HEIDENHAIN MANUALPLUS 4110 User manual

MANUALplus
4110
NC Software
507 807-xx
9/2004
User Training

This manual is intended to improve your operation and programming of the MANUALplus 4110.
By way of examples, the setup of the lathe, the description and measurement of tools, and the
creation of cycle programs and ICP contours are explained step by step.
These examples were created with NC software 507 807-xx.
© 2004 Dr. JOHANNES HEIDENHAIN GmbH
All texts, pictures and graphics, as well as any parts thereof, are copyrighted material. They may
only be copied and printed for private, scientific and non-commercial informative purposes,
and only if they include this copyright notice. Dr. JOHANNES HEIDENHAIN GmbH reserves the
right to revoke this permission at any time. Without obtaining written permission in advance from
Dr. JOHANNES HEIDENHAIN GmbH, the texts, pictures and graphics may not be duplicated,
archived, stored on a server, included in newsgroups, used in online services, saved on
CD-ROMs or printed in publications. The unlawful duplication and/or dissemination of the
copyrighted texts, pictures and graphics will be prosecuted according to civil and criminal law.

Basic Knowledge
Fundamentals
1
User Components
2
System Operation
3
Tool Management
Setup
4
Tool Measurement
5
Machine Setup
6
Longitudinal Machining Example
Programming
7
Surface Machining Example
8
Recess Machining Example
9
Simulation
10
Program Execution
11
12

HEIDENHAIN MANUALplus 4110 Basic Knowledge 1.1
Axis directions and reference points
Axis directions
X axis: the cross slide is referred to as
the X axis. All X-axis values that are
displayed or entered are regarded as
diameters.
Z axis: the saddle is referred to as the
Z axis.
Traverse motions:
Program a positive value to depart
the workpiece.
Program a negative value to
approach the workpiece.
Reference points
The machine datum (M) is the origin
of the machine coordinate system. As
a rule, the machine datum is at the
intersection of the Z axis with the
spindle surface.
The workpiece datum (W) is the
origin of the workpiece coordinate
system. As a rule, the workpiece
datum is at the intersection of the Z
axis with the end surface.

HEIDENHAIN MANUALplus 4110 Basic Knowledge 1.2
Lathe design
Tool in front of or behind the workpiece
Depending on the design of the lathe, the tool is either in front of or behind the workpiece. The
MANUALplus 4110 detects the design of your machine, and takes the position of the X axis into
account for the graphic support, the simulation and the machining of the workpiece.
Tool in front of the workpiece
Tool behind the workpiece
This documentation assumes a lathe with tools in front of the workpiece.

HEIDENHAIN MANUALplus 4110 Basic Knowledge 1.3
The coordinate system
Two-dimensional coordinate system
C axis
Accuracy
Positions can be programmed to an accuracy of 1 µm (0.001 mm) or 0.001°. This is also the
accuracy with which they are displayed.
The position of the tool tip is clearly
defined by its X and Z coordinates in a
two-dimensional coordinate system.
The MANUALplus 4110 recognizes
linear and circular contour
elements. A workpiece contour is
programmed by entering the
coordinates for a succession of points
and connecting them with linear or
circular contour elements.
The coordinates entered for the axes X
and Z are referenced to the
workpiece datum.
Angles entered for the C axis are
referenced to the datum of the C axis.

HEIDENHAIN MANUALplus 4110 Basic Knowledge 1.4
Tool-tip radius compensation (TRC)
Programmed paths of traverse are
referenced to the theoretical tool tip
S. The radius of the tool tip on lathe
tools causes inaccuracies when
machining tapers, chamfers and radii.
These inaccuracies are removed with
the cutter radius compensation. A
new path of traverse (the equidistant
line) is calculated to compensate for
this error.

HEIDENHAIN MANUALplus 4110 Basic Knowledge 1.5
Feed rate and spindle speed
Feed rate
You select from the following methods:
Feed rate per revolution in mm/rev
The feed rate depends on the spindle speed. The tool is moved at the programmed value for
each spindle revolution.
Feed per minute in mm/min.
The feed rate is independent of the spindle speed. The tool constantly moves at the
programmed value.
Spindle speed
You select from the following methods:
Constant spindle speed
You program the spindle speed directly. The spindle speed is independent of the diameter the
tool is working on.
Constant cutting speed
You program the spindle speed indirectly. The MANUALplus 4110 changes the spindle speed
depending on the diameter momentarily being worked on by the tool. This results in a constant
cutting speed.
Example:
Constant spindle speed:
Sections 1 to 3: identical spindle
speeds
Constant cutting speed:
Section 1: High spindle speed
Section 2: Constantly decreasing
spindle speed
Section 3: Low spindle speed
Maximum speed (speed limitation):
If the constant spindle speed that you program is greater than the specified maximum
spindle speed, the maximum speed is valid.
For constant cutting speed the speed is limited by the defined maximum spindle
speed.

HEIDENHAIN MANUALplus 4110 Basic Knowledge 1.6

HEIDENHAIN MANUALplus 4110 User Components 2.1
Data input keypad
Menu key Calls the main menu in the Machine and
Organization modes of operation
Process key Selects a mode of operation.
(Prerequisite: the MANUALplus 4110 must be in the
main menu)
Backspace key Deletes the character to the left of the cursor
Deletes the most recent error message
Switching key Toggles the support graphics between internal and
external machining
Clear key Deletes all error messages

HEIDENHAIN MANUALplus 4110 User Components 2.2
Data input keypad
Numbers (0 to 9) For value entry
Decimal point key For entering the decimal point
Minus key For entering the algebraic sign
Enter key Confirms the entered value
Store key Concludes data input and stores values
Arrow keys Moves the cursor in the indicated
direction by one position (character, field,
line, etc.)
Page forward/
Page back
Shows the information on the
previous or next screen page
Switches between two input windows
Info key Calls the error information or PLC status
display

HEIDENHAIN MANUALplus 4110 System Operation 3.1
Menu selection, soft keys
Menu selection (9-field box)
The MANUALplus 4110 presents cycles, tools and functions in the Machine and Tool
Management modes as a 9-field box. Each field of this symbol corresponds to the numerical key
that is located at the same position on the control’s numerical keypad.
The meaning of the symbol / menu item is also described in the footer.
Example: The “4” key calls the Roughing cycles, longitudinal/transverse submenu.
Soft keys
A bar at the bottom of the screen shows you the meaning of the soft keys. Press the
corresponding key to call the function.
Soft keys as toggle switches:
Some soft keys work like toggle
switches. The status that they activate
remains until it is switched off again.
Mode activated (blue background)
Mode deactivated

HEIDENHAIN MANUALplus 4110 System Operation 3.2
Machine data display
Position display
Meaning of the color of the axis letter:
Black: axis is active
White: axis is not activate
Distance-to-go display
Distance-to-go display for cycle and program execution: The distance remaining is calculated
from the current position and the target position of the active traversing command, and displayed.
Distance-to-go display in Manual mode
Axes are traversed with the handwheels: The distance-to-go is not displayed
Axes are traversed with the jog keys with protection zone monitoring active: The distance-to-
go for the Z axis refers to the protection zone position
Axes are traversed with the jog keys with protection zone monitoring not active: The distance-
to-go refers to the software limit switches
The machine data display is configurable. The display on your screen may therefore
deviate from the example shown.
Display of X and Z position:
Momentary distance from the tool tip
to the workpiece datum. The unit of
measurement is mm or inch,
depending on the setting.
Display of C position:
Momentary spindle position in
degrees (°)
Elements of the distance-to-go display

HEIDENHAIN MANUALplus 4110 System Operation 3.3
Machine data display
Protection zone status
Feed rate display
Set the feed rate
The following symbols indicate the
protection zone status:
Protective zone monitoring activated
Protective zone monitoring deactivated
Feed rate display element:
Top line: Programmed feed rate
Bottom line:
Current feed-rate override
Actual feed rate (taking the feed-
rate override into account)
Units / type of feed rate
mm/r: Feed rate per revolution
mm/min: Feed rate per minute
Cycle ON:
Cycle or program is being performed
Cycle STOP
Rapid traverse paths: The feed rate is
displayed as feed rate per minute
Set the feed rate per revolution (feed rate per minute is deactivated)
Set the feed rate per minute

HEIDENHAIN MANUALplus 4110 System Operation 3.4
Machine data display
Spindle display
Setting the cutting speed or spindle speed:
Spindle utilization
Spindle display element:
Top line: Programmed cutting speed
or spindle speed
Bottom line:
Current speed override
Actual spindle speed (taking the
speed override into account)
Little number beside the S: Gear range
Units:
Cutting speed: m/min
Spindle speed: r/min
Spindle rotates counterclockwise (M3)
Spindle rotates clockwise (M4)
Spindle stop
Display for positioning of spindle
(M19):
Top line: Target position
Bottom line: Current position
Driven tool:
Identification: The S is highlighted
The display refers to the driven tool
Set a constant cutting speed (the constant spindle speed is deactivated)
Set a constant spindle speed
Spindle utilization display element:
Current performance of the spindle
motor relative to the rated motor
performance
Bottom line: Maximum speed (speed
limitation)

HEIDENHAIN MANUALplus 4110 System Operation 3.5
Machine data display
Tool display
One tool holder (two-digit T display)
The T number indicates the position in the tool management.
Turret or automatic tool changer (four-digit T display)
The first two digits: Position in the tool management
The last two digits: Rotated position of the turret
Tool display element:
Identification letter: T
Depending on the tool carrier, either a
2- or 4-digit number follows (without
leading zeros)
Fields dx, dz: Current tool
compensation
Example “T1”
T1 from the tool manager is activated.
Example “T28”
T28 from the tool manager is activated.
Example “T101”:
T1 from the tool manager is activated.
Rotated turret position: 1
Example “T2908”:
T29 from the tool manager is
activated.
Rotated turret position: 8

HEIDENHAIN MANUALplus 4110 System Operation 3.6
Switch-on and traversing the reference marks
Switching on the machine
Axis and spindle enabling
The axes are enabled after the drives are switched on. You can traverse the axes per handwheel
or with the axis direction keys. (On some machines protective covers and guard doors must be
locked for the axes to be enabled.)
Colors of the identification letters:
White identification letters: Axes are not enabled
Black identification letters: Axes are enabled
Main switch on
In the screen dialog line, the
MANUALplus 4110 shows you step by
step how to proceed when starting the
system.
Symbol indicating the existence of current
PLC status information
Call the PLC status display:
Press the Info key
(On some machines the PLC status
display is called automatically.)
Switch the drive on
(the PLC status display closes
automatically)

HEIDENHAIN MANUALplus 4110 System Operation 3.7
Switch-on and traversing the reference marks
Traversing the reference marks
For machines with standard encoders or distance-coded encoders a reference run must be made.
Reference runs are not necessary on machines with EnDat encoders.
Sequence for reference run:
On standard encoders: A fixed reference mark is traversed. This direction of approach must be
considered.
For distance-coded encoders: The MANUALplus 4110 finds the position after a brief reference
run. (There are reference marks every 20 to 80 mm.)
Traversing the reference marks:
Pre-position the axes with
handwheels or jog keys
Press the X Reference soft
key
Press the Z Reference soft
key
Activate Cycle Start

HEIDENHAIN MANUALplus 4110 System Operation 3.8
Switch-on and traversing the reference marks
Confirm tool
The MANUALplus 4110 assumes that
the most recently active tool is still in the
tool holder.
Confirm the tool with the Tool change
button
(The tool and feed rate are enabled.)
On some machines (such as those with automatic tool changer) the acknowledgment
is automatic.