Adaption of post processor - MAXcomputer GmbH - www.max-computer.de
Main menu:
Adaption of post processor
Revised: December 2020
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.
This information is for nccad from version 8 up.
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.
- For CAM the contour-data must be exported and buffered normally in the following formats
a) DXF for 2D-drawings and 2 1/2D-milling
b) STL for 3D-bodies and 3D-milling or 3D-printing.
Many CAM-programs can import other formats, too.
Note: The two formats DXF and STL can be imported directly in nccad to use the CAM-module of nccad. - The exported file is imported 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.
It must take into account the specific code elements and properties. Each machine resp. control unit has got its individual "dialect". Before generating the NC-code the machine resp. the appropriate postprocessor must be chosen. - The CNC-program is read by the operational system of the machine and machining is done.
You have to use 3 different programs (CAD, CAM and CNC) and 2 times export/import is necessary.
Compatibility problems can occur.
In our Coordinate-System KOSY resp. our Multi-Controller MCS all these steps can be taken within our delivered CAD/CAM-Software nccad, without compatibility problems.
Of course we want to support customers who wants to continue working with his favorite CAD-program using more complex or special functions which nccad does not offer. If our system has to cooperate with other CAD/CAM-programs, nccad must import a suitable NC-program, that means that the post-processor of the external CAD/CAM-software has to be adjusted. This is not very difficult and can always be done, but not all software companies allow their customers to do the adjustment themselves; they do it for extra charge.
We know a number of producers who have made an adjustment in their CAM-program, mostly under the name of "KOSY" or who let their customers do the adjustment themselves, such as:
CAM-programs with ready resp. available KOSY-adjustment (list without guarantee):
- Autodesk Fusion 360 (available on Autodesk Homepage)
- DeskProto
- Esprit
- millit light/KOSY
- Pictures by PC
- SurfCAM
- NC-Studio
- MarvinCAD
- Visual mill (Rhino)
- AlphaCAM
- MTS
CAM-programs adjustable by customers (knowledge of 1-July-02)
- DeskProto
- millit pro
- edgeCAM
- Pro/ENGINEER
- PEPS
- SolidCAM xx
- 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 (Nxxx) are allowed but not necessary.
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
We recommend to make a test with a simple example
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 5 to 400 (corresp. to approx. 0,5 to 40 mm/sec.), some machines have higher values.
Values for coordinates from -9999.999 to +9999.999 mm, i.e. max. figures incl. special signs = 9.
The max. number of decimal places is free as long as there are no more than 9 figures on the whole. KOSY 1/2 can position only 1/100mm, KOSY3, 4,5, and HE, as well as the control unit MCS can do values of 1/1000 mm (1µm), but - depending on equipment - postion to 1,25 µm only, for example.
Some examples:
G01 X22.12 F100
G01 Y-15.7
G00 X33.123
G00 Y-55.008
Additional commands and special functions
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:
06.07.2012
Pete Meyer
More text lines must be executed as comment lines, therefore: ; (semicolon) at the beginning, e.g.:
; CAMx PP for KOSY
Comments at the end of a sentence are introduced by ; (semicolon), e.g.
G00 X100 Y100 Z50 ; safe start position
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 ;230V ON
^ letter O (Output)
or
Switch on other relays, e.g. high-frequency-spindle at relay 2:
M10 O2.1 ;spindle ON
or
Reference-travel to the endswitches:
G76 (all axes) or G76 X0 or G76 Y0 or G76 Z0
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.
File name
- The file must get the extension *.KNC (KOSY NC-program).