Are there any plans for a Fanuc post processor in the future? Fanuc control is very popular in the USA. If not, (anyone may respond) then which post would be to closest to Fanuc? I currently use the HAAS with arcs post and it works well with minimal editing of code, but was wondering if any of the posts were closer. Thanks, and great program!
Give this a whirl. Save the attachment to your computer then run SheetCam and go to Options->machine->post processor. Clcik on the ‘Import post’ button. Using the box that appears, navigate to the post and open it.
Hello Les, thanks for the timely response. I have tried the fanuc post you sent and it seems to work fine except for: (1) It does not post the G43 tool offset and (2) It post’s the tapping feed as the thread pitch, not the actual feed in inches per minute (3) The tap rapids below work piece by .06 before tapping. It also does this on the Haas post except it rapids to .1 above work piece correctly. Example: 1/4-20 tap is run at 200 rpm. The way to calculate the feed is RPM/20= inches per minute. 200/20=10. The Fanuc also recognizes G84 for rigid tapping. I am enclosing the job files for both.
It would not let me upload the .nc files.
Here is how we set up a tapping cycle for a Fanuc:
Haas is the same, minus the M29 S200
(1/4-20 TAP)
M6T1
G0G90G54X0Y0M3S200
G43H01Z.1M8
M29S200
G84Z-.5F10.R.1
M5
M9
G0G91G28A0Y0
G90
M30
I took a look at the post and G43 had been commented out. I have put it back in.
(2) It post’s the tapping feed as the thread pitch, not the actual feed in inches per minute
This post was modified from the Mach3 post. Mach3 uses pitch rather than feed rate. I have fixed it.
(3) The tap rapids below work piece by .06 before tapping. It also does this on the Haas post except it rapids to .1 above work piece correctly.
You have the start depth set to 0.1" (0.1" below the top of the work). The post adds 1mm as a safety clearance resulting in a total of about -0.06". If you want to start above the work use a negative start depth.
Fanuc also recognizes G84 for rigid tapping.
I did it using moves rather than a canned cycle just for compatibility. This way I know exactly what is going on and I don’t have to worry about quirks in different canned cycles. The post can be modified to use canned cycles if need be.
Les, I just tried out the re-modified post on the previous jobs above and it looks like we have a winner. The code was run through 3 separate g-code simulators and no errors were reported. I also went though the code my self and saw no errors. The only edits I do now will vary on the job and how I want to run it. As far as the G84 tapping cycle, you are right in leaving that out for compatibility. If an operator wants to use G84, then it is a simple program edit. Thank you for the new post.