Solidcam to EMC2 post processor

Hi All.
I searched Linuxcnc.org for working post processor from SolidCam to EMC, and did not found any.
So I changed existing FANUC (for Mill) and FANUC0T (for Lathe) in SolidCam.
It worked for me in SolidCam 2008SP12 and SolidCam2009 SP0. I am using EMC2.2

To use modified post processor extract attached archive (which includes both post processors) to C:\Program Files\SolidCAM2009\Gpptool , choose to override existing files (you can backup existing files just to be safe).

This is my first post in this forum, so if I made any mistakes I want to apologize in advance.

Can you please explain what changes are necessary? I'm trying to make a postprozessor for Unigraphics NX6 perhaps this could help me.

Axel

axel88 wrote:

Can you please explain what changes are necessary? I'm trying to make a postprozessor for Unigraphics NX6 perhaps this could help me.

Axel

hi Axel

there is not alot to edit if you have a good standard fanuc post, just check your cycles, and G80 line on end of cycles like drilling, as fanuc can take G80 Zxx EMC likes G80 G00 Zxx

cutter comp drive lines is also worth a check.

Lathe wise there are not many cycles there so most of it just system output code
should not take long if you have a good starting ground and know how to edit a post.

rob

This post processor seems to work alright for me with Solidcam and EMC2. Although, I tried performing a Transformation->Translate->Matrix, which uses WHILE loops. When I tried to load the code, EMC2 didn't recognize the structure of the WHILE loop and gave me an invalid character error. I'm pretty sure that the post processor needs to be modified but I'm not sure how. My generated code looks like this... Any help would be greatly appreciated.

(CNC-HOUSING-CENTER.TAP)
( MCV-OP ) (18-JAN-2012)
(SUBROUTINES: O2 .. O6)
G90 G17
G80 G49 G40
G54
G91 G28 Z0
G90
M01
N1 M6 T1
(TOOL -1- MILL DIA 3.97 R0. MM )G0 X0. Y0. Z10. S15000 M3
M8
#21 = 0
WHILE [#21 LT 2] DO 1
(

---

)
(TAB ROUGHING - FRONT - POCKET)
(

---

)
G10G91 L2 P1 X0. Y42. Z0.
G90
#21 = #21 + 1
G1
END 1
G10G91 L2 P1 X0. Y-84. Z0.
G90
G91 G28 Z0
G90
M01
N2 M6 T8G0 X-14.852 Y-34.5 Z10. S1000 M3
M8
#21 = 0
WHILE [#21 LT 2] DO 1
(

---

)
(OUTER CHAMFER - FRONT - PROFILE)
(

---

)
G0 X-14.852 Y-34.5 Z15.
Z7.75
G1 Z5.625 F100
X-33.295 F500
G2 X-34.855 Y-33.818 R2.125
X-35.156 Y-33.485 R18.875
X-35.688 Y-32.079 R2.125
G10G91 L2 P1 X0. Y42. Z0.
G90
#21 = #21 + 1
G1
END 1
G10G91 L2 P1 X0. Y-84. Z0.

Also, the section of the post processor that I think needs to be modified is shown below.

@loop
local integer var_num

var_num = loop_level + 20
{nb, '#', var_num, ' = 0'}
{nb, ' WHILE [#', var_num, ' LT ', loop_count, '] DO ', loop_level}
endp

;

---

@end_loop
local integer var_num

var_num = loop_level + 20
{nb '#', var_num, ' = #', var_num, ' + 1'}
{nb 'G'home_number}
{nb ' END ', loop_level}
endp

;

---

Here's is my modified Solidcam to EMC2 post processor. It has been modified so that it can do arrays of parts that have multiple tool changes without duplicating all of the tool changes in your array of parts. ie. Instead of going through all of the tool changes on part 1 and then indexing to part 2, effectively duplicating all of your tool changes. Run tool #1 on an array of parts, then tool change, then tool #2 on the same array of parts, etc..

Hi everyone,

I'm having trouble with generating G-code from SolidCAM2012.
I tried to choose fanuc and fanuc5a machines and also tried to set the post processor (at machine settings) to the one which is for LinuxCNC, but I faced to two cases:
1.: if i choose the postprocessor which is made for LinuxCNC: error in SolidCAM. It sais "File LINUXCNC.GPP, Line 6. variable 'Peck' is unable to recognize", and the same error for other variables too.
2.: if i choose the original SolidCAM postprocessor file (fanuc or fanuc5a), it generates a G-code, that LinuxCNC unable to load because a bunch of unknown g-codes and d-codes.

Does anyone has experience with Solidcam2012 vs. LinuxCNC? I am very pissed off, I want to make is work for 3 days...

Help please!!

Thank you!
Adam

have you try'd Robo-Dan's post processor ?

if you can post your solidworks files and gcode as an attachment i'll take a look and see if we can find the problem

which version post processor and which version of linuxcnc you are using will help
also the exact version of solidworks / solidcam and service packs used etc .

I feel that it may be just a few updates needed to the post processor .

Thank you for the quick and very helpful reply cncbasher!

Trying Robo-Dan's GPP file, and selecting Fanuc5a machine in SolidCAM solved my problem!
I don't really know, why i haven't try this one earlier... to be honest i thought the problem is somewhere else, because I tried several GPP files and the problem seemed to be in choosing the appropriate way of generating the code and the settings of the pre-defined machines.

So, for everyone who want to use Solidcam2012 with LinuxCNC:
1.: Reame Robo-Dan's attached postprocessor file to something (LinuxCNC.GPP for instance) and copy it to .../Programfiles/SolidCAM2012/Gpptool/
2.: Select machine "Fanuc5a" at CAM-Part settings
3.: Go into Fanuc5a's settings by double-clicking on it
4.: In Machine ID Editor (which pops up) select the new, freshly copied postprocessor file on the right
5.: It should work!


Thank you and also Robo-Dan so much again!

Adam