354 268-21 - heidenhain

content.heidenhain.de

354 268-21 - heidenhain

Pilot

MANUALplus

4110

NC-Software

345 809-xx

English (en)

4/2003


Keyboard Symbol

Menu

Call the “Main menu“ (Machine mode of operation)

Switching key

Switches the help graphics for internal/

external machining

Process

Select a mode of operation

Numbers (0 to 9)

For entering values and selecting soft keys ...

Minus

For entering the algebraic sign

Decimal point

Enter

Confirm the entered value

Store

Conclude data input and transfer values

Keyboard Symbol

Backspace

Delete the character to the left of the cursor

Clear

Delete error messages

Cursor keys

Move the cursor in the indicated

direction by one position (character,

field, line, etc.)

Page up, page down (PgUp/PgDn)

Show the information on the previous/

next screen page; toggle between

two input windows

Info

Activate the error display or the

PLC status display


The Pilot

... is your concise programming guide for the HEIDENHAIN

MANUALplus 4110 control. For more comprehensive information

on operating the MANUALplus, refer to the User's

Manual.

Certain symbols are used in the Pilot to denote specific

types of information:

Important note!

Warning: danger to the user or the machine!

Chapter in the User's Manual where you will find

more detailed information on the current topic.

The information in this Pilot applies to the MANUALplus with

the software number 345 809-xx (Release 6.4).

Contents

Operation of the MANUALplus .......................................... 4

Setup ................................................................................. 5

Tool Measurement ............................................................ 7

Manual Operation .............................................................. 8

Teach-In ............................................................................. 9

Program Sequence ............................................................ 9

Graphic Simulation ............................................................. 10

Cycles ............................................................................... 11

Workpiece blank ................................................................ 12

Single Cuts ........................................................................ 13

Area Clearance .................................................................. 16

Recess Cycles .................................................................. 20

Thread Cycles.................................................................... 26

Undercut Cycles ................................................................ 29

Drilling and Boring Cycles .................................................. 30

Milling Cycles .................................................................... 34

Drilling and Milling Patterns ............................................... 39

DIN Cycle .......................................................................... 43

ICP Programming .............................................................. 44

DIN Programming .............................................................. 48

Tool Management.............................................................. 109

Create a Workpiece using Cycles...................................... 116

Contents

3


Control operation

4

Operation of the MANUALplus

Operating modes

The MANUALplus has three operating modes:

Machine

Tool Management

Organization

You can switch between the different operating modes using the

Process key (sequence: Process key – select the required mode using

the cursor keys – Process key).

The Process key can only be used when the main menu of the

current operating mode is active.

Menu selection

In the Machine and Tool Management modes of operation, the

available menus are arranged in a 9-field window. To select a menu

item, press the corresponding number key.

Data input

You can move the cursor to the desired input field with the “vertical“

arrow keys. Use the right and left arrow keys to position the cursor

within the input field to delete existing or add new characters.

Entered or changed data will not be transferred to the control until

you press “Input finished“ or “Save“. If you leave the input

window with “Back“, all entries or changes you made will be

lost.

Error display

Errors/message are signaled by the error symbol

(on the left-hand side of the title bar). With the “Info“

key you can open the error window and read the

messages that have been recorded by the control.

Clearing an error message

You can clear one error message using “Backspace“.

All error messages are canceled with

“Clear“.


Setup

Entering machine data (“Set S, F, T“)

With “Set S, F, T“ you enter the machine data required for manual

operation, as well as the maximum speed and tool angle.

Note with driven tools:

MANUALplus recognizes from the tool description whether a driven

tool is used.

If the active tool is a driven tool, the displayed spindle and machine

tool data refer to the driven tool.

Milling cutters always qualify as “driven tools“.

After system start, MANUALplus assumes that the tool

that was last used is still inserted in the tool holder. If this

is not the case, you must inform the control of the tool

change.

At a “constant cutting speed“, MANUALplus calculates the

spindle speed depending on the tool tip position. The smaller

the diameter of the tip, the higher the spindle speed. The

“maximum spindle speed D“, however, is never exceeded.

Display fields for machine data

Position display

Display of the current distance between tool tip

and workpiece datum in X and Z, or the current

position of the C axis.

Distance-to-go

MANUALplus calculates the distance remaining

from the current position to the target position of

the active traversing command.

Spindle utilization

Utilization of the spindle motor

T display

T number of the inserted tool

Tool compensation values

F display

Symbol for cycle status

Upper field: programmed value

Lower field: setting of override control and actual

feed rate

S display

Symbol for spindle status

Upper field: programmed value

Lower field: setting of override control and actual

spindle speed

With position control (M19): spindle position

Gear range (small number next to “S“)

“S“ highlighted: S display is valid for the driven tool

Setup

5


6

Setup

Setting the axis values (defining workpiece datum)

The workpiece datum can be defined in two different ways:

“Touch“ the end face of the workpiece and use “Z=0” to define this

position as the “workpiece zero point Z“.

Enter the position of the tool (distance between tool and workpiece

zero points) and confirm with “Save”.

The graphic support window shows the distance between machine

datum and workpiece datum (aka “displacement“).

See “3.4 Machine Setup“.

Setting the protection zone

The protection zone can be defined in two different ways:

Move the tool until it reaches the “protection zone“ and confirm with

“Take over position”.

Enter the coordinates at the position of the “protection zone“ (distance:

workpiece datum to protection zone); confirm with “Save”.

The graphic support window shows the distance

between machine datum and protection zone.

“–99999.000“ means: Protection zone monitoring is

not active


Tool Measurement

You can compare the dimensions of non-measured tools by comparing

them with a measured tool.

Sequence (example):

1 Insert the reference tool and enter the T number in “Set S, F, T“.

2 Turn an end face and define this coordinate as the workpiece zero

point.

3 Return to “Set S, F, T“, insert the tool to be measured and enter the

associated T number.

4 Activate “Measure tool”.

5 Touch the end face with the tool, enter the value “0“ for the “measuring

point coordinate Z“ (workpiece datum) and confirm with “Take

over Z“. MANUALplus stores the tool dimension and deletes any

exisiting compensation values for the tool.

6 Touch the diameter with the tool. Enter this coordinate as the “measuring

point coordinate X” and confirm with “Take over X“. MANUALplus

stores the tool dimension and deletes any exisiting compensation

values for the tool.

7 If you are measuring a lathe or recessing tool, enter the cutting

radius and confirm with ”Save radius”.

You can only measure tools that have already been entered

in the tool table.

Tool Compensation

1 Select ”X offset f. tool”, ”Z offset f. tool” or ”Special

correction“ – the compensation value is

shown in the distance-to-go display.

2 Using the handwheel, move by the distance to be

compensated.

3 Press ”Save” to tranfer the compensation value.

Deleting tool compensation values

You can delete existing compensation values with

the function keys ”Erase X offset”, ”Erase Z offset”

and ”Delete special”.

Tool Measurement

7


Manual mode

8

Manual mode

With manual workpiece machining, you move the axes with the

handwheels or jog controls. You can also use cycles, for example, for

machining complex contours. The paths of traverse and the cycles,

however, are not stored.

After switch-on and traversing the reference marks, MANUALplus is

always in ”Manual“ mode. This mode remains active until you select

”Teach-in” or ”Program run”. You can return to Manual mode with the

”Menu“ key.

Before you start machining, you should set the workpiece datum

using ”Set axis values“ to ensure that the display shows the correct

position.

Tool change

You need to enter the T number and check the tool parameters.

Handwheel operation

The Handwheel resolution selector switch on the machine operating

panel enables you to set the traverse per handwheel increment.

Jog operation (joystick)

The feed rate is defined in ”Set S, F, T“ and the feed rate for rapid

traverse in the parameter ”Machine parameters – Feeds“.

Cycles

When using cycles, you need to:

Set the spindle speed

Set the feed rate

Insert tool, define T number and check tool data

Approach cycle start point

Select the cycle, define the parameters, and

grapchically simulate the cycle execution

Run the cycle


Teach-in (Cycle mode)

In Teach-in mode you machine a workpiece step by step with

cycles. MANUALplus ”memorizes“ how the workpiece was machined

and stores the working steps in a cycle program.

DIN macros are programmed in the DIN editor and then integrated in

the DIN cycle.

Program run

In the machining mode, you use already-programmed cycle programs

and DIN programs for parts production. You can check your programs

befor running them using the ”Graphic simulation” function.

Program execution

With the function keys, you can determine whether a program is to be

executed continuously, cycle by cycle, or block by block. Independent

of this setting, program run will be interrupted immediately if you

press ”Cycle stop”.

Compensation: You can enter tool compensation values and additive

corrections during program run (function key ”Tool/Add correct.”).

Base blocks: The program-block display is switched to base blocks.

The traversing and switching commands are now shown in ”DIN

format“.

MANUALplus starts program run from the

cycle (or DIN block) that is highlighted.

The starting position is not changed by a

previous graphic simulation.

DIN programs: When selecting the

startup block, ensure that the machine run

data (S, F, T) are set before the control

reaches the first traversing command.

Program

Danger of collision!

MANUALplus does not convert faulty cycles.

It is therefore very important that you

check whether a cycle program resulting in

an error message can be run. Teach-in,

9


Graphic simulation

10

Graphic simulation

The graphic simulation feature enables you to check the machining

sequence, the proportioning of cuts and the finished contour before

actual machining.

Graphical elements:

Coordinate system: The workpiece datum serves as the origin of

the coordinate system.

Contours: At the beginning of a cycle simulation, the programmed

contour is depicted in “cyan“.

The light dot (small white square) represents the theoretical tool tip.

Rapid traverse paths are shown as broken white lines.

Feed paths are shown as continous green lines. They represent the

path of the theoretical tool tip.

Tool-tip (cutting edge): MANUALplus shows the “cutting edge“ of

the tool as a continuous yellow line. This graphic display is based on

the tool data. If the control does not have enough data on the tool, it

can only represent the tool tip as a light dot.

The area that is covered by the tool is shaded.

Warnings

MANUALplus displays warnings in the leftmost field of the function-key

row.

Extra functions:

Track: Switch from “Wire frame“ to “Cutting

path“ graphic.

Slide: Switch from “Light dot“ to “Tool tip“ graphic.

Process times (machining time): Switch to “Time

calculation“.

Face view: Switch to Face view if you have

programmed drilling cycles or C-axis machining

for the end face.

Surface view: Switch to Surface view if you have

programmed drilling cycles or C-axis machining for

the lateral surface.

Time Calculation

During simulation, MANUALplus calculates the

machining and idle machine times.

If you are working with cycle programs, each cycle

is shown in a separate line. With DIN programs, a

separate line is inserted in the table for each new

tool (i.e. for each tool call with T).


Cycles

You must set the workpiece datum and check the tool data before you

use cycles.

Define the individual cycles as follows:

Position the tool tip with the handwheels or jog keys to the cycle

start point (only in Manual mode).

Select and program the cycle.

Run a graphic simulation of cycle execution.

Execute the cycle.

Save the cycle (only in Teach-in mode).

In Teach-in mode

the starting point X, Z and

the machine data S, F and T

need to be entered in the cycle description.

In Manual mode, you must program these machinen dat

before calling a cycle.

MANUALplus does not store any cycles in Manual mode.

Danger of collision!

MANUALplus approaches the starting point before cycle execution

diagonally in rapid traverse. If the tool cannot approach

the starting point without collision, you must define an

auxiliary position with the cycle “Rapid traverse positioning“.

Cycle keys

A programmed cycle will not be executed until you

press the Cycle START button. You can interrupt a

cycle at any time during execution with Cycle STOP.

During a cycle interruption you can:

Resume cycle execution with “Cycle START“. The

control will always resume execution of the cycle

at the point of interruption – even if you have

moved the axes during the interruption.

Move the axes with the jog keys or with the

handwheels.

Abort machining with the “Cancel“ function key.

Cycles

11


Workpiece blank

12

Blank Bar/Tube

The cycle describes the workpiece blank and the setup used. This

information is evaluated during the simulation.

Information on cycle parameters:

X: Outside diameter

Z: Length (including transverse allowance and clamping range)

I: Inside diameter for workpiece blank ”tube”

K: Right edge (transverse allowance)

B: Clamping range

J: Type of clamping

0: No clamping

1: Outside clamping

2: Inside clamping

Workpiece blank contour ICP

The cycle integrates the workpiece blank defined with ICP and describes

the setup used. This information is evaluated during the simulation.

Information on cycle parameters:

X: Clamping diameter

Z: Clamping position in Z

B: Clamping range

J: Type of clamping

0: No clamping

1: Outside clamping

2: Inside clamping

N: ICP contour number


Rapid traverse positioning

Approach tool change point

The tool approaches the “target point“ in rapid traverse.

If you press the “T-Change approach“ function key , the tool moves to

the tool change point in rapid traverse. MANUALplus then switches to

the tool entered in “T“.

The direction in which the tool approaches the target point –

transversely, longitudinally or diagonally, depends on whether

you enter the target coordinates in the X axis, in the Z axis, or

in both X and Z.

M functions

Enter machine commands (M functions) and confirm them with “Input

finished“. The function is executed after pressing “Cycle START“.

See your machine manual for the meaning of the M functions.

Longitudinal linear machining

The tool moves from the “start point X, Z“ to the

“target point Z2“ at the programmed feed rate.

When the cycle is completed, the tool remains at

the cycle end position.

Contour linear longitudinal (“with return“)

The tool approaches the workpiece, executes the

longitudinal cut and returns to the “start point“ at

the end of the cycle.

Transverse linear machining

The tool moves from the “start point X, Z“ to the

“target point X2“ at the programmed feed rate.

When the cycle is completed, the tool remains at

the cycle end position.

Contour linear traverse (“with return“)

The tool approaches the workpiece, executes the

transverse cut and returns to the “start point“ at the

end of the cycle.

Single cuts

13


Single cuts

14

Linear machining at angle

MANUALplus calculates the target position and moves the tool on a

straight line from the “start point X, Z“ to the “target position“. When

the cycle is completed, the tool remains at the cycle end position.

Contour linear angle (“with return“)

MANUALplus calculates the target position. The tool approaches the

workpiece, executes the linear cut and returns to the “start point“ at

the end of the cycle.

Cutting radius compensation is effective in the “with

return“ mode.

Parameter combinations for defining the target point:

see support graphics

Circular machining

(With the appropriate soft key, you can select whether

the circular arc is to be machined clockwise or

counterclockwise.)

The tool moves in a circular arc from the “start point X, Z“ to the “end

point contour X2, Z2“ at the programmed feed rate. When the cycle is

completed, the tool remains at the cycle end position.

Contour circular (“with return“)

The tool approaches the workpiece, executes the circular cut and

returns to the “start point“ at the end of the cycle.

Cutting radius compensation is effective in the “with return“

mode.


Chamfer

The cycle produces a chamfer that is dimensioned relative to the

corner of the workpiece contour. When the cycle is completed, the

tool remains at the cycle end position.

Contour chamfer (“with return“)

In this cycle, the tool approaches the workpiece, machines the

chamfer and returns to the “start point“ at the end of the cycle.

Cutting radius compensation is effective in the “with

return“ mode.

The direction of tool traverse depends on the algebraic sign

for the parameter “element position J“ (see Help graphic).

Parameter combinations for defining the chamfer: see

support graphics.

Rounding

The cycle produces a rounding arc that is dimensioned relative to the

corner of the workpiece contour. When the cycle is completed, the

tool remains at the cycle end position.

Contour rounding (“with return“)

In this cycle, the tool approaches the workpiece, machines the

rounding arc and returns to the “start point“ at the end of the cycle.

Cutting radius compensation is effective in the “with

return“ mode.

The direction of tool traverse depends on the algebraic sign

for the parameter “element position J“ (see support

graphics).

Single cuts

15


16

Clearance cycle group

Cut longitudinal

Cut transverse

Roughing (expanded): The cycle machines the defined area, taking

the optional contour elements into account.

Finishing (expanded): The cycle finishes the defined contour section,

taking the optional contour elements into account.

Information on cycle parameters:

B: Chamfer or rounding at end of contour

B>0: Rounding radius

B


Plunge longitudinal

Plunge transverse

Roughing (expanded): The cycle machines the defined area, taking

the optional contour elements into account.

Finishing (expanded): The cycle finishes the defined contour section,

taking the optional contour elements into account.

Information on cycle parameters:

R: Rounding (on both sides of the contour valley)

B1, B2: Chamfer or rounding (B1 contour start; B2 contour end)

B>0: Rounding radius

B


18

Clearance cycle group

ICP longitudinal contour-parallel

ICP transverse contour-parallel

With ICP cycles, you define the machining parameters within the

cycle description and specify the contour to be machined in an ICP

macro.

Roughing: The cycle machines the area defined by the “start point X,

Z” and the “ICP contour N“ parallel to the contour.

Finishing: The cycle finishes the contour area defined by “ICP contour N”.

Danger of collision!

If the setup and tip angles of the tool have not been defined,

the tool plunge-cuts into descending contours at the programmed

plunging angle.

If the setup and tip angles of the tool have been defined,

the tool plunge-cuts at the maximum possible angle. In this

case, the resulting contour will not be completely finished

and may need to be reworked.


ICP cutting longitudinal

ICP cutting transverse

With ICP cycles, you define the machining parameters within the cycle

description and specify the contour to be machined in an ICP macro.

Roughing: The cycle machines the area defined by the “start point X, Z”

and the “ICP contour N”.

Finishing: The cycle finishes the contour area defined by “ICP contour N”.

Finishing: The steeper the tool plunges into the material, the

greater the feed rate decrease (maximum: 50%).

Danger of collision!

If the setup and tip angles of the tool have not been defined,

the tool plunge-cuts into descending contours at the programmed

plunging angle.

If the setup and tip angles of the tool have been defined, the

tool plunge-cuts at the maximum possible angle. In this case,

the resulting contour will not be completely finished and may

need to be reworked.

Clearance cycle group

19


Recessing cycles

20

Recessing radial

Recessing axial

Recessing (expanded): The cycle machines the defined area, taking

the optional contour elements into account.

Finishing (expanded): The cycle finishes the defined contour section,

taking the optional contour elements into account.

Information on the cycle parameters:

R: Rounding (on both sides of contour valley)

B1, B2: Chamfer or rounding (B1 contour start; B2 contour end)

B>0: Rounding radius

B


ICP recessing radial

ICP recessing axial

With ICP cycles, you define the machining parameters within the

cycle description and specify the contour to be machined in an ICP

macro.

Recessing: The cycle machines the area defined by the “start point X,

Z” and the “ICP contour N”.

Finishing: The cycle finishes the contour area defined by “ICP contour N”.

Recessing:

“Cutting width P” is defined: infeeds † P.

“Cutting width P” is not defined:

Infeeds † 0.8*cutting width of tool.

Finishing: The tool returns to the ”start point X, Z” at the end

of the cycle.

Recessing cycles

21


Recessing cycles

22

Recess turning radial

Recess turning axial

Recess turning (expanded): The cycle machines the defined area

with alternating recessing and roughing motions, taking the optional

contour elements into account.

Recess turning – finishing (expanded): The cycle finishes the defined

contour section, taking the optional contour elements into account.

Information on the cycle parameters:

O: Recess feed rate

R: Rounding (on both sides of contour valley)

B1, B2: Chamfer or rounding (B1 contour start; B2 contour end)

B>0: Rounding radius

B


ICP recess turning radial

ICP recess turning axial

With ICP cycles, you define the machining parameters within the

cycle description and specify the contour to be machined in an ICP

macro.

Recess turning: The cycle machines the area defined by the “start point

X, Z” and the “ICP contour N” with alternating recessing and roughing

motions.

Recess turning – finishing: The cycle finishes the contour area defined by

“ICP contour N”. The cycle machines the material defined in “Oversizes I,

K“.

Recess turning: Which points need to be defined?

Falling contours: Only the “start point X, Z“ – not the “contour

beginning point X1, Z1“

Rising contours: The “start point X, Z“ and the “contour beginning

point X1, Z1“

Finishing:

The tool returns to the “start point X, Z” at the end of the

cycle.

In “Oversizes I, K“, define the material that is machined in the

finishing cycle.

Recessing cycles

23


Recessing cycles

24

Undercut H

This cycle machines a “Form H” undercut. The workpiece is approached

at a safety clearance. If you do not enter a value for W, it will

be calculated from K and R. The final point of the undercut is then

located at the “final point contour”.

Information on the cycle parameters:

R: Undercut radius – default: no circular element

W: Plunge angle – default: W is calculated

Undercut K

The resulting contour geometry depends on the tool that is used.

Cycle run

1 Pre-position at an angle of 45° to safety clearance above “corner point

contour X1, Z1” in rapid traverse.

2 Plunge-cut at an angle of 45° – the path of traverse is calculated from

the parameter “undercut depth I”.

3 Retract to “start point X, Z“ on same path.

This cycle does not take any cutting radius compensation

values into account.


Undercut U

This cycle machines a “Form U” undercut.

Information on the cycle parameters:

X2: End point of end face – default: the end face is not finished

I: Undercut diameter

K: Undercut breadth – If the cutting breadth of the tool is not

defined, the control assumes that the tool's cutting width

equals K.

B Chamfer or rounding

B>0: Rounding radius

B0: Rounding radius

B


Threadcut cycle group

26

Thread cycle (longitudinal) – Expanded

This cycle cuts a single- or multi-start thread. With the function key,

you can determine whether an external or internal thread is to be

machined. The thread starts at the “start point X“ and ends at the “end

point Z2“ (without a thread run-in or run-out).

Information on the cycle parameters:

F1: Thread pitch (is evaluated for the feed rate)

U: Thread depth – default:

external threads: U=0.6134*F1

internal threads: U=–0.5413*F1

I: 1st cutting depth – no input: I is calculated automatically

from U and F1

A: Feed angle – default: 30°; range: –60° < A < 60°

A0: infeed on right thread flank

J: Remaining cutting depth – default: 1/100 mm

D: Number of grooves – default: 1 (= single-start thread)

E: Incremental pitch (increases/reduces the pitch per revolution

by E) – default: 0

“Cycle STOP“ only becomes effective

at the end of a thread cut.

The feed rate and spindle speed overrides

are disabled during execution of

the cycle.

The function “Last cut” can be activated

at the end of the cycle. The last

thread cut is repeated, allowing

handwheel compensation.


Regroove (longitudinal) thread

With this cycle, you can repair a single-start thread. Since you have

already unclamped the workpiece, MANUALplus needs to know the

exact position of the thread.

Cycle run

1 Pre-position threading tool so that tip is at center of thread groove.

2 Transfer the tool position and the spindle angle with “Take over

position”.

3 Manually move the tool out of the thread groove.

4 Position tool to “start point X, Z”.

5 Start cycle with “Input finished”, then press the “Cycle START”

button.

Information on the cycle parameters:

C: Measured angle (spindle angle)

ZC: Measured position (tool position)

F1: Thread pitch (is evaluated for the feed rate)

U Thread depth – default:

external threads: U=0.6134*F1

internal threads: U=–0.5413*F1

I: 1st cutting depth

I


Threadcut cycle group

28

Tapered thread

API thread

This cycle cuts a single- or multi-start tapered/API thread. With the

function key, you can determine whether an external or internal

thread is to be machined. The thread starts at the “start point X“ and

ends at the “end point Z2“ (without an thread run-in or run-out). With

an API thread, the thread depth is decreased at the thread runout.

Information on the cycle parameters:

F1: Thread pitch (is evaluated for the feed rate)

U: Thread depth – no input:

external threads: U=0.6134*F1

internal threads: U=–0.5413*F1

I: 1st cutting depth – no input: I is calculated automatically from

U and F1

A: Feed angle – default: 30°; range: –60° < A < 60°

A0: infeed on right thread flank

J: Remaining cutting depth – no input: 1/100 mm

D: Number of grooves – default: 1 (= single-start thread)

E: Incremental pitch (increases/reduces the pitch per revolution

by E) – default: 0

”Cycle STOP” only becomes effective at the end of a thread cut.

The feed rate and spindle speed overrides are disabled

during execution of the cycle.

The function ”Last cut” can be activated at the end of the

cycle. This function repeats the last thread cut, allowing

handwheel compensation.

Tapered thread

API thread


Undercut cycles

28

Thread undercut DIN 76

Undercut DIN 509 E

Undercut DIN 509 F

These cycles execute an undercut, and can also machine a cylinder

start chamfer, the adjoining cyclinder and the adjoining end face.

Undercut parameters that are not defined are automatically calculated

from the standard table.

Thread undercut: If you enter an “undercut oversize P”, the undercut

cycle will be divided into pre-turning and finish-turning. “P“ is the

longitudinal oversize. The transverse oversize is preset to 0.1 mm.

Information on the cycle parameters:

FP: Thread pitch (with thread undercut) – default: FP is determined

from the diameter

E: Feed reduction (for plunge-cutting) – default: feed rate F

R: Undercut radius – default: value from standard table.

The undercut radius is executed on both sides of the undercut.

B: Cylinder 1st cut length– default: no chamfer machined at start

of cylinder

WB: 1st cut angle – default: 45 °

RB: 1st cut radius– default: no chamfer radius is machined

All parameters that you enter will be accounted for – even if the

standard table prescribes other values.

Example: Thread undercut DIN 76


30

Drilling and boring cycles

Drilling axial

Drilling radial

This cycle drills a hole on the end face/lateral surface of the workpiece.

Information on the cycle parameters:

C: Spindle angle (C-axis position) – default: current spindle position

Z1/X1: Start point drill – no input: drilling will start from position Z/X

E Dwell time (for chip breaking at end of hole) –

default: 0

AB Drilling lengths – default: 0

V: Drilling variants – default: 0

0: Without feed reduction

1: Reduction for drilling through

2: Reduction for spot drilling

3: Reduction for spot drilling and drilling through

If you program both “AB” and “V”, the feed rate is reduced

for spot and through drilling (reduction factor: 50%).

MANUALplus uses the tool parameter “driven tool” to determine

whether the programmed spindle speed and feed rate

apply to the spindle or the driven tool.

Drilling axial

Drilling radial


Deep-drilling (pecking) axial

Deep-drilling (pecking) radial

The bore hole on the end face/cylindrical surface is drilled in several

passes. After each pass, the drill retracts and, after a dwell time,

advances again to the first pecking depth, minus the safety distance.

Information on the cycle parameters:

C: Spindle angle (C-axis position) – default: current spindle position

Z1/X1: Start point drill – no input: drilling will start from position Z/X

P: 1st hole depth – no input:

hole will be drilled in one pass

IB: Hole depth reduction value – default: 0

JB: Minimum hole depth – default: 1/10 of P

B: Return length – default: retract to “start point”

E Dwell time – default: 0

AB Drilling lengths – default: 0

V: Drilling variants – default: 0

0: Without feed reduction

1: Reduction for drilling through

2: Reduction for spot drilling

3: Reduction for spot drilling and drilling through

If you program both “AB” and “V”, the feed rate is reduced

for spot and through drilling (reduction factor: 50%).

MANUALplus uses the tool parameter “driven tool” to determine

whether the programmed spindle speed and feed

rate apply to the spindle or the driven tool.

Deep-drilling axial

Deep-drilling radial

Drilling and boring cycles

31


32

Drilling and boring cycles

Tapping axial

Tapping radial

With this cycle, you can tap a thread into a bore hole on the end face/

lateral surface of a workpiece. The tapping tool requires a certain

overrun at the start of thread which is defined in the parameter “slop.

length B“ to reach the programmed spindle speed and feed rate.

Information on the cycle parameters:

C: Spindle angle (C-axis position) – default: current spindle position

F1: Thread pitch (is evaluated for the feed rate) – default: thread pitch of

the tool

B: Run-in length

Default: 2 * thread pitch F1

SR: Return speed – Default: same spindle speed as for tapping

MANUALplus uses the tool parameter “driven tool” to determine

whether the programmed spindle speed and feed rate

apply to the spindle or the driven tool.

Tapping axial

Tapping radial


Thread milling axial

This cycle mills a thread into an exisiting bore hole.

The tool is positioned to the “thread end point“ within the bore hole.

The tool then approaches with the “approach radius R,“ mills the

thread in a 360° revolution, advancing by the “thread pitch F“. The

cycle then retracts the tool and returns it to the start point.

Information on the cycle parameters:

C: Spindle angle (C-axis position)

Z1: Start point thread– default: Start point Z

Z2: End point thread

I: Internal thread diameter

R: Approach radius – default: (I – cutter diameter)/2

F1: Thread pitch

J: Thread direction – default: 0

J=0: Right

J=1: Left

H: Cutting direction – default: 0

H=0: Up-cut milling

H=1: Down-cut milling

Drilling and boring cycles

33


Rapid traverse positioning

This cycle switches on the C axis, and positions the spindle (C axis) and

the tool.

Information on the cycle parameters:

X2, Z2: End point

C2: Final angle

A subsequent manual milling cycle switches off the C axis.

“Rapid traverse positioning“ is is only required in the Manual

mode.

Groove axial

Groove radial

This cycle creates a groove on the end face/lateral surface of a

workpiece. The groove width equals the cutter diameter.

Information on the cycle parameters:

C: Spindle angle (C-axis position) – default: current spindle angle

Z1/X1: Upper edge of milling – default: Start point Z/X

Z2/X2: Lower edge of milling

P: Plunging depth – default: total depth in one infeed

FZ: Infeed – default: active feed rate Groove axial

Milling cycles

33


Milling cycles

34

Figure axial

Figure radial

Depending on the parameters, the cycle either mills a contour or roughs/

finishes a pocket on the end face/lateral surface.

You can define the following contours:

Rectangle (Q=4, LB)

Square (Q=4, L=B)

Circle (Q=0, RE>0, L and B: no entry)

Triangle or polygon (Q=3 or Q>4, L>0)

Information on the cycle parameters:

U: Overlap factor

No entry: Contour milling

U>0: Pocket milling – (minimum) overlap of the milling paths

= U*cutter diameter

H: Cutting direction – default: 0

H=0: Up-cut milling

H=1: Down-cut milling

J: Contour milling:

J=0: On the contour

J=1: Inside

J=2: Outside

Pocket milling:

J=0: From the inside out

J=1: From the outside in

O: Milling procedure (only for pocket milling) – default: 0

O=0: Roughing

O=1: Finishing

Figure axial

Figure radial


ICP figure axial

ICP figure radial

Depending on the parameters, the cycle either mills a contour or roughs/

finishes a pocket on the end face/lateral surface.

Information on the cycle parameters:

U: Overlap factor

No entry: Contour milling

U>0: Pocket milling – (minimum) overlap of the milling

paths = U*cutter diameter

H: Cutting direction – default: 0

H=0: Up-cut milling

H=1: Down-cut milling

J: Contour milling:

J=0: On the contour

J=1: Inside

J=2: Outside

Pocket milling:

J=0: From the inside out

J=1: From the outside in

O: Milling procedure (only for pocket milling) – default: 0

O=0: Roughing

O=1: Finishing

ICP figure axial

ICP figure radial

Milling cycles

35


Milling cycles

36

Face milling

Depending on the parameters, the cycle mills on the end face:

One or two surfaces (Q=1 or Q=2, B>0)

One rectangle (Q=4, LB)

One square (Q=4, L=B)

One triangle or polygon (Q=3 or Q>4, L>0)

One circle (Q=0, RE>0, L and B: no entry)

For one or two surfaces, “B“ defines the remaining thickness (the

material which remains). For an even number of surfaces you can

program “B“ instead of “V“.

Information on the cycle parameters:

B: Width across flats

When Q=1, Q=2: B is the remaining thickness

Rectangle: Rectangle width

Square, polygon (Q‡4): B is the width across flats

Circle: no entry

A: Angle to the X axis – default: 0

Polygon (Q>2): Position of the figure

Circle: no entry

H: Cutting direction – default: 0

H=0: Up-cut milling

H=1: Down-cut milling

J: Uni-/bidirectional

J=0: Unidirectional

J=1: Bidirectional

O: Roughing/finishing – default: 0

O=0: Roughing

O=1: Finishing


Helical groove milling

The cycle mills a helical groove from “Z1“ to “Z2“. “C1“ defines the

position of the groove beginning. Use “P“ and “K“ to define a ramp at

the beginning and end of the groove. The groove width equals the

cutter diameter.

The first downfeed is carried out with “I“ – MANUALplus calculates the

subsequent downfeedings as follows:

Current downfeed = I * (1 – (n–1) * E)

n: nth downfeeding

The downfeed is reduced step-by-step to >= 0.5 mm. After that each

downfeed is 0.5 mm.

Information on the cycle parameters:

C1: Start angle

X1: Diameter

Z1, Z2: Start point/end point groove

F1: Pitch

P, K: Approach length, run-out length

U: Groove depth

I: Maximum downfeed

E: Cutting depth reduction

Milling cycles

37


Pattern linear axial

The function “Pattern linear axial“ can be activated in drilling cycles

(drilling, pecking, tapping) and milling cycles (groove, ICP contour) to

machine a hole or milling pattern arranged at regular spacing in a

straight line on the end face.

You describe the “Pattern start point/end point“ and the individual

pattern positions with the following parameter combinations:

Pattern start point:

X1, C1 or

XK, YK

Pattern positions:

Ii, Ji and Q

I, J and Q

Hole pattern: MANUALplus generates the commands M12

and M13 (tighten/release shoe brake) under the following

conditions: the drilling/pecking tool must be “driven“ (Parameter

“Tool driven H“) and the “Turning direction MD“ must

be defined.

ICP milling contours: When the contour start point is not the

coordinate system origin, the distance “contour start point –

coordinate system origin“ is added to the pattern position.

Drilling and milling patterns

39


40

Drilling and milling patterns

Pattern circular axial

The function “Pattern circular axial“ can be activated in drilling cycles

(drilling, pecking, tapping) and milling cycles (groove, ICP contour) to

machine a hole or milling pattern arranged at regular spacing on a

circle or circular arc on the end face.

You describe the center point of the circular arc and the individual pattern

positions with the following parameter combinations:

XM, CM

XK, YK

Hole pattern: MANUALplus generates the commands M12

and M13 (tighten/release shoe brake) under the following

conditions: the drilling/pecking tool must be “driven“ (Parameter

“Tool driven H“) and the “Turning direction MD“ must be

defined.

ICP milling contours: When the contour start point is not the

coordinate system origin, the distance “contour start point –

coordinate system origin“ is added to the pattern position.


Pattern linear radial

The function “Pattern linear radial“ can be activated in drilling cycles

(drilling, pecking, tapping) and milling cycles (groove, ICP contour) to

machine a hole or milling pattern arranged at regular spacing in a straight

line on the cyclindrical surface.

Information on the cycle parameters:

C: Spindle angle – default: current spindle position

Z1, C1: Start point pattern – default: “start point Z“ is used as the

starting point for the pattern

ZE: End point pattern – default: Z1 is used as the end point

Wi: Angle increment (pattern distance) – default: The holes/millings

are arranged on the cylindrical surface at regular spacing

ICP milling contours: When the contour start point is not the

coordinate system origin, the distance “contour start point –

coordinate system origin“ is added to the pattern position.

Drilling and milling patterns

41


42

Drilling and milling patterns

Pattern circular radial

The function “Pattern circular radial“ can be activated in drilling cycles

(drilling, pecking, tapping) and milling cycles (groove, ICP contour) to

machine a hole or milling pattern arranged at regular spacing on a circle

or circular arc on the cylindrical surface.

Information on the cycle parameters:

C: Spindle angle (C-axis position) – default: current spindle position

ZM,CM: Center of pattern

A: Angle of 1st hole (spindle angle) – default: 0°

Wi: Angle increment (pattern distance) – default: The holes/millings

are arranged on the cylindircal surface at regular spacing

ICP milling contours: When the contour start point is not the

coordinate system origin, the distance “contour start point –

coordinate system origin“ is added to the pattern position.


DIN Cycle

You only need to define the number of the DIN macro in the input

window.

The machine data that are programmed in the cycle (in Manual mode:

the currently active machine data) become effective as soon as you

start cycle execution. You can change the machine data (S, F, T) at any

time by editing the DIN macro.

In this cycle, no start point is defined. Please keep in mind that

the tool moves on a diagonal path from the current position to

the first position that is programmed in the DIN macro.

DIN-Zyklus

43


ICP Programming

44

ICP Programming

After calling an IPC cycle, you can activate the ICP editor with the

function key “Edit ICP“.

Programming and adding to ICP contours

You program an ICP contour by entering the contour elements one

after the other in the correct sequence. Form elements (chamfers,

roundings, undercuts) can be entered as part of the contour or can be

“superimposed“ when the basic contour is finished. The transition to

the next contour element is determined with the “Tangential transition“

function key.

If you extend an ICP contour, the new element is “joined onto“ the

last contour element. A small box indicates the last contour element

when the ICP contour is displayed but is not being edited.

Each unsolved contour element is identified by a small symbol below

the graphics window.

Contour direction: ICP cycles rough and finish in the contour direction.

You change the contour direction with “Turn contour“.

Changing a contour element

Select the element you wish to change and press “Change element“. The

data is then prepared for editing.

If a contour contains “unsolved“ contour elements, you cannot change

the “solved“ elements. You can, however, set or delete the “tangential

transition“ for the element located directly before the unsolved contour

area.

If the element to be changed is an unsolved element, the

associated symbol is marked “selected“.

The element type and the direction of rotation of a circular

arc cannot be changed.

Soft keys Symbol

Select “Superpositioning“

Tangential transition

from linear to circular element

Tangential transition

from circular to circular element or

linear element (rotation direction

see symbol)

Colors in the contour graphics

Yellow: For solved elements

Gray: For unsolved, depictable elements

Red: Selected solution, selected

element, selected corner

Blue: Remaining contour


ICP Contour Elements

Line entry: First select the direction with the corresponding menu

symbol and then enter the contour element dimensions. For a line in

an angle, refer to the help graphics for the direction of the angle.

Circular element entry: Select the direction of rotation and the type of

dimensioning with the corresponding menu symbols. MANUALplus

also requires an indication for the end point, either by entering:

the midpoint,

the radius, or

the midpoint and the radius

End face and lateral surface contours: Dimensioning is either

Cartesian or polar. The setting of the “Polar“ function key is the

determining factor. You can enter Cartesian coordinates as absolute or

incremental values.

The start point of the contour is defined when you

describe the first contour element.

The end point of the contour is determined by the target

point of the last contour element.

The contour element is finished at a special feed rate.

MANUALplus automatically calculates all missing

coordinates, points of intersection, center points, etc., that

can be derived mathematically.

You can enter contour coordinates as absolute or incremental

values.

If you call the “Selection of ICP contours“, MANUALplus

displays – depending on the cycle – only ICP contours for

the turning contour, end face or lateral surface.

Call lines menu

Call arcs menu

ICP Programming

45


ICP Programming

46

Chamfer

Rounding

The corner point is defined by “XS, ZS”. You need only enter the “chamfer

width B”/”rounding radius B”.

Turning contours: If the first element of the ICP contour is a chamfer/

rounding, it is necessary to specify the position of the chamfer/

rounding with “J”.

Parameters

XS, ZS: Contour corner point

B: Chamfer width / rounding radius

J: Element position

J = 1: Transverse element in +X direction

J=–1: Transverse element in –X direction

J = 2: Longitudinal element in +Z direction

J=–2: Longitudinal element in –Z direction

F: Special feed

Chamfer/rounding for turning contours

Chamfer/rounding for end face and lateral surface

contours


Thread undercut DIN 76

Undercut DIN 509 E

Undercut DIN 509 F

An “undercut” consists of a longitudinal element, an undercut and a

transverse element. You can start the undercut definition with either the

longitudinal or the transverse element.

Thread undercut: the diameter of the longitudinal element represents the

thread diameter (or, with internal threads, the core diameter).

Parameters that are not defined are automatically calculated from the

standard table. Also for a thread undercut:

“FP“ is calculated from “XS“

“I, K, W, and R“ are calculated from “FP“

Parameters (depending on the type of the undercut)

XS, ZS: Start point of the undercut

X, Z: End point of the undercut

FP: Thread pitch

I: Undercut diameter – default: value from the standard table

K: Undercut length – default: value from the standard table

W: Undercut angle – default: value from the standard table

R: Undercut radius – default: value from the standard table

P: Transverse depth– default: value from the standard table

A: Transverse angle– default: value from the standard table

U: Finishing oversize– default: no finishing oversize

J: Element position– default: 1

J=1: Undercut begins with longitudinal

element

J=–1: Undercut begins with transverse

element

F: Special feed

The “element position J” cannot be entered

when superimposing the undercut

and cannot be changed when programming

changes to ICP contours.

If you are programming an internal thread,

it is advisable to preset the “FP” since the

diameter of the longitudinal element is not

the thread diameter. If you have

MANUALplus calculate the thread pitch automatically,

slight deviations may occur.

ICP Programming

47


Overview of G Commands

48

DIN Programming

Rohteilbeschreibung Seite

G20 Futterteil Zylinder/Rohr 51

G21 Rohteilkontur 51

Tool positioning without machining Page

G0 Rapid traverse positioning 52

G14 Approach tool change point 52

Simple linear and circular paths Page

G1 Linear path 53

G2 Circular path – increm. center point coordinates 54

G3 Circular path – increm. center point coordinates 54

G12 Circular path – absolute center coordinates 54

G13 Circular path – absolute center coordinates 54

Feed rate, spindle speed Page

G26 Speed limitation for spindle 55

G126 Speed limitation for driven tool 55

G64 Interrupted (intermittent) feed 55

G94 Constant feed 55

G95 Feed per revolution 55

G195 Feed per revolution of driven tool 55

G96 Constant cutting speed 55

Feed rate, spindle speed Page

G196 Constant cutting speed for driven tool 55

G97 Spindle speed (in rev/min) 55

G197 Spindle speed (in rev/min) for driven tool 55

Tool-tip /milling cutter radius compensation (TRC/MCRC) Page

G40 Switch off TRC/CRC 56

G41 Switch on TRC/CRC 56

G42 Switch on TRC/CRC 56

Tool compensation Page

G148 Change cutter compensation 56

G149 Additive correction 57

G150 Compensate right tool tip 57

G151 Compensate left tool tip 57

Zero point displacement Page

G51 Zero point displacement 58

G56 Additive zero point displacement 58

G59 Absolute zero point displacement 59

Oversizes Page

G57 Paraxial oversize 60

G58 Contour-parallel oversize 60

Clearance cycle group Page

G80 End of cycle 61

G81 Longitudinal roughing 61

G82 Transverse roughing 61

G817 Longitudinal contour roughing 62


Clearance cycle group Page

G818 Longitudinal contour roughing 62

G819 Longitudinal contour roughing with recessing 63

G827 Transverse contour roughing 62

G828 Transverse contour roughing 62

G829 Transverse contour roughing with recessing 63

G83 Simple contour repeat cycle 64

G836 Contour-parallel roughing 65

G87 Line with radius 66

G88 Line with chamfer 66

G89 Contour finishing cycle 67

Grooving cycles Page

G86 Simple recessing cycle 68

G861 Axial contour cutting 69

G862 Radial contour cutting 69

G863 Axial contour finishing cut 71

G864 Radial contour finishing cut 71

G865 Simple axial cutting cycle 70

G866 Simple radial cutting cycle 70

G867 Axial finishing cut 71

G868 Radial finishing cut 71

Recess-turning cycle group Page

G811 Simple axial recess-turning cycle 72

G815 Axial recess-turning cycle 73

G821 Simple radial recess-turning cycle 72

G825 Radial recess-turning cycle 73

Threadcut cycle group Page

G31 Universal thread cycle 74

G32 Simple thread cycle 75

G33 Individual thread cut 76

G35 Metric ISO thread 77

G350 Simple longitudinal single-start thread 78

G351 Extended longitudinal multi-start thread 78

G352 Tapered API thread 79

G353 Tapered thread 80

G799 Axial thread milling 90

Undercut cycles, cut-off cycle Page

G25 Undercut contour (DIN509 E, DIN509 F, DIN76) 81

G85 Undercut cycle (DIN509 E, DIN509 F, DIN76) 82

G851 Undercut with cylinder machining DIN 509 E 83

G852 Undercut with cylinder machining DIN 509 F 83

G853 Undercut with cylinder machining DIN 76 83

G856 Undercut form U 84

G857 Undercut form H 85

G858 Undercut form K 85

G859 Cut-off cycle 86

Drilling cycles Page

G36 Tapping cycle 89

G71 Drilling cycle 87

G74 Pecking cycle 88

G799 Axial thread milling 90

Overview of G Commands

49


50

Overview of G Commands

End-face machining Page

G100 End-face rapid traverse 91

G101 End-face linear path 92

G102 End-face circular arc 93

G103 End-face circular arc 93

G304 Figure definition end-face complete circle 97

G305 Figure definition end-face rectangle 97

G307 Figure definition end-face polygon 98

G791 End-face linear groove 94

G793 End-face contour milling cycle 95

G797 End-face surface milling 96

G799 Axial thread milling 90

Lateral-surface machining Page

G120 Lateral-surface reference diameter 99

G110 Lateral-surface rapid traverse 99

G111 Lateral-surface linear path 100

G112 Lateral-surface circular arc 101

G113 Lateral-surface circular arc 101

G314 Figure definition lateral-surface complete circle 104

G315 Figure definition lateral-surface rectangle 105

G317 Figure definition lateral-surface polygon 105

G792 Lateral-surface linear groove 102

G794 Lateral-surface contour milling cycle 103

G798 Helical groove milling 104

Drilling and milling patterns Page

G743 Linear pattern on end face 106

G744 Linear pattern on lateral surface 106

G745 Circular pattern on end face 107

G746 Circular pattern on lateral surface 108

Other G Functions Page

G4 Dwell time 57

G60 Deactivate protection zone 57

See the User's Manual

G9 Block precision stop

G152 Datum shift (C axis)

G153 Standardizing the C axis

G193 Feed rate per tooth

G204 Wait for moment


Chuck part, cylinder/tube G20

G20 describes the workpiece blank and the setup used. This

information is evaluated during the simulation.

Parameters

X: Diameter

Z: Length (including transverse allowance and clamping range)

K: Right edge (transverse allowance)

I: nside diameter for workpiece blank ”cylinder.”

B: Clamping range

J: Type of clamping

0: No clamping

1: Outside clamping

2: Inside clamping

Workpiece blank contour G21

G21 describes the setup used. The workpiece blank is described with

G1, G2/3 and G12/13 commands that follow immediately after G21. G80

concludes the contour description.

This information is evaluated during the simulation.

Parameters

X: Clamping diameter

Z: Clamping position in Z

B: Clamping range

J: Type of clamping

0: No clamping

1: Outside clamping

2: Inside clamping

Definition of Workpiece Blank

51


Tool positioning

without machining

52

Rapid traverse G0

The tool moves at rapid traverse along the shortest path to the target

point.

Parameters

X, Z: Target point (X diameter)

G0 is also used in contour descriptions for defining the start point.

Tool change point G14

The slide moves in rapid traverse to the tool change point. In setup

mode, define permanent coordinates for the tool change.

Parameters

Q: Sequence – default: 0

0: Diagonal path of traverse

1: First in X axis, then in Z

2: First in Z axis, then in X

3: X axis only

4: Z axis only


Linear path G1

The tool moves linearly at the feed rate to the “end point“.

Parameters

X, Z: End point (X diameter)

A: Angle (angular direction): see graphic support window

B: Chamfer/rounding

B left undefined: angential transition

B=0: Nontangential transition

B>0: Rounding radius

B


Simple Linear and

Circular Paths

54

Circular path

G2, G3 – incremental midpoint dimensions

G12, G13 – absolute midpoint dimensions

The tool moves in a circular arc at the feed rate to the “end point“.

Parameters

X, Z: End point (X diameter)

R: Radius

Q: Point of intersection – default: Q=0

B: Chamfer/rounding

B left undefined: Tangential transition

B=0: Nontangential transition

B>0: Rounding radius

B


Speed limitation for spindle G26/

driven tool G126

G26/G126 limits the speed. A speed limitation remains in effect until a

new value is programmed for G26/G126.

Parameters

S: (Maximum) speed

The speed limitation remains in effect even after concluding

the DIN program and exiting “program run“.

If the speed programmed is greater than the speed set in

the machine parameter “General parameters for spindle – absolute

maximum speed“, then the speed limit of this parameter

takes effect.

Interrupted (intermittent) feed G64

G64 interrupts the programmed feed for a short period of time. The

function remains in effect until you program G64 without parameter

definitions.

Parameters

E: Pause duration – range: 0.01 s < E < 999 s

F: Feed duration – range: 0.01 s < E < 999 s

Feed rate constant G94 (minute feed)

G94 defines the feed rate independent of drive.

Parameters

F: Feed rate in mm/min or inch/min

Feed per revolution G95/G195

G95/G195 defines the feed rate as a function of drive.

G95: Referred to main spindle

G195: Referred to spindle 1 (driven tool)

Parameters

F: Feed rate in mm/revolution or inch/revolution

Constant cutting speed G96/G196

G96/G196 defines a constant cutting speed.

G96: The speed of the main spindle is dependent on

the X position of the tool tip.

G196: The speed of spindle 1 (driven tool) is dependent

on the diameter of the tool.

Parameters

S: Cutting speed in m/min or ft/min

Spindle speed G97 / G197

G97: Constant speed for the main spindle

G197: Constant speed for spindle 1 (driven tool)

Parameters

S: Speed in revolutions per minute

Feed rate, spindle speed

55


Tool-tip and milling cutter

radius compensation

56

Tool-tip and milling cutter radius compensation (TRC,

MCRC) G40, G41, G42

G40: Switch off TRC/MCRC

TRC/MCRC remains in effect until a block with G40 is reached.

The block containing G40, or the block after G40 muct contain a linear

path of traverse (G14 is not permissible).

G41/G42: Switch on TRC/MCRC

A linear path of traverse (G0/G1) must be programmed in or after the

block containing G41/G42.

TRC/MCRC is taken into account from the next path of traverse.

G41: TRC/MCRC with direction of traverse to the left of the contour –

inside machining (with direction of traverse in –Z)

G42: TRC/MCRC with direction of traverse to the right of the contour –

outside machining (with direction of traverse in –Z)

(Changing the) cutter compensation G148

With “O“ you can define which wear compensation values are to be

taken into account.

DX and DZ become effective after program start and after a T command.

Parameters

O: Selection – default: 0

O=0: DX, DZ active

O=1: DS, DZ active

O=2: DX, DS active

Some recessing and roughing cycles as well

as the milling cycles already include the

TRC/MCRC calls. You must therefore ensure

that TRC/MCRC is disabled before you call

these cycles. The commands G40, G41, G42

must not be used within the cycles.

The recessing cycles G861 to G868 and recess-turning

cycles G81x and G82x automatically

take the “correct“ wear compensation

into account.


Additive correction G149

To activate the additive correction function, program G149 followed by a

“D number“ (for example: G149 D901). “G149 D900“ resets the additive

correction function.

Additive corrections are effective from the block in which G149 is

programmed and remain effective until

the next “G149 D900“

the next tool change

the end of program.

Parameters

D: Additive correction – default: D900 – Range: 900 to 916

Compensate right tool tip G150

Compensate left tool tip G151

With recessing tools, the “tool orientation“ function defines whether the

tool reference point is set at the left or the right side of the tool tip.

G150: Reference point at right of tool tip

G151: Reference point at left of tool tip

G150/G151 is effective from the block in which it is programmed and

remains effective until

the next tool change

the end of program.

Dwell time G4

MANUALplus interrupts the program run for the

programmed length of time before executing the next

program block. If G4 is programmed together with a

path of traverse in the same block, the dwell time

only becomes effective after the path of traverse has

been executed.

Parameters

F: Dwell time – Range: 0 s < F < 999 s

Deactivate protection zone G60

The function G60 cancels a programmed monitoring

of the protection zone. G60 is only effective in the

block in which it is programmed.

Corrections,

other G Functions

57


Zero point displacement

58

Zero point displacement G51

G51 displaces the workpiece datum by “Z“ (or “X“). The displacement is

referenced to the workpiece datum (setup operation: “Setting axis

values“).

Even if you shift the datum several times with G51, the displacement is

always referenced to the workpiece datum from the setup mode.

A workpiece datum defined with G51 remains in effect up to the end of

program or until it is canceled by another zero point displacement.

Parameters

X, Z: Displacement (X as diameter)

Additive zero point displacement G56

G56 displaces the workpiece datum by “Z“ (or “X“). The displacement is

referenced to the currently active workpiece datum.

If you shift the workpiece datum several times with G56, the displacement

is added to the currently active datum.

Parameters

X, Z: Displacement (X as diameter)

G51 and G59 each cancel additive zero point displacements.


Absolute zero point displacement G59

G59 sets the workpiece datum to “X, Z“. The new datum is valid to the

end of program.

Parameters

X, Z: Displacement (X as diameter)

G59 cancels all previous zero point displacements (with G51,

G56 or G59).

Zero point displacement

59


Oversizes

60

Axis-parallel (paraxial) oversize G57

G57 defines different oversizes for X and Z. G57 must be programmed

before the cycle in which the oversize is to be taken into consideration.

The following cycles take the oversizes into consideration:

Roughing cycles: G81, G817, G818, G819, G82, G827, G828, G829, G83

Recess and recess-turning cycles: G81x, G82x, G86x

Cycles G81, G82 and G83 do not delete the oversizes after cycle

completion. For the other cycles, the oversizes are not valid after cycle

completion.

Parameters

X / Z: Oversize in X / Z (X as diameter)

Contour-parallel oversize (equidistant) G58

G58 defines a contour-parallel oversize. G58 must be programmed

before the cycle in which the oversize is to be taken into consideration.

A negative oversize is permitted with Cycle G89.

The following cycles take the oversize into consideration:

Roughing cycles: G817, G818, G819, G827, G828, G829, G83

Recess and recess-turning cycles: G81x, G82x, G86x

Cycle G83 does not delete the oversizes after cycle completion.

Parameters

P: Oversize


End of cycle G80

G80 concludes the contour description after roughing, recess, undercut

and milling cycles. A block with G80 must not contain any other commands.

Longitudinal roughing cycle G81

Transverse roughing cycle G82

G81/G82 machines (roughs) the contour area described by the current

tool position and “X, Z“. If you wish to machine an oblique cut, you

must define the angle with I and K.

Parameters

X/Z: Starting point/end point of the contour (X diameter value)

I/K: Offset/maximum infeed

I/K>0: Machine contour line

I/K


62

Clearance cycle group

Longitudinal contour roughing G817 / G818

Transverse contour roughing G827 / G828

G817/G818 and G827/G828 machine (rough) the contour area described

by the current tool position and the data defined in the subsequent

blocks – without plunge-cutting.

Tool position at end of cycle:

For G817/G827: at cycle starting point and last retraction coordinate

For G818/G828: at cycle starting point

Parameters

X/Z: Cutting limit (X as diameter value)

P: Maximum approach – Maximum infeed distance

H: Type of departure – default: 1

0: Machine contour outline after each pass

1: Retract at 45°; machine contour outline after last pass

2: Retract at 45° – do not machine contour outline

I, K: Oversizes – default: 0

Descending contour elements will not be machined.

Cutter radius compensation: is carried out

Oversizes: G57/G58 oversizes are taken into consideration

if I and K are not given in the cycle. The oversizes are

deleted upon cycle completion.

In the parameter “Active Parameters – Machining – Safety

distances“, you can change the safety distance which is

taken into account after each pass.

Example: Longitudinal roughing cycle G817

Example: Transverse roughing cycle G828


Longitudinal contour roughing with recessing G819

Transverse contour roughing with recessing G829

G819/G829 machines (roughs) the contour area described by the tool

position and the subsequent blocks – with plunge-cutting.

Tool position at the end of cycle: cycle starting point.

Parameters

X/Z: Cutting limit (X as diameter value)

P: Maximum approach – Maximum infeed distance

E: Infeed

E=0: Descending contours are not machined

No input: Feed rate is reduced as a function of approach

angle – maximum feed rate reduction: 50%.

H: Type of departure – default: 1

0: Machine contour outline after each pass

1: Retract at 45°; machine contour outline after last pass

2: Retract at 45° – do not machine contour outline

I/K: Oversizes – default: 0

Cutter radius compensation: is carried out

Oversizes: G57/G58 oversizes are taken into consideration if I

and K are not given in the cycle. The oversizes are

deleted upon cycle completion.

In the parameter “Active Parameters – Machining – Safety

distances“, you can change the safety distance which is

taken into account after each pass.

Example: Longitudinal roughing cycle G819

Danger of collision!

If the setup and tip angles of the tool have

not been defined, the tool plunge-cuts at

the plunging angle.

If the setup and tip angles have been

defined, the tool plunge-cuts at the

maximum possible angle. In this case, the

resulting contour will not be completely

finished and may need to be reworked.

Clearance cycle group

63


64

Clearance cycle group

Simple contour repeat cycle G83

G83 carries out the functions programmed in the following blocks more

than once. The following blocks contain simple traverses or cycles

without contour description. G80 ends the machining cycle.

G83 starts the cycle execution from the current tool position. Before

each pass, the tool advances by the infeed distance defined in I and K.

Machining is executed as defined in the blocks after G83, taking the

distance from the tool position to the contour start point as an “oversize“.

G83 repeats this operation until the “start point“ is reached.

Tool position at end of cycle: cycle starting point

G83 must not be nested, not even by calling subprograms.

Parameters

X, Z: Start point (X as diameter)

I/K: Maximum approach (enter I and K without sign)

No tool-tip radius compensation is carried out – you can

program cutter radius compensation separately with G41/

G42 and switch it off again with G40.

Oversizes: G57 oversizes are taken into consideration. A

G58 oversize is taken into account if TRC is active. The

oversizes remain in effect even after the end of cycle.

Danger of collision!

After each pass, the tool returns on a diagonal

path before it advances to the next pass.

Program an additional path at rapid traverse

if there is any danger that the tool could collide

with the workpiece.


Contour-parallel roughing G836

G836 machines (roughs) workpiece sections parallel to the contour. “X,

Z“ define the contour start point, the subsequent blocks describe the

contour area. G80 ends the contour description.

Tool position at end of cycle: cycle starting point.

Parameters

X, Z: Start point (X as diameter)

P: Maximum approach – Maximum infeed distance

I/K: Oversizes – default: 0

Q: Longitudinal or transverse machining – default: 0

0: Longitudinal machining

1: Transverse machining

Cutter radius compensation: is carried out

Oversizes: G57/G58 oversizes are taken into consideration

if I and K are not given in the cycle. The oversizes are

deleted upon cycle completion.

In the parameter “Active Parameters – Machining – Safety

distances“, you can change the safety distance which is

taken into account after each pass.

Clearance cycle group

65


66

Clearance cycle group

Line with radius G87

G87 machines transition radii at orthogonal, paraxial inside and outside

corners.

A preceding longitudinal or transverse element is machined if the tool is

located at the X or Z coordinate of the corner before the cycle is executed.

Parameters

X, Z: Corner point (X as diameter)

B: Radius

E: Reduced feed rate – default: active feed rate

Cutter radius compensation: is carried out

Oversizes: are not considered

Line with chamfer G88

G88 machines chamfers at orthogonal, paraxial inside and outside

corners.

A preceding longitudinal or transverse element is machined if the tool

is located at the X or Z coordinate of the corner before the cycle is

executed.

Parameters

X, Z: Corner point (X as diameter)

B: Chamfer width

E: Reduced feed rate – default: active feed rate

Cutter radius compensation: is carried out

Oversizes: are not considered


Contour finishing cycle G89

G89 finishes the contour area described in the blocks following the

cycle call.

With TRC: G41/G42 in the block after G89 switches TRC on and defines

whether the tool moves to the left or the right of the contour (with regard

to the direction of the contour).

G41: To the right of the contour

G42: To the left of the contour

TRC is automatically disabled at the end of cycle.

Without TRC: Do not define G41/G42 in the block after G89.

Parameters

B: Chamfer/rounding (at the beginning of a contour section)

B>0: Rounding radius

B0: Tool retracts by K

J: Element position (when the contour section begins with a

chamfer/rounding) – default: 1; Reference element:

J = 1: Transverse element in +X direction

J=–1: Transverse element in –X direction

J = 2: Longitudinal element in +Z direction

J=–2: Longitudinal element in –Z direction

Oversizes: A G58 oversize is taken into consideration if I is not

given in the cycle. The oversizes are deleted after cycle

completion.

Clearance cycle group

67


Recessing cycle

68

Simple recessing cycle G86

G86 machines simple radial and axial recesses with chamfers.

MANUALplus determines the position of the recess from the “tool

orientation“.

A programmed oversize is taken into account during rough-machining. In

the second step, the recess is finish-machined. The “Dwell time E“ is

only taken into account during the finish-machining.

G86 machines chamfers at the sides of the recess. If you do not wish

MANUALplus to cut the chamfers, you must position the tool at a

sufficient distance from the workpiece. Calculate the starting position as

follows:

XS = XK + 2 * (1.3 – b)

XS: Start position (diameter value)

XK: Contour diameter

b: Chamfer width

Tool position at end of cycle:

Radial recess: X – start position; Z – last recess position

Axial recess: X – last recess position; Z – start position

Parameters

X, Z: Target point (X as diameter)

I, K: Oversize/width of recess

Radial recess: I = oversize; K = recess width

Axial recess: I = recess width; K = oversize

If you do not enter a recess width, a recessing stroke results

(recess width = tool width).

E: Dwell time (for chip breaking) – default: length of time for one

revolution

Cutter radius compensation: is not carried out

Oversizes: are not considered


Axial contour cutting G861

Radial contour cutting G862

G861/G862 recesses the contour area described by the tool position and

the subsequent blocks.

Tool position at end of cycle: cycle starting point.

Parameters

P: Cutting width

I, K: Oversizes – default: 0

Q: Roughing/finishing

Q=0: Roughing only

Q=1: Roughing and finishing

E: Finishing feed rate – default: active feed rate

Calculating the proportioning of cuts

“Cutting width P“ is defined: infeeds † P

“Cutting width P“ is not defined: infeeds † 0.8 * cutting

width of the tool

Cutter radius compensation: is carried out

Oversizes: G57/G58 oversizes are taken into consideration

if I and K are not given in the cycle. The oversizes are

deleted upon cycle completion.

Recessing cycle

69


Recessing cycle

70

Simple axial cutting cycle G865

Simple radial cutting cycle G866

G865/G866 recesses the rectangle described by the tool position and

base corner “X, Z“.

Tool position at end of cycle: cycle starting point.

Parameters

X, Z: Target point (X as diameter)

P: Cutting width

I, K: Oversizes – default: 0

Q: Roughing/finishing

Q=0: Roughing only

Q=1: Roughing and finishing

E: Finishing feed rate/dwell time

for Q=0: Dwell time (for chip breaking) – default: length of time

for two revolutions

for Q=1: finishing feed rate – default: active feed rate

Calculating the proportioning of cuts

“Cutting width P“ is defined: infeeds † P

“Cutting width P“ is not defined: infeeds † 0.8 * cutting

width of the tool

Cutter radius compensation: is carried out

Oversizes: G57/G58 oversizes are taken into consideration

if I and K are not given in the cycle. The oversizes are deleted

upon cycle completion.


Axial contour finishing cut G863

Radial contour finishing cut G864

G863/G864 finishes the contour area described by the blocks following

the cycle call.

Tool position at end of cycle: cycle starting point.

Parameters

E: Finishing feed rate

Cutter radius compensation: is carried out

Axial finishing cut G867

Radial finishing cut G868

G867/G868 finishes the contour area described by the tool position and

“X, Z“.

Tool position at end of cycle: cycle starting point.

Parameters

X, Z: Target point (X as diameter)

E: Finishing feed rate – no input: active feed rate

Cutter radius compensation: is carried out

Example: Contour finishing cut G863

Example: Finishing cut G868

Recessing cycle

71


Recessing cycle

72

Simple axial recess-turning cycle G811

Simple radial recess-turning cycle G821

G811/G821 machines (recesses) the rectangle described by the tool

position and “X, Z“.

Tool position at end of cycle: cycle starting point.

Parameters

X, Z: Target point (X as diameter)

P: (Maximum) plunging depth

I, K: Oversize in X, Z – default: 0

Q: Roughing/finishing

Q=0: Roughing only

Q=1: Roughing and finishing

Q=2: Finishing only

U: Turning operation unidirectional – default: 0

U=0: Turning operation bidirectional

U=1: Turning operation unidirectional

G811: in the direction of the main spindle

G821: MANUALplus machines in the direction of the tool position

– “target point X“

B: Offset width – default: 0

O: Recessing feed rate – default: active feed rate

E: Finishing feed rate– default: active feed rate

Cutter radius compensation: is carried out

Oversizes: G57/G58 oversizes are taken

into consideration if I and K are not given

in the cycle. The oversizes are deleted

upon cycle completion.

When Q=2, use “I, K“ to define the

material to be machined during finishing.


Axial recess-turning cycle G815

Radial recess-turning cycle G825

G815/G825 machines (recesses) the contour section defined by the tool

position and the contour description in the following blocks.

Tool position at end of cycle: cycle starting point.

Parameters

X, Z: Cutting limitation (X as diameter)

P: (Maximum) plunging depth

I, K: Oversize in X, Z – default: 0

Q: Roughing/finishing

Q=0: Roughing only

Q=1: Roughing and finishing

Q=2: Finishing only

U: Turning operation unidirectional – default: 0

U=0: Turning operation bidirectional

U=1: Turning operation unidirectional

G815: in the direction of the main spindle

G825: MANUALplus machines in the direction of the tool

position – “target point X“

B: Offset width – default: 0

O: Recessing feed rate – default: active feed rate

E: Finishing feed rate– default: active feed rate

Cutter radius compensation: is carried out

Oversizes: G57/G58 oversizes are taken

into consideration if I and K are not given

in the cycle. The oversizes are deleted

upon cycle completion.

When Q=2, use “I, K“ to define the

material to be machined during finishing.

Recessing cycle

73


Threadcut cycle group

74

Universal thread cycle G31

(with and without contour description)

G31 cuts threads in any desired direction and position. You can chain

several threads. If you program the “final point X, Z”, the thread starts

at the current tool position and ends at “X, Z”. If you do not define the

“end point X, Z”, G31 will expect the following blocks to contain the

contour elements on which the thread is to be machined (contour

description). You can define up to 6 contour elements. G80 ends the

contour definition.

The infeeds in “type of infeed V=0 or V=1” are calculated on the basis

of U and I. With “types of infeed V=2 or V=3”, the infeeds are calculated

from speed and “thread pitch F”.

Parameters

X, Z: End point of thread (X diameter)

F: Thread pitch

U: Thread depth

U>0: Internal thread

U


Simple thread cycle G32

G32 cuts a simple thread in any desired direction and position (longitudinal,

tapered or transverse thread; internal or external thread). The

thread starts at the current tool position and ends at “X, Z”.

Parameters

X, Z: End point of thread (X diameter)

F: Thread pitch

U: Thread depth

U>0: Internal thread

U


Threadcut cycle group

76

Individual thread cut G33

G33 cuts threads in any desired direction and position (longitudinal,

tapered or transverse threads; internal or external threads).

The thread starts at the current tool position and ends at “X, Z”.

Parameters

X, Z: End point of thread (X diameter)

F: Thread pitch

B: Slop. length – default : 0

P: Overflow length – default : 0

C: Starting angle (if the thread start is defined relative to a contour

element which is not rotationally symmetrical) – default: 0

Q: Number of spindle – default: 0 (main spindle)

H: Reference direction for spindle pitch – default: 3

H=0: Feed in Z axis (for longitudinal and tapered threads up to a

maximum angle of +45°/–45° to the Z axis)

H=1: Feed in X axis (for transverse and tapered threads up to a

maximum angle of +45°/–45° to the X axis)

H=3: Path feed

E: Variable pitch (increases/reduces the pitch per revolution by E) –

default: 0

“Cycle STOP“ only becomes effective at the end of a thread cut.

The feed rate and spindle speed overrides are disabled during

execution of the cycle.


Metric ISO thread G35

With G35, you can cut internal and external longitudinal threads. From

the tool position relative to the final point of the thread, MANUALplus

automatically determines whether an internal or external thread is to be

cut.

Parameters

X, Z: End point of thread (X diameter)

F: Thread pitch – default: value from standard table

I: Maximum infeed – default: I is calculated from the thread pitch

and the speed

Q: Number of air cuts after the last cut – default: 0

B: Remainder cut – default: 0

B=0: Division of the last cut into 1/2, 1/4, 1/8, 1/8 cut.

B=1: No remaining cut division

“Cycle STOP” only becomes effective at the end of a thread cut.

The feed rate and spindle speed overrides are disabled during

execution of the cycle.

If you are programming an internal thread, it is advisable to

preset “F” since the diameter of the longitudinal element is not

the thread diameter. If you have MANUALplus calculate the

thread pitch automatically, slight deviations may occur.

Threadcut cycle group

77


Threadcut cycle group

78

Simple longitudinal single-start thread G350

Extended longitudinal multi-start thread G351

With G350/G351, you can cut internal and external longitudinal threads.

The thread starts at the tool position and ends at “Z“.

Parameters

Z: Final point of thread

F: Thread pitch

U: Thread depth

U>0: Internal thread

U0: Infeed from right thread flank

A


Tapered API thread G352

This cycle cuts a tapered single- or multi-start API thread.The depth of

thread increases at the overrun at the end of thread. The thread

begins at “XS, ZS“ and ends at “X, Z“.

Parameters

XS,ZS: Starting point of thread (XS as diameter)

X, Z: End point of thread (X as diameter)

F: Thread pitch

U: Thread depth

U>0: Internal thread

U0: Infeed from right thread flank

A


Threadcut cycle group

80

Tapered thread G353

This cycle cuts a tapered single- or multi-start thread. The thread

begins at “XS, ZS“ and ends at “X, Z“.

Parameters

XS,ZS: Starting point of thread (XS as diameter)

X, Z: End point of thread (X as diameter)

F: Thread pitch

U: Thread depth

U>0: Internal thread

U0: Infeed from right thread flank

A


Undercut contour G25

The function G25 enables you to machine various undercuts. These form

elements can then be integrated in roughing or finishing cycles.

If you do not define the following parameters, MANUALplus determines

the values from the diameter or, for undercuts according to DIN 76, from

the thread pitch given in the standard table:

DIN 509 E: I, K, W, R

DIN 509 F: I, K, W, R, P, A

DIN 76: I, K, W, R

Parameters

H: Type of undercut – default: 0

0, 5: DIN 509 E

6: DIN 509 F

7: DIN 76

I: Undercut depth – default: value from standard table

K: Undercut width – default: value from standard table

R: Radius – default: value from standard table

P: Transverse depth – default: value from standard table

W: Undercut angle – default: value from standard table

A: Transverse angle – default: value from standard table

FP: Thread pitch – default: is calculated from thread diameter

U: Grinding oversize – default: 0

E: Reduced feed (the undercut will be performed at the feed

rate E) – default: active feed rate

If you define the parameters, the undercut

is machined to the defined dimensions.

If you are programming an internal thread, it

is advisable to preset the “FP” since the

diameter of the longitudinal element is not

the thread diameter. If you have

MANUALplus calculate the thread pitch automatically,

slight deviations may occur.

Undercut cycles

79


Undercut cycles

80

Undercut cycle G85

With the function G85, you can machine undercuts according to DIN 509

E, DIN 509 F and DIN 76 (thread undercut). “K“ defines the type of

undercut.

See the table for the undercut parameters.

The adjoining cylinder is machined if the tool is positioned at the cylinder

diameter (“X“) “in front of“ the cylinder.

Parameters

X, Z: Target point (X as diameter)

I: Grinding oversize/depth

DIN 509 E, F: wear oversize – default: 0

DIN 76: undercut depth

K: Undercut length and type

K left undefined: DIN 509 E

K=0: DIN 509 F

K>0: undercut length for DIN 76

E: Reduced feed rate (for performing the undercut) – default: active

feed rate

Undercut angle for undercuts according to DIN 509 E and F: 15°

Transverse angle for an undercut according to DIN 509 F: 8°

Cutter radius compensation: is not carried out

Oversizes: are not considered

Undercut according to DIN 509 E

Diameter I K R

< 18 0.25 2 0.6

> 18 - 80 0.35 2.5 0.6

> 80 0.45 4 1

Undercut according to DIN 509 F

Diameter I K R P

< 18 0.25 2 0.6 0.1

> 18 - 80 0.35 2.5 0.6 0.2

> 80 0.45 4 1 0.3

I = undercut depth

K = undercut length

R = undercut radius

P = transverse depth


Undercut DIN509 E with cylinder machining G851

Undercut DIN509 F with cylinder machining G852

Undercut DIN76 with cylinder machining G853

G851/G852/G853 execute an undercut, and can also machine a

cylinder start chamfer, the adjoining cylinder and the adjoining end

face.

Meaning of the NC blocks after cycle call (example G851):

N.. G851 I.. K.. W... /Cycle call with parameters

N.. G0 X.. Z.. /Corner of start chamfer

N.. G1 Z.. /Undercut corner

N.. G1 X.. /Final point of end face

N.. G80 /End of contour description

Parameters

I: G851, G852: Undercut depth – default: value from standard table

G853: Undercut diameter – default: value from standard table

K: Undercut length – default: value from standard table

W: Undercut angle – default: value from standard table

R: Undercut radius – default: value from standard table

P: Transverse depth – default: value from standard table

A: Transverse angle – default: value from standard table

B: Cylinder 1st cut length – default: no chamfer at start of cylinder

RB: 1st cut radius – default: no chamfer radius

WB: 1st cut angle – angle at which chamfer is machined: default: 45°

E: Reduced feed (the undercut will be performed at the feed

rate E) – default: active feed rate

H: Departure type – default: 0

H=0: Tool returns to start point

H=1: Tool remains at final point of end face

Example G851

U: Finishing oversize (in area of the cylinder) –

default: no finishing oversize

FP: Thread pitch

P: Oversize (if you enter “P”, the undercut cycle

will be divided into rough-machining and finishmachining.

The value programmed for “P” is

then accounted for as a longitudinal oversize.

The transverse oversize is preset to 0.1 mm.)

Cutter radius compensation: is carried out

Oversizes: are not considered

Undercut cycles

81


Undercut cycles

82

Undercut Form U G856

G856 machines a “Form U“ undercut, finishes the adjoining end face and

machines a chamfer/rounding.

Tool position at end of cycle: cycle starting point

Meaning of the NC blocks after G856:

N.. G856 I.. K.. ... /Cycle call with parameters

N.. G0 X.. Z.. /Undercut corner

N.. G1 X.. /Final point of end face

N.. G80 /End of contour description

Parameters

I: Undercut diameter (diameter value)

K: Undercut width – If the cutting width of the tool is not defined,

the control assumes that the tool's cutting width equals K.

B: Chamfer/rounding

B>0: Rounding radius

B


Undercut Form H G857

G857 machines a “Form H“ undercut. If you do not enter W, it will be

calculated on the basis of K and R. The final point of the undercut is then

located at the corner point of the contour.

Tool position at end of cycle: cycle starting point

Parameters

X, Z: Corner point of the contour (X as diameter)

K: Undercut length

R: Undercut radius – default: no circular element

W: Plunge angle – default: W is calculated

Cutter radius compensation: is carried out

Oversizes: are not considered

Undercut Form K G858

G858 machines a “Form K“ undercut. A linear cut is made at an angle of

45°.

Tool position at end of cycle: cycle starting point

Parameters

X, Z: Corner point of the contour (X as diameter)

I: Undercut depth

Cutter radius compensation: is not carried out

Oversizes: are not considered

Undercut cycles

83


Cut-off cycle

84

Cut-off cycle G859

Cycle G859 cuts off the lathe part. If programmed, a chamfer or rounding

is also machined. At the end of the cycle, the tool returns to the start

point along a paraxial path.

Parameters

X: Cut-off diameter

Z: Cut-off position

I: Diameter feed reduction – default: no reduction

XE: Inside diameter (pipe)

E: Reduced feed rate – default: active feed rate

B: Chamfer/rounding

B>0: Rounding radius

B


Simple drilling cycle G71

G71 is used for axial and radial drillings. With stationary tools, the axial

hole must lie in the turning center.

The control starts execution of the cycle at the current tool and spindle

position.

Depending on “X/Z“, G71 decides whether a radial or axial drill hole

will be machined.

Parameters

X: Final point hole for axial drilling (X as diameter value)

Z: Final point hole for radial drilling

A: Drilling lengths – default: 0

E: Dwell time (for chip breaking at end of hole) – default: 0

V: Drill variants (feed rate reduction: 50%)

0: Without feed rate reduction

1: Feed rate reduction for through drilling

2: Feed rate reduction for spot drilling

3: Feed rate reduction for spot and through drilling

K: Drilling depth (radial drillings: radius) – default: is calculated

Drilling cycles

87


88

Drilling cycles

Deep-hole pecking cycle G74

G74 is used for axial and radial drillings. With stationary tools, the axial

hole must lie in the turning center. The hole is drilled in several passes.

The control starts execution of the cycle at the current tool and

spindle position.

Depending on “X/Z“, G74 decides whether a radial or axial drill hole

will be machined.

Parameters

X: Final point hole for axial drilling (X as diameter value)

Z: Final point hole for radial drilling

R: Safety distance – default: Value from “Active Parameters –

Machining – Safety distances“

P: 1st drilling depth – default: Drill in one operation

I: Reduction value – default: 0

B: Return distance – default: Retract to“starting point of hole“

J: Minimum hole depth – default: 1/10 of P

A: Drilling lengths – default: 0

E: Dwell time (for chip breaking at end of hole) – default: 0

V: Drill variants (feed rate reduction: 50%)

0: Without feed rate reduction

1: Feed rate reduction for through drilling

2: Feed rate reduction for spot drilling

3: Feed rate reduction for spot and through drilling

K: Drilling depth (radial drillings: radius) – default: is calculated


Thread tapping cycle G36

G36 can be used for axial and radial threads. With stationary tools, the

axial thread must lie in the turning center.

Depending on “X/Z“, G36 decides whether a radial or axial drill hole

will be machined.

Parameters

X: Final point hole for axial thread tapping (X as diameter value)

Z: End point of thread with radial machining

F: Feed per revolution – Thread pitch

B: Run-in length – default: 2 * thread pitch F1

Q: Number of spindle

Q=0: For stationary tool (spindle)

Q=1: For driven tool (auxiliary spindle)

H: Reference direction – default: 0

reference direction for spindle pitch:

H=0: Feed rate on Z axis

H=1: Feed rate on X axis

S: Retraction speed – default: Same spindle speed as for tapping

K: Drilling depth (radial drillings: radius) – default: is calculated

Drilling cycles

89


90

Drilling cycles

Thread milling cycle G799

G799 mills a thread into an existing bore hole.

Position the tool in center of the bore hole before calling G799. The cycle

positions the tool within the bore hole at the “thread end point“. The tool

then approaches with the “approach radius R“, mills the thread in a 360°

revolution, advancing by the “thread pitch F“. The cycle then retracts the

tool and returns it to the start point.

Parameters

Z: Thread starting point

K: Thread depth

R: Approach radius – default: (I – cutter diameter)/2

F: Thread pitch

I: Inside thread diameter

H: Cutting direction – default: 0

H=0: Up-cut milling

H=1: Down-cut milling

J: Thread direction – default: 0

J=0: Right

J=1: Left


Contour starting point/End-face rapid traverse G100

Geometry: G100 defines the starting point of an end-face contour.

Parameters

X, C: Target point (diameter), end angle – angle direction: see

support graphics

XK,YK: Target point (Cartesian coordinates)

Machining: The tool moves at rapid traverse along the shortest path

to the target point.

Parameters

X, C: Target point (diameter), end angle – angle direction: see

support graphics

XK,YK: Target point (Cartesian coordinates)

Z: Target point – default: current Z position

Danger of collision!

With G100 the tool moves in a linear motion – even if you only

program “C“. Use G110 to position the workpiece at a certain

angle.

End-face machining

91


92

End-face machining

End-face linear path cycle G101

Geometry: G101 defines a path on an end-face contour.

Parameters

X: Target point (X as diameter value)

C: Target angle – angle direction: see support graphics

XK, YK: Target point (Cartesian coordinates)

A: Angle to the positive XK axis

Q: Point of intersection – default: Q=0

Q=0: Near point of intersection

Q=1: Remote point of intersection

B: Chamfer/rounding

B left undefined: Tangential transition

B=0: Non-tangential transition

B>0: Rounding radius

B


End-face circular arc cycle G102/G103

Geometry: G102/G103 defines a circular arc on an end-face contour.

Parameters

X: Target point (X as diameter value)

C: Target angle – angle direction: see support graphics

XK, YK: Target point (Cartesian coordinates)

R: Radius

I, J: Center point (in Cartesian coordinates)

Q: Point of intersection – default: Q=0

Q=0: Near point of intersection

Q=1: Remote point of intersection

B: Chamfer/rounding

B left undefined: Tangential transition

B=0: Non-tangential transition

B>0: Rounding radius

B


94

End-face machining

End-face linear groove cycle G791

G791 mills a groove from the current tool position to the end point.

Tilt the spindle to the desired angle before calling G791.

Parameters

X, C: Diameter, target angle – end point of the groove (polar

coordinates)

XK, YK: End point of the groove (Cartesian coordinates)

K: Groove length – referenced to the center of the cutter

A: Groove angle – reference: see support graphics

Z: Lower edge of milling

J: Milling depth – default: begin milling at the current tool position

P: Maximum infeed – default: total depth in one infeed

F: Infeed rate (for depth infeed) – default: active feed rate


End-face contour milling cycle G793

G793 mills figures or “free contours“ on the end-face.

The figure or “free contour“ to be milled follows G793:

Figure: G304 – circle, G305 – rectangle or G307 – polygon followed

by G80.

Free contour: G100 – Start point free contour; contour description

with G101 to G103; G80 – end of contour description

Parameters

Z, ZE: Upper edge of milling, lower edge of milling

P: Maximum infeed– default: One infeed

U: Overlap factor – default: 0

U=0: contour milling

U>0: (minimum) overlapping = U*cutter diameter

R: Approach radius (radius of approach/depart arcs) – default: 0

R=0: Contour element is approached directly – followed by

vertical depth-infeeding

R>0: Cutter moves in approach/depart arcs

R


96

End-face machining

End-face surface milling cycle G797

Depending on “Q“, G797 mills surface, a polygon or the figure defined in

the command after G797.

If “Q=0“, one of the following figures is programmed in the next command,

followed by a G80:

G304 – Circle

G305 – Rectangle

G307 – Polygon

A polygon defined with G797 (Q>0) is in the center. A figure defined in

the next command may also be positioned off-center.

Parameters

X: Border diameter

Z, ZE: Reference edge, lower edge of milling

B: Width across flats – not applicable when Q=0

when Q=1: B is the remaining thickness

when Q ‡ 2: B is the width across flats

V: Edge length – not applicable when Q=0

R: Chamfer/rounding – not applicable when Q=0

R0: Rounding radius

A: Inclination angle (reference: see support graphics) – not

applicable when Q=0

Q: Number of surfaces (0 † Q † 127) – default: 0

Q=0: Figure description follows G797

Q=1: One surface

Q=2: Two surfaces offset by 180°

Q=3: Triangle

Q=4: Rectangle, square

Q>4: Polygon

P: Maximum infeed – default: in one infeed

U: Overlap factor – (minimum) overlapping =

U*cutter diameter – default: 0.5

I, K: Contour-parallel oversize, in infeed direction

F: Infeed rate (for depth infeed) – default:

active feed rate

E: Reduced feed rate for circular elements –

default: current feed rate

H: Cutting direction – default: 0

H=0: Up-cut milling

H=1: Down-cut milling

O: Roughing/finishing – default: 0

O=0: Roughing

O=1: Finishing

J: Uni-/bidirectional (when Q=1 or Q=2)

J=0: Unidirectional

J=1: Bidirectional


Figure definition end-face complete circle G304

G304 defines a complete circle on an end face. Program this figure

together with G793 or G797.

Parameters

XK, YK: Center point

R: Circle radius

Figure definition end-face rectangle G305

G305 defines a rectangle on an end face. Program this figure together

with G793 or G797.

Parameters

XK, YK: Center point

A: Angle – Reference: see support graphics

K: Rectangle length

B: Rectangle height

R: Chamfer/rounding

R0: Rounding radius

End-face machining

97


98

End-face machining

Figure definition end-face polygon G307

G307 defines a polygon on an end face. Program this figure together

with G793 or G797.

Parameters

XK, YK: Center point

Q: Number of edges (3 † Q † 127)

A: Angle – Reference: see support graphics

K: Width across flats(KW)/length

K0: Edge length

R: Chamfer/rounding

R0: Rounding radius


Reference diameters G120

G120 determines the reference diameter of the “unrolled surface

area“. Program G120 if you use “CY“ with G110 to G113. G120 is modal.

Parameter

X: Diameter

Contour start point/Lateral-surface rapid traverse G110

Geometry: G110 defines the starting point of a lateral-surface contour.

Parameters

Z, C: Target point, target angle

CY: Target point as length value

Machining: The tool moves at rapid traverse along the shortest path to

the target point.

Parameters

Z, C: Target point, target angle

CY: Target point as length value

X: Target point (diameter) – default: current X position

Lateral-surface machining

99


Lateral-surface machining

100

Lateral-surface linear path cycle G111

Geometry: G111 defines a path on a lateral-surface contour.

Parameters

Z, C: Target point, target angle – angle direction: see support graphics

CY: Target point as length value

A: Angle of inclination – Reference: see support graphics

Q: Point of intersection – default: Q=0

Q=0: Near point of intersection

Q=1: Remote point of intersection

B: Chamfer/rounding

B left undefined: Tangential transition

B=0: Non-tangential transition

B>0: Rounding radius

B


Lateral-surface circular arc cycle G112/G113

Geometry: G112/G113 defines a circular arc on an lateral-surface

contour.

Parameters

Z, C: Target point, target angle – angle direction: see support graphics

CY: Target point as length value (Reference: G120 reference diameter)

R: Radius

K, J: Center point (J as length value)

W: Angel center point – angle direction: see support graphics

Q: Point of intersection – default: Q=0

Q=0: Near point of intersection

Q=1: Remote point of intersection

B: Chamfer/rounding

B left undefined: Tangential transition

B=0: Non-tangential transition

B>0: Rounding radius

B


Lateral-surface machining

102

Lateral-surface linear groove G792

G792 mills a groove from the current tool position to the end point.

Tilt the spindle to the desired angle before calling G792.

Parameters

Z, C: Target point, target angle

K: Groove length – referenced to the center of the cutter

A: Groove angle – reference: see support graphics

Z: Milling surface (diameter)

J: Milling depth – default: begin milling at the current tool position

P: Maximum infeed – default: total depth in one infeed

F: Infeed rate (for depth infeed) – default: active feed rate


Lateral-surface contour milling cycle G794

G794 mills figures or “free contours“ on the lateral-surface.

The figure or “free contour“ to be milled follows G794:

Figure: G314 – circle, G315 – rectangle or G317 – polygon followed

by G80.

Free contour: G110 – Start point free contour; contour description

with G111 to G113; G80 – end of contour description

Parameters

X, XE: Upper milling edge (diameter), milling surface

P: Maximum infeed – default: One infeed

U: Overlap factor – default: 0

U=0: Contour milling

U>0: (Minimum) overlapping = U*cutter diameter

R: Approach radius (radius of approach/depart arcs) – default: 0

R=0: Contour element is approached directly

R>0: Cutter moves in approach/depart arcs

R


Lateral-surface machining

104

Helical groove milling G798

G798 mills a helical groove from the current tool position to the “Target

point X,Z“. “Start angle C“ defines the position of the groove beginning.

Parameters

X: Target point (diameter value) – default: current X position

Z: Groove target point

C: Start angle – default: 0

F: Pitch

P, K: Approach length, runout length – default: 0

U: Groove depth

I: Maximum downfeed – default: no downfeed

E: Reduction value for downfeed reduction – default: 1

Figure definition lateral-surface complete circle G314

G314 defines a complete circle on a lateral surface. Program this figure

together with G794.

Parameters

Z, C: Center point, angle of the center point

CY: Center point as length value

R: Circle radius


Figure definition lateral-surface rectangle G315

G315 defines a rectangle on a lateral surface. Program this figure

together with G794.

Parameters

Z, C: Center point, angle of the center point

CY: Center point as length value

A: Angle – reference: see support graphics

K: Rectangle length

B: Rectangle width (height)

R: Chamfer/rounding

R0: Rounding radius

Figure definition lateral-surface polygon G317

G317 defines a polygon on a lateral surface. Program this figure together

with G794.

Parameters

Z, C: Center point, angle of the center point

CY: Center point as length value

Q: Number of edges (3 † Q † 127)

A: Angle – reference: see support graphics

K: Width across flats (KW)/length

K0: Edge length

R: Chamfer/rounding

R0: Rounding radius

Lateral-surface machining

105


Drilling and milling patterns

106

Linear pattern on end face G743

With Cycle G743, you can machine drilling or milling patterns on the end

face. If you do not enter “ZE“, the drilling/milling cycle or figure description

from the next NC block is used – drilling cycle G71, G74, G36 or

figure G304, G305, G307 (milling).

Parameters

XK, YK: Starting point of pattern (Cartesian coordinates)

Z, ZE: Start point/final point for drilling and milling

X, C: Diameter, starting angle (polar coordinates)

A: Pattern angle

I, J; Ii, Ji: End point of pattern; hole spacing

R, Fi: Pattern length, distance to next position

Q: Number of bore holes or figures – default: 1

Linear pattern on lateral surface G744

With Cycle G744, you can machine drilling or milling patterns in which the

bore holes are arranged at a regular spacing in a straight line on the

lateral surface. If you do not enter “XE“, the drilling/milling cycle or figure

description from the next NC block is used – drilling cycle G71, G74, G36

or figure G314, G315, G317 (milling).

Parameters

Z, C: Start point, final angle (polar coordinates)

X, XE: Start point/final point for drilling and milling (diameter)

ZE, W: End point, end angle of pattern

Wi: Angle increment – distance to next position

Q: Number of bore holes or figures – default: 1


Circular pattern on end face G745

With Cycle G745, you can machine drilling or milling patterns in which

the bore holes are arranged at a regular spacing on a circular arc on

the end face. If you do not enter “ZE“, the drilling/milling cycle or

figure description from the next NC block is used – drilling cycle G71,

G74, G36 or figure G304, G305, G307 (milling).

Parameters

XK, YK: Midpoint of pattern (Cartesian coordinates)

Z, ZE: Start point/final point for drilling and milling

X, C: Diameter, angle – midpoint pattern (polar coordinates)

K: Pattern diameter – default: the current X position is transferred

A, W: Starting/final angle – position of first/last hole/figure

Wi: Final angle – distance to next position

Q: Number of bore holes or figures – default: 1

V: Direction of rotation (input is necessary only if W is defined) –

default: 0

Location of the holes/figures:

V=0: On the longer arc

V=1: Clockwise, starting at A

V=2: Counterclockwise, starting at A

Drilling and milling patterns

107


Drilling and milling patterns

108

Circular pattern on lateral surface G746

With Cycle G746, you can machine drilling or figure patterns in which the

bore holes are arranged at a regular spacing on a circular arc on the

lateral surface. If you do not enter “XE“, the drilling/milling cycle or figure

description from the next NC block is used – drilling cycle G71, G74, G36

or figure G314, G315, G317 (milling).

Parameters

Z, C: Midpoint, angle (midpoint of pattern in polar coordinates)

X, XE: Start point/final point for drilling and milling (diameter)

K: Pattern diameter

A, W: Starting/final angle

Wi: Angle increment – distance to next position

Q: Number of bore holes or figures – default: 1

V: Direction of rotation (input is necessary only if W is defined) –

default: 0

Location of the holes/figures:

V=0: On the longer arc

V=1: Clockwise, starting at A

V=2: Counterclockwise, starting at A


Tool Management

MANUALplus differentiates between the following tool types:

Lathes

Recessing tools

Threading tools

Drills

Tapping tools

Millers (cutters)

See the list at right to allocate individual tools to the tool types.

Information regarding tool data

The datum for determining the “Setup dimensions X, Z“ is based on

the characteristic shape of each tool. The graphic support window describes

the reference-point position for the selected tool type.

Tool orientation: Determines the position of the tool tip, setup angle

direction, reference-point position, etc.

Driven tool: Determines whether the main spindle or a driven tool is

turning to drill the centered bore hole.

If the direction of rotation is defined, M3/M4 is automatically generated

for the spindle or for the secondary spindle.

Tool parameters whose identification letters are shown in gray

can be entered optionally. MANUALplus uses these parameters

when specific cycle parameters are not entered, when

plunging angles or feed rates need to be calculated, etc.

With driven tools, the cutting data always refer to the

auxiliary spindle.

Lathes

Roughing tools

Finishing tools

Fine finishing tools

Copying tools

Button tools

Recessing tools

Plunging tools

Undercutting tools

Cutting-off tools

Parting tools

Threading tools

All kinds of threading tools except tapping tools

Drilling Tools

Center drills

Spot drills

Twist drills

Reversible carbide tip drills

Counterborers and countersinkers

Reamers

Tapping tools

All kinds of tapping tools

Milling tools

Slot (groove) cutting tools

End milling tools

Thread milling tools

Tool Management

109


Lathe tools

110

Lathe tools

Tool parameters

X, Z: Setup dimensions

R: Cutting radius

WO: Tool orientation (number shown in graphic support window)

A: Setup angle – range: 0°† A † 180°

B: Tip angle – range: 0° † B † 180°

DX, DZ: Wear compensation

Q: (Reference to) tool text

MD: Direction of rotation (3=M3; 4=M4) default: not assigned

TS: Cutting speed – default: not defined

TF: Feed rate – default: not defined

PT: Tool life – default: not defined

RT: Rem. dwell: Remaining tool life (display field)

PZ: Number of units – default: not defined

RZ: Remaining pieces (display field)

The direction of the setup angle depends on the tool orientation.

The figure at top right illustrates how goose-necked

roughing or finishing tools for longitudinal machining with

WO= 1, 3, 5, 7 are dimensioned.

Facing tools

Facing tools are defined in the same way as those for longitudinal

turning. The figure below explains the dimensioning of facing tools

with tool orientation WO=1 and WO=7.

Continued

X B

Z

R

A

B

A R

X

WO = 1 WO = 7

Z


Neutral tools

The tool orientation values WO=2, 4, 6, 8 are used for “neutral“ tools.

Neutral means the cutting edge is perpendicular to the X or Z axis. For

the dimensions of neutral tools: see figure at upper right.

Button tools

Tip angle “B=0” identifies the tool as a button tool. The “reference

point” for determining the “Setup dimensions X, Z” of button tools

depends on the tool orientation. See figure at bottom right for the

dimensioning of button tools with “WO=1” and “WO=2”.

X

X

R

A

B

Z

WO = 2 WO = 8

Z

X

R

X

WO = 1 WO = 2

A

Z

B

Z

Lathe tools

111


Recessing tools

112

Recessing tools

Tool parameters

X, Z: Setup dimensions

R: Cutting radius

WO: Tool orientation (number shown in graphic support window)

K: Cutting width

DX, DZ: Wear compensation

DS: Special compensation

Q: (Reference to) tool text

MD: Direction of rotation (3=M3; 4=M4) default: not assigned

TS: Cutting speed – default: not defined

TF: Feed rate – default: not defined

PT: Tool life – default: not defined

RT: Rem. dwell: Remaining tool life (display field)

PZ: Number of units – default: not defined

RZ: Remaining pieces (display field)

With recessing tools, you define the position of the reference

point with “WO”.

“DX and DZ” compensate for wear on the two sides of the

tool tip that lie next to the “reference point”. “DS” compensates

for wear on the third side of the tool tip (see figure at

bottom right).

“K” is evaluated if the corresponding parameter is not defined

in the recessing cycle.

DS

DX

DZ

DZ

WO = 3 WO = 1

DX

DS


Threading tools

Tool parameters

X, Z: Setup dimensions

WO: Tool orientation (number shown in graphic support window)

DX, DZ: Wear compensation

Q: (Reference to) tool text

MD: Direction of rotation (3=M3; 4=M4) default: not assigned

tools

TS: Spindle speed (cutting speed is not permitted with threading

tools) – Default: not defined

PT: Tool life – default: not defined

RT: Rem. dwell: Remaining tool life (display field)

PZ: Number of units – default: not defined

RZ: Remaining pieces (display field) Threading

113


Drilling tools

114

Drilling tools

Tapping tools

Tool parameters

X, Z: Setup dimensions

WO: Tool orientation (number shown in graphic support window)

I: Hole diameter / thread diameter

B: Tip angle – range: 0°


Milling tools

Tool parameters

X, Z: Setup dimensions

I: Cutter diameter

WO: Tool orientation (number shown in graphic support window)

K: Number of teeth

DX/DZ: Wear compensation

Q: (Reference to) tool text

MD: Direction of rotation (3=M3; 4=M4) default: not assigned

TS: Cutting speed – default: not defined

TF: Feed rate per tooth – default: not defined

PT: Tool life – default: not defined

RT: Rem. dwell: Remaining tool life (display field)

PZ: Number of units – default: not defined

RZ: Remaining pieces (display field)

When milling with “constant cutting speed”,

MANUALplus calculates the spindle speed

from the “cutter diameter I”.

The “Number of teeth K“ is evaluated in

“G913 Feed rate per tooth“.

I is necessary to show the tool tip in graphic

simulation.

Milling tools

115


Workpiece Generation

116

Create a Workpiece using Cycles

This section explains the steps necessary to machine

a workpiece. This machining operation is performed

in “Teach-in“ mode. This has the advantage

that, once you have machined the first workpiece,

you have a complete cycle program that can be repeated

any time.

The generated cycle program can be used in the “Program”

mode for the production of further units.

Process

Clamp workpiece

Enter and check tool data

Set up the machine

Define the workpiece datum with

“Set axis values “

Determine the tool dimensions

Switch to “Teach-in“ mode

Machine the workpiece cycle by cycle

For further information, see: “9.1 Cycle

Programming“

Entering tool data

In the “Tool Management” mode, you set up a database (T number) for

each tool. You also define the tool orientation, and depending on the tool

type, various other parameters (setup and tool-tip angle, cutter width,

etc.) . A “tool description” is assigned to each tool.

Check the data if the tools have already been entered.

1. Select the Tool Management mode of operation

Press the Process key

Place the cursor on ”Tool management”

Press the Process key again

2. Enter the tool

Look for a free space in the tool list

Switch to tool input menu with “Add”

Select tool type

Enter tool data – except setup dimensions

Enter or assign tool text

Store data with “Save”

3. Return to Machine mode

Press the Process key

Place the cursor on ”Machine”

Press the Process key again


Setting the workpiece datum

1. Machine the end face

Use a measured tool

Enter machine data in ”Set T, S, F”

Use handwheels and jog controls to

machine the end face

2. Set workpiece datum

Select ”Setup”

Select ”Set axis values”

Touch end face with tool tip

Press ”Z=0” to accept position as

datum

3. Return to main menu

Press the Menu key

Measuring tools

1. Insert the tool to be measured

2. Enter the tool number

Select ”Set T, S, F”

Enter the tool number

Press ”Save”

3. Measure the tool

Activate ”Measure tool”

Touch the diameter, then retract

Measure diameter and enter value as the ”Measuring

point coordinate X”

Touch the end face and enter ”0” for the ”Measuring point

coordinate Z”

4. Return to main menu

Press the Menu key

5. Repeat these steps for all tools

Workpiece Generation

117


Workpiece Generation

118

Creating a cycle program

1. Call Teach-in (cycle programming)

Select “Teach-in“

2. Set the program number

Activate the “program list“

Enter the number of the cycle program

Press “Select“to transfer the number of the cycle program

Switch to the alphabetic keyboard using the “Change text“ key

Enter the name of the cycle program

Confirm your entry with “Save“

3. For each cycle

Activate “Add cycle“

Select your cycle

Enter the cycle parameters

Accept the parameters with “Input finished“

Check the cycle execution using graphic simulation

Execute the cycle

Store the cycle with “Save“

4. Return to the main menu

Press the Menu key


Cycle Overview

Workpiece blank Page

Blank bar/tube 12

Workpiece blank contour ICP 12

Single cuts Page

Rapid traverse positioning 13

Approach tool change point 13

Longitudinal/transverse linear machining 13

Linear machining at angle 14

Circular machining 14

Chamfer 15

Rounding 15

M Function 13

Roughing cycles longitudinal/transverse Page

Cut longitudinal/transverse 16

Plunge longitudinal/transverse 17

ICP contour parallel longitudinal/transverse 18

ICP cutting longitudinal/transverse 19

Recessing cycles Page

Radial/axial recessing 20

Radial/axial ICP recessing 21

Radial/axial recess turning 22

Radial/axial ICP recess turning 23

Undercut H 24

Undercut K 24

Undercut U 25

Cut-off 25

Thread and undercut cycles Page

Thread cycle 26

Thread regrooving 27

Tapered thread 28

API thread 28

Undercut DIN 76 29

Undercut DIN 509 E 29

Undercut DIN 509 F 29

Drilling cycles Page

Axial/radial drilling cycle 30

Axial/radial pecking cycle 31

Axial/radial tapping cycle 32

Axial thread milling cycle 33

Milling cycles Page

Rapid traverse positioning 34

Axial/radial groove milling 34

Axial/radial figure milling 35

Axial/radial ICP contour milling 36

End-face milling 37

Helical groove milling 38

Hole patterns Page

End-face linear pattern 39

End-face circular pattern 40

Lateral-surface linear pattern 41

Lateral-surface circular pattern 42

DIN cycle Page

DIN cycle 43

More magazines by this user
Similar magazines