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