centre point programming

are not supported yet.

See G2

Dwell in number of rotations (G4 S10) is not supported.

Is not enabled until spindle 1 or 2 has been activated.

Turns off TRANSMIT and TRACYL.

Turns off TRANSMIT and TRACYL.

Is not enabled until spindle 1 or 2 has been activated.

One speed limit only may be programmed per block.

Changeover of compensation or modification of the offset value not

until the compensation function has been deselected meanwhile.

See G41

Effect for FINE shift not yet clear

See G54

One C-axis zero offset only is accepted per block. Zero offsets of the

B and Z3 axes are not possible.

See G58

Is modal

Will be fully supported only in the inch version.

Implementation after having clarified where the reference points are

In one block, only the C axis of the current machining spindle or that of

the milling spindle can be approached..

Disables G96 internally, i.e. G94 corresponds to G94 G97. Has only an

effect on the linear axes but not on the rotary axes.

9

125

G codes

A-D821UK-1_200420

125


9 | G codes

Memo

G95 Disables G96 internally, i.e. G95 corresponds to G95 G97.

G96

Enables G95 internally and then may apply the feedrate value in mm/

min.

G153 The reference point in channel 1 (milling spindle) is the centre of rotation

of the B axis and that in channel 2 (disc-type turret) is the tool

mounting.

GOTOB Jump is omitted if the specified label does not exist. A distinction

between jump in forward and backward direction is not made, i.e. GO-

TOB and GOTOF can be used both to jump forwards and backwards.

GOTOF See GOTOB

IC()

Incremental programming is supported for axes (X,Y,Z,C,...) but not for

lengths (I,J,K,...) and the axis of counter spindle Z3.

IF

Condition may only contain arithmetical comparisons of numbers and

'normal' variables. Enquiries e.g. about the machine status or system

variables are not possible. The conditional execution is limited to jump

commands.

L

Jump is omitted if the specified subroutine does not exist. The nesting

depth is not controlled. At the moment, parameter transfer is supported

only for standard subroutines from template_twin500.tnc. The

SAVE option and the repeated run of a subroutine when being called

are not supported.

M336 The chuck is unclamped /even with the spindle running). The spindle

is not clamped, i.e. M336 has the same function as M333.

RET Works in the same way as M17.

S

Assignment of the spindle speed to the active spindle only

(see SETMS)

SPCOF Only the current machining spindle can be addressed.

Position control for spindles 1 and 2 (driven tools) has no effect during

simulation.

SPOS Only the current machining spindle can be addressed.

Position control for spindles 1 and 2 (driven tools) has no effect during

simulation.

126

A-D821UK-1_200420


9 | G codes

9.2.1 Commands not supported (examples)

Memo

The following NC commands are not implemented. If required and technically feasible,

they can be implemented later (if required for specific machine models).

General commands:

ACN

Absolute dimensions for rotary axes, negative direction of rotation

ACP

Absolute dimensions for rotary axes, positive direction of rotation

AMIRROR

ANG

AP

AR

ASCALE

CASE

CHF

CHR

CIP

DC

DITE

DITS

FA

FFWOF

FGROUP

FL

FXS

MIRROR

P

POS

POSA

POSP

REPEAT

REPEATB

RND

RNDM

RP

MRP

SCALE

SETAL

SUPA

TOFRAME

TRAANG

TRAORI

TURN

WAITP

WAITS

Mirror image on the specified axis is not supported yet. The assignment

of MD10610 and MD 10612 is not clear.

Contour angle

Polar angle when programming with polar coordinates

Opening angle for arcs

Scaling of the specified axes

Branching

Length of chamfer for contours

Length of chamfer in direction of movement for contours

Circular interpolation via intermediate point

Absolute dimensions for rotary axes, shortest path

Thread run-out path

Thread run-in path

Axial feed

Pilot control OFF (by analogy, FFWON)

Feedrate value applies all axes specified

Limit speed for synchronous axes

Retraction from fixed stop ON (by analogy, FXST, FXSW)

Mirror image on the specified axis is not supported yet.

The assignment of MD10610 and MD 10612 is not clear.

Repetitive call of subroutines

Positioning of the specified axis (axes) without block advance

Positioning of the specified axis (axes) with block advance

Positioning of the specified axis (axes) via intermediate points

Repetitive execution of a specific part of the program

Repetitive execution of the specified block

Contour corner rounding

Contour corner rounding (modal)

Polar radius when programming with polar coordinates

Rotation of machining plane with ROT or AROT

Scaling of the specified axis (axes)

Setting an alarm

Disabling all zero offsets block by block

Frame generation after tool orientation

Transformation to inclined axis

three, four and five-axis transformation

Selection of additional circular passes for G2/G3

Waiting for end of traverse movement

Waiting for reaching the spindle position

9

127

G codes

A-D821UK-1_200420

127


DMG MORI LifeCycle Services

DMGMORI.COM

DMG MORI Academy – Our locations for your training!

Chicago

Bielefeld

Seebach

Leonberg

Geretsried

Wernau

Pfronten

Winterthur Klaus

Moscow

Ulyanovsk

Iga

Shanghai

Singapore

Excellence

REALIZER

Center

Bielefeld

Wernau

Chicago

2400 Huntington

Gildemeisterstraße 60

Antoniusstraße 14

Blvd., IL- 60192

D - 33689 Bielefeld

D - 73249 Wernau

Hoffman Estates

Geretsried

Klaus

Moscow

Lausitzer Straße 7

Oberes Ried 11

ul. Novohohlovskaya 23 / 1

D - 82538 Geretsried

A - 6833 Klaus

RU - 109052 Moscow

Leonberg

Winterthur

Ulyanovsk

Riedwiesenstraße 19

Sulzer-Allee 70

DMG MORI Street 1

D - 71229 Leonberg

CH - 8404 Winterthur

RU - 433400 Ulyanovsk

Excellence

REALIZER

Shanghai

Center

Pfronten

Singapore

No. 331 Guangzhong

Tiroler Straße 85

3 Tuas Link 1

Road, Minhang District

D - 87459 Pfronten

SG - 638584

Shanghai 201108, China

Seebach

Iga

Neue Straße 61

201 Midai, Iga City

D - 99846 Seebach

Mie, 519-1414, Japan

DMG MORI Academy GmbH

Gildemeisterstraße 60, D - 33689 Bielefeld

fon: +49 (0) 52 05 / 74 25 01, fax: +49 (0) 52 05 / 74 25 02

training@dmgmori.com, www.dmgmori.com

Hooray! Your file is uploaded and ready to be published.

Saved successfully!

Ooh no, something went wrong!