ap-4-12.dvi


Acta Polytechnica Vol. 52 No. 4/2012

Creating a Multi-axis Machining Postprocessor

Petr Vavruška1

1
Department of Production Machines and Equipment, Faculty of Mechanical Engineering, Czech Technical University
in Prague, Horská 3, 128 00 Prague 2, Czech Republic

Correspondence to: p.vavruska@rcmt.cvut.cz

Abstract

This paper focuses on the postprocessor creation process. When using standard commercially available postprocessors it

is often very difficult to modify its internal source code, and it is a very complex process, in many cases even impossible,

to implement the newly-developed functions. It is therefore very important to have a method for creating a postprocessor

for any CAM system, which allows CL data (Cutter Location data) to be generated to a separate text file. The goal of

our work is to verify the proposed method for creating a postprocessor. Postprocessor functions for multi-axis machining

are dealt with in this work. A file with CL data must be translated by the postprocessor into an NC program that has

been customized for a specific production machine and its control system. The postprocessor is therefore verified by

applications for machining free-form surfaces of complex parts, and by executing the NC programs that are generated

on real machine tools. This is also presented here.

Keywords: postprocessor, NC program, interpolation.

1 Introduction

Most CAM (Computer Aided Manufacturing) sys-
tems are able to export general data, called CL data
(Cutter Location data), in a text file. The CL data
file consists of information about the coordinate sys-
tem, tools, etc. It is necessary to adjust this CL data
file for a specific production machine. Each produc-
tion machine has a different structural design and a
unique control system. A file with CL data is then
translated by the postprocessor into an NC program
that has been adapted to a specific production ma-
chine and its control system, see [3].

Figure 1: NC program creation process

Especially for multi-axis machining, it is neces-
sary to include further features for generating the
relevant NC programs, e.g. the location of the ro-
tary axes of the machine tool. However, when using
standard commercially-available postprocessors, it is
often very difficult to modify its internal source code
and it is a very complex process, in many cases even

impossible, to implement the newly developed func-
tions. It is therefore very important to be able to cre-
ate a postprocessor for any CAM system, which gen-
erates CL data to a separate text file. Subsequently,
the postprocessor that is created must be verified by
applications for machining free-form surfaces of com-
plex parts, by executing the NC programs that are
generated on a real machine tool.

2 Method for creating a

postprocessor

The postprocessor falls within the chain shown in
Figure 1, which illustrates the idea that the post-
processor is not necessarily a part of the CAM sys-
tem, but can also be a stand-alone program, and is in
essence a compiler. The issue of compilers is taught
e.g. at the Faculty of Electrical Engineering (CTU
in Prague), and can be found in [2]. The CL data
file contains all necessary information for creating a
specific NC program. Besides the coordinate system
and tools mentioned above, a CL data file consists
of information about the toolpath, the orientation of
the tool, tool changes, the feed-rate value, the spindle
speed value and the direction of rotation, the desired
cooling, the type of interpolation, etc. A method
for creating a postprocessor for CL data analysis has
been proposed. This method is based on using soft-
ware that can be found as open-source or free soft-
ware. FLEX and BISON software generate source
codes in C language for lexical and syntactic ana-
lyzers on the basis of lexical and syntactic analysis

113



Acta Polytechnica Vol. 52 No. 4/2012

rules created by the programmer. The software is
distributed under General Public License (GPL) and
forms part of the GNU project. Lexical and syntac-
tic analysis is needed to decode the input text file
(CL data). After this decoding process, the data is
passed to other postprocessor functions, where it is
further processed according to the programmed al-
gorithms. Other postprocessor functions (transfor-
mations, modality of words, block formatting, etc.)
will be written in the source code of C language as
a separate text file. The final software that we need
is a compiler of source codes written in C language
to obtain a binary file of the postprocessor. A com-
piler called Dev-C++ is used for this purpose, but of
course a different C language compiler can be used.
This is summarized in Figure 2.

Figure 2: Postprocessor creation method

3 Postprocessors for multi-axis

milling

For more than three-axis machining, it is necessary to
transform the coordinates of the tool reference point
in each block of CL data. The transformation de-
pends on the nomenclature of the actual machine
tool. It is also necessary to consider the required ma-
chining principle. In multi-axis machining there are
two basic machining principles: positioning (index-

ing), and continuous machining. In the case of posi-
tioning, the workpiece is set to the desired position
using rotary axes, and the cutting moves are realized
using linear axes only. The postprocessor then trans-
forms the coordinates according to the same angular
coordinates. The limits of the rotary axes are checked
only in the block by setting the desired positions of
the rotary axes. Whereas in continuous machining
it is necessary to check the positions of the rotary
axes of the machine tool in each block, in the case
of four-axis machining we can speak of plane coor-
dinate transformation (the coordinates of the linear
axis, which is parallel to the axis of rotation, remain
unchanged), and the axis of rotation also usually does
not have limits. Figure 3a shows the nomenclature of
the Haas TM1 four-axis machine tool, which is avail-
able at the Department of Production Machines and
Equipment (CTU in Prague, Faculty of Mechanical
Engineering).

Five-axis machining is a larger issue. In this case
we must consider the spatial transformation, which is
ambiguous. In a CL data file, we can find positions of
the tool that may be represented by two identical po-
sitions on the machine tool, see Figure 4a. We know
only the position of the tool reference point and the
orientation of the tool axis, and we look for the posi-
tion of all machine tool axes. This is an application
of inverse kinematics. Multi-axis machine tools are
distinguished by their nomenclature (location of the
rotary axes), and hence transformation equations can
be created. The transformation equations are usually
created using transformation matrices, which can be
found e.g. in [4]. Figure 3b shows the kinematics
of a five-axis machining center, which is available at
the Department of Production Machines and Equip-
ment (CTU in Prague, Faculty of Mechanical Engi-
neering). It is based on the MCV 1000 three-axis
milling machine tool (made by Kovosvit MAS), and
is supplemented by the rotary/tilting table made by
Nikken. In this case, the two rotary axes are on the
work-piece clamping device. This is known as the
table-table concept. The transformation matrices for
this machine can be found in [5].

Figure 3: Nomenclature of machine tools (a – four-axis Haas TM1, b – five-axis MAS MCV 1000)

114



Acta Polytechnica Vol. 52 No. 4/2012

Figure 4: Range of movement of the tilting axis (a – ambiguous positions, b – limits of tilting axis)

Postprocessors for continuous multi-axis machin-
ing must include solutions for the limits of the rotary
axes. It is usually possible to specify the limits of
machine tool axes and then during transformation
the postprocessor checks the positions of the axes in
the whole machine tool. However, in the event that
the subsequent position of some rotary axis would
exceed the limit of this axis, and in the next NC
program block the postprocessor generates the posi-
tions of the alternative machine tool axes (and they
do not exist), without the tool retracting from the
workpiece in order to change the positions of the ma-
chine tool axes, then a collision might occur between
a tool and a workpiece. This is because a linear inter-
polation is programmed between the two consecutive
blocks in the NC program. Other places in the NC
program where this problem may occur are called
stationary points, where the tool axis is parallel to
the rotary axis C (in the case of the five-axis ma-
chining tool mentioned above). In fact, there is no
line during multi-axis machining using linear interpo-
lation, but a spatial curve is created because of the
existence of rotary axes. In the case of very short
increments of the toolpath, the curve approaches a
straight line, but when the angular coordinate is too

high the curve is visible on the surface and the work-
piece is devalued. However if these critical points
are dealt with using a proprietary algorithm, the im-
pending destruction of the product is averted. The
limits of tilting axis B of the MAS MCV 1000 ma-
chine tool are shown in Figure 4b as “LIM 1” and
“LIM 2” (“-LIM 2” is the mirrored “LIM 2”, as an
area of possible ambiguous solutions for the position
of the tilting axis). Figure 5 shows a difference be-
tween the characteristics of the coordinates of two NC
programs, the first without using the algorithm for
flipping of the tilting axis over the stationary point
(characteristics of the coordinates in Figure 5a), the
second with this algorithm (characteristics of the co-
ordinates in Figure 5b). The green box in Fig. 5b
surrounds the area from the stationary point to the
point where the limit of tilting axis B is reached.
If the tool is at a safe distance from the workpiece,
the machine tool axes can change the positions, and
the machining process can continue after the tool ap-
proaches the workpiece again. The approach is im-
plemented in such a way that at first the tool moves
at a rapid speed in the position near the surface,
and then it moves at the working feed-rate to the
cut.

Figure 5: Usage of the algorithm for flipping over the stationary point (a – without, b – with)

115



Acta Polytechnica Vol. 52 No. 4/2012

Figure 6: Testing the four-axis milling postprocessor

The format of the NC program depends on the
control system used in the machine tool. There is
also a common language for NC code — the ISO lan-
guage (ISO code), but the producers of the control
systems are still trying to bring new features in their
systems. In order to generate these functions in the
NC program correctly, the postprocessor has to iden-
tify areas in the CL data file where these functions
can be used. The postprocessor can be extended by
non-standard functions that are derived from specific
requirements in production, or from practices within
the company where the postprocessor will be used.
In these two cases it was necessary to adjust the NC
program to the requirements of the Haas control sys-
tem (in the case of Haas TM1) and to the require-
ments of Heidenhain iTNC 530 (in the case of MAS
MCV1000). An adjusted ISO format had to be used
for the Haas control system. The part (blade) for
testing the postprocessor functions is shown in Fi-
gure 6, together with a part of the NC program (the
block with the tool change is marked in red, and the
blocks with tool length and radius compensation are
marked in green) and the real machining of the blade.

Heidenhain control systems allow for program-
ming using the adjusted ISO language, and along
with it they also offer programming in their own
language called “dialogue”, see [1]. This language
is very different from the ISO code. Due to the
machine operator requirements, it was necessary to
modify the postprocessor so that the format of the
NC program corresponds with this language. A com-
parison between a CL data section and the corre-
sponding section of an NC program is shown in Fi-
gure 7, where the blocks that correspond to each
other are marked in blue and green, and the feed rates
programmed through the parameters are marked in
red.

The final figures show a test of the postprocessor.
The creation of toolpaths (for roughing and for fin-
ishing) is shown in Figure 8, where the test part is
an impeller. After this part was machined on a ma-
chine tool (see Figure 9a), the surfaces were measured
using a Mitutoyo coordinate measurement machine,
see Figure 9b. It can be surely stated that the post-
processor algorithms for multi-axis milling have been
verified.

Figure 7: CL data in comparison with the NC program (a – CL data, b – NC program)

116



Acta Polytechnica Vol. 52 No. 4/2012

Figure 8: Testing toolpath creation (a – roughing, b – finishing)

Figure 9: Finished blade (a – after machining, b – during the measurement)

4 Conclusion

This paper has summarized my findings from design-
ing and verifying the multi-axis machining postpro-
cessor creation method. The method is based on
translating a text file with CL data. A CL data
file is generated by the CAM system, and then it is
translated by the appropriate postprocessor into an
NC program. The appropriate postprocessor must
be created for a specific CAM system, a particular
machine tool and a control system. The multi-axis
postprocessor method has been verified by the CA-
TIA CAM system. An experiment machining real
parts on CNC machine tools proved the functionality
and the applicability of the postprocessor algorithms.
This postprocessor creation method can also be eas-
ily applied (after analysis of the actual format of the
CL data and adaptation of the lexical and syntac-
tical analyzers of the postprocessor) to other CAM
systems.

Acknowledgement

The results have been obtained with the support
of the 1M0507 Czech Ministry of Education, Youth

and Sports grant “Research Center of Manufacturing
Technology”.

References

[1] iTNC 530, př́ıručka uživatele – programováńı po-
dle DIN/ISO. Traunreut : Heidenhain, 2002.
463 p. (in Czech)

[2] Melichar, B. et al.: Konstrukce překladač̊u. I.
a II. část. 1. edition, Prague : CTU, 1999. 636 p.
ISBN 80-01-02028-2. (in Czech)

[3] Ryb́ın, J.: Automatické ř́ıdićı systémy. 1. edition,
Prague : CTU, 1991. 150 p. ISBN 80-01-00694-8.
(in Czech)

[4] Stejskal, V., Valášek, M.: Kinematics and dynam-
ics of machinery. 1. edition, New York : Marcel
Dekker, INC., 1996. 494 p. ISBN 0-8247-9731-0.

[5] Vavruška, P., Rybńın, J.: Postprocessing and its
applications on free-form surfaces. Research re-
port no. V-08-088. CTU in Prague, Research Cen-
ter of Manufacturing Technology, 2008. 54 p. (in
Czech)

117