Adaption of post processor - MAXcomputer GmbH - www.max-computer.de

Go to content

Main menu:

Adaption of post processor

Customer service > Tips and tricks
 
CNC-Codes for KOSY and the Multi-Controller MCS

Revised: October 2006

Many of our customers have already a CAD/CAM-equipment and generate CNC-programs for various CNC-Machines. The following information will help you to understand the particularities of the CNC-code for KOSY.

The Way from designing to manufacturing the workpiece:

  • You draw (construct) the workpiece with the CAD-program available, either 2D or 3D and save the data of the contours in a file. The export-formats for contour-data are set up within the system, e.g. DXF in 2D or 3D, or STL in 3D.

  • The contour-data are read in a CAM-program and completed with the machining data (which tool, which contour corrections, which feed, which depth per step etc.).

  • A so-called postprocessor, which belongs to the CAM-program, generates one- or more CNC-programs for the control of the CNC-machine, e.g. a CNC-program for roughing and one for finishing.

  • The CNC-program is read by the operational system of the machine and machining is done.


In our Coordinate-System KOSY resp. our Multi-Controller MCS all these steps can be taken within our delivered CAD/CAM-Software nccad
, the CNC-code need not be open. However, if our system has to cooperate with other CAD/CAM-programs, nccad must import a suitable CNC-program, that means that the post-processor of the external CAD/CAM-software has to be adjusted to KOSY. This is not difficult and can always be done, but not all software companies allow their customers to do the adjustment; they do it for extra charge.

We know a number of producers who have made a KOSY adjustment in their CAM-program, or who let their customers do the adjustment themselves, such as:

CAM-programs with ready resp. available KOSY-adjustment:
- DeskProto
- Esprit
- millit light/KOSY
- Pictures by PC
- SurfCAM
- NC-Studio
- MarvinCAD
- Visual mill (Rhino)
- AlphaCAM
- ProNC

CAM-programs adjustable by customers (knowledge of 1-July-02)
- DeskProto
- millit pro
- SurfCAM
- edgeCAM
- Pro/ENGINEER
- PEPS
SolidCAM 2000
- WorkNC

CAM-programs, adjustable by furnisher (knowledge of 1-July-02)
- Catia
- Unigraphics

You have to keep in mind the following criteria when adjusting the post-processor to KOSY resp. to MCS:

Criteria for post-processors for KOSY

Code rules
The CNC-Code for KOSY is based on DIN/ISO 66025. Within this norm there are some rules for KOSY:

  • The code word consists of a letter (G or M) and a 1- or 2-digit number from 0 to 99.

  • The code word has to be repeated at the beginning of each line.

  • Line numbers are not allowed.

  • Values for the feed F may not stand alone in one line, but must be put at the end of a moving order.


Some examples:
G00 X10 Y30
G01 Z-1
G2 X20 Y30 I5 J0 F100

Circles
With circles and arcs the distances to the middle have always to be given completely and relative to the starting point, e.g.:
G02 X20 Y30 I5 J3

Range of values
As for any other CNC-machine, there are also limits for the values of our Coordinate-System KOSY, or our Multi-Controller MCS:

  • Values for feed F from 1 to 250 (corresp. to ca. 0,5 to 25 mm/sec.), some machines have higher values.

  • Values for coordinates from -9999.99 to +9999.99 mm, i.e. max. figures incl. special signs = 8.

  • The max. number of decimal places is free as long as there are no more than 8 figures on the whole. They are always rounded to 2 decimal places. In our normal version KOSY can only position 1/100 mm.


Some examples:
G01 X22.12 F100
G01 Y-15.7
G00 X33.123
G00 Y-55.008

Additional commands and lines at the beginning of a program
At the beginning of a CNC-program 2 documenting lines are obligatory, with any contents, e.g. date in the first line and name of editor in the second line:
06.07.2001
Pete Meyer

At the beginning of a CNC-program the following commands are necessary:

Switch on the spindle e.g. Universal spindle at relay 6:
M10 O6.1
Switch on other relays, e.g. high-frequency-spindle at relay 2:
M10 O2.1
Reference-travel to the endswitches:
G76

Additional commands at the end of the program
At the end the following commands should be given automatically:

Switch off the spindle e.g. Universal spindle at relay 6:
M10 O6.0
Switch off other relays, e.g. high-frequency spindle at relay 2:
M10 O2.0
If wanted, travel to a defined home-position:
G77
or to a freely chosen home-position, e.g.:
G00 X0 Y200 Z30

Attributes and volume of text
CNC-programs are basically text files without any special text formatting. They are so-called ASCII-files. You have to follow some rules:

  • Each line must be closed by CR LF.

  • The file must not be bigger than 8 MB.


These instructions are valid for the version nccad4.5 and higher.

 
 
Back to content | Back to main menu