Solidcam to EMC2 post processor

Adam ,
attach files as a zip archive should work dependant on file size
if you have problems attaching , send it to me directly and i'll make sure it makes it

Lukas,
your problem I think relates to perhaps typo's , you say Dely etc it should be Delay colent should be coolent

Thanks!

So, it worked as a .zip... find my files in my previous post!

Good luck!
Adam

cncbasher wrote:

Adam ,
attach files as a zip archive should work dependant on file size
if you have problems attaching , send it to me directly and i'll make sure it makes it

Lukas,
your problem I think relates to perhaps typo's , you say Dely etc it should be Delay colent should be coolent

Lukas ,
let me know what you find , I don't at the moment have solidcam 2013 installed , so cant check directly , but I will be upgrading in the next day or so
once I have my databases backed up . so any problems i'll take a look at

Lukas,

When I had trouble with making this stuff work, I also faced to these variable-error massages.
Especially when I chose Fanuc (not the Fanuc5a) machine and tried to set a previous version of postprocessor-file (downloaded also from this forum).
These files (I attached) solved the problem for me, hope that they also work in SolidCAM 2013...

.

The variables were renamed in the new versions till 2011 .

mist_coolant was renamed to mach_mist_coolant
flood_collant was renamed to mach_flood_coolant

and so on ..

The LINUXCNC.GPP post processor file works well in SolidCAM 2013 for me.

However, be aware that the G43 command has been commented out in it, so G code created with this will not carry out tool length compensation. If you don't carry out any tool changes in a given job you won't notice, but when you do change to a tool with a different length you may well suffer a tool crash as I did yesterday.

It serves me right for not checking my code properly before running it, but just a word of warning for others who may want to use this file.

The relevant lines are numbers 399 & 400 as shown below:

;gcode = 43
;{nb, 'G'gcode, ' H'tool_number, ' D'(tool_number+30), ' '}

Remove the leading ; to re-enable the lines. I also think that the D parameter is not supported in G43 for LinuxCNC, so I removed that part from the second line.

Ben

I'm testing this post processor on SolidWorks2014. I can use in milling operations, and linuxcnc accept the code (simulation only for now). But for the turning version, I can't find the machine FANUC0T, so I'm wondering if I need the FANUC0T.VMID file to be able to select the machine.

João

I found the post processor by Robo Dan and other forum members to be very useful for starting out. Along the way as I've added parts to my G0704 mill I have modified it to support these things:

• Auto Z touch off plate code from OrangeCat (calls M600 at beginning of file and intercepts M6 T# calls to measure each tool)
• G33.1 rigid tapping support (must have mill setup to do rigid tapping).
• Clearer naming. Instead of Fanuc5a the controller is called LinuxCNC.
• Prints out a list of all the tools used in the job at the top of the gcode output including their descriptive names.
• Uses LinuxCNC DEBUG command to print out the tool needed at each tool change.
• Outputs gcode files with .ngc extension instead of .tap
• General cleanup of the commented out code
• Increased precision for all coordinates. Helps with TPI during tapping
• Tool Length offset (Gcode 43) is commented out on lines 372 for the version without auto touch off. If you change tools or use the TLO table in linuxcnc you'll probably want to uncomment it

CAVEATS

I have not tested everything possible. Specifically I have not done any 4th axis stuff or any tool compensation. The way I use Solidcam is to select all the operations in a setup and generate a single gcode file for these. As long as it simulates right in Solidcam, linuxcnc will work the exact same way. I have tested nothing with changing planes or multiple setups in one file (ie MAC 1, MAC 2 in same file). I create a new file for each machining position since I need to take the part out of the vise, change it around and re-zero anyway.

If you use the auto z touch off version make sure you clear the TLO before *each* job (ie hitting start). I have a button to clear the TLO using pyvcp and an led that shows me if the TLO is currently set.

I have also not touched nor added the lathe controller. I will be looking at that in the next 6 months as I get my lathe converted to a simple 2 axis lathe.

INSTALLATION

Unzip the zip file and copy all 4 of the files to your Gpptool directory. Use windows search if you don't know where the Solidcam Gpptool directory is. Decide whether you want to run the auto z touch off version or not and then rename the version you want to use to LINUXCNC.GPP. Afterwards fire up SolidCam and LinuxCNC will appear in your list of controllers.

Unless you have an auto z touch off plate and have remapped M600 and M6 in linuxcnc you really don't want to run the auto touch off version.

BUGS

I know of only one strange situation with the auto touch off version. If you abort in the middle of the job and then want to restart on a certain line the Auto Z touch off measuring doesn't work properly. The proper procedure is to clear the current tool length offset, use the MDI to issue M600, Start the program again (I usually start right at a tool change). Practice, or watch the Z height closely or you will bury a tool in the work piece.

YMMV, not responsible if you destroy your machine or it kills your dog.