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. 


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. 


X: Clamping diameter 

Z: Clamping position in Z 






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. 



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. 



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. 


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 





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

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


B

18 


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”. 


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 steeper the tool plunges into the material, the 

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


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. 


19

Recessing cycles 

20 

Recessing radial 

Recessing axial 

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




Information on the cycle parameters: 

R: Rounding (on both sides of contour valley) 



B

ICP recessing radial 

ICP recessing axial 



macro. 

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

Z” and the “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. 


21


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. 


O: Recess feed rate 

R: Rounding (on both sides of contour valley) 



B

ICP recess turning radial 

ICP recess turning axial 



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. 


23


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”. 


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. 


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 


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). 


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. 


C: Measured angle (spindle angle) 

ZC: Measured position (tool position) 


U Thread depth – default: 



I: 1st cutting depth 

I


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. 



U: Thread depth – no input: 



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. 


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. 


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. 



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%). 


whether the programmed spindle speed and feed 

rate apply to the spindle or the driven tool. 

Deep-drilling axial 

Deep-drilling radial 


31

32 


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. 



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 


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. 


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 


33

Rapid traverse positioning 

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

the tool. 


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. 


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


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) 


U: Overlap factor 

No entry: Contour milling 

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

= U*cutter diameter 




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. 


U: Overlap factor 

No entry: Contour milling 

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

paths = U*cutter diameter 




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 


ICP figure axial 

ICP figure radial 


35


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“. 


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 




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. 


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 


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 


Pattern circular axial 

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


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. 



coordinate system origin“ is added to the pattern position.

Pattern linear radial 

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


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

line on the cyclindrical surface. 


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 



coordinate system origin“ is added to the pattern position. 


41

42 


Pattern circular radial 

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


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

or circular arc on the cylindrical surface. 



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 



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 


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 


45


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. 


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 



49

50 


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 


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.” 






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 






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

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 left undefined: Tangential transition 

B=0: Nontangential transition 


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 


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 


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 


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) 


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 


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

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





Example: Longitudinal roughing cycle G819 


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. 


63

64 


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. 


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) 


I/K: Oversizes – default: 0 

Q: Longitudinal or transverse machining – default: 0 

0: Longitudinal machining 

1: Transverse machining 









65

66 


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 


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 



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) 


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. 


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. 


Parameters 

P: Cutting width 


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 






69


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“. 


Parameters 


P: Cutting width 





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 



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. 


Parameters 

E: Finishing feed rate 


Axial finishing cut G867 

Radial finishing cut G868 

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

“X, Z“. 


Parameters 


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


Example: Contour finishing cut G863 

Example: Finishing cut G868 


71


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“. 


Parameters 


P: (Maximum) plunging depth 

I, K: Oversize in X, Z – default: 0 




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 


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. 


Parameters 

X, Z: Cutting limitation (X as diameter) 

P: (Maximum) plunging depth 

I, K: Oversize in X, Z – default: 0 




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 


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. 


73


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 





U


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 



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 


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. 


77


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 




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) 





A


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) 





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. 


79


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 


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° 



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.) 




81


82 

Undercut Form U G856 

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

machines a chamfer/rounding. 


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

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. 


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 



Undercut Form K G858 

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

45°. 


Parameters 

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

I: Undercut depth 




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) 




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 


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. 



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. 



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 


89

90 


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 


I: Inside thread diameter 




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 


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 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=0: Near point of intersection 

Q=1: Remote point of intersection 



B=0: Non-tangential transition 


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) 








B

94 


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 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 




O: Roughing/finishing – default: 0 

O=0: Roughing 


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 


A: Angle – Reference: see support graphics 

K: Rectangle length 

B: Rectangle height 

R: Chamfer/rounding 



97

98 


Figure definition end-face polygon G307 

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

with G793 or G797. 

Parameters 


Q: Number of edges (3 † Q † 127) 

A: Angle – Reference: see support graphics 

K: Width across flats(KW)/length 

K0: Edge length 


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 



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

Lateral-surface machining 

99


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 


A: Angle of inclination – Reference: see support graphics 








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 








B


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 


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


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 



A: Angle – reference: see support graphics 

K: Rectangle length 

B: Rectangle width (height) 



Figure definition lateral-surface polygon G317 

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

with G794. 

Parameters 



Q: Number of edges (3 † Q † 127) 

A: Angle – reference: see support graphics 

K: Width across flats (KW)/length 

K0: Edge length 




105


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 


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 


107


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 


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


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 


Plunging tools 

Undercutting tools 

Cutting-off tools 

Parting 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 


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


112 




R: Cutting radius 


K: Cutting width 


DS: Special compensation 




TF: Feed rate – default: not defined 





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








tools 

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

tools) – Default: not defined 




RZ: Remaining pieces (display field) Threading 

113

Drilling tools 

114 

Drilling tools 

Tapping tools 




I: Hole diameter / thread diameter 

B: Tip angle – range: 0°

Milling tools 



I: Cutter diameter 


K: Number of teeth 

DX/DZ: Wear compensation 




TF: Feed rate per tooth – default: not defined 





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 


117


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

354 268-21 - heidenhain

You also want an ePaper? Increase the reach of your titles

Delete template?

Save as template?