Need a SheetCAM post for Fanuc control on a KOMO router table.

[LogicIndustries]

I'm helping out a buddy whose business runs a mid-late 90's KOMO router table with a GE Fanuc control.

Their current CAM software isn't Windows 10 compatible and the company wants $20K to "upgrade" them to a version that will work.

So, I suggested that they transition to SheetCAM, because it works every bit as well as the POS they're using now and costs a fraction as much.

We did up a dummy program on some of their parts using the Mach3 post and the code looks just fine, it's just not in exactly the format that the Fanuc control wants.

I did a Google search and found a few posts here where a guy had posted a Fanuc post processor, but when I tried to download them the file always came back as missing.

Anyone got a Fanuc post they can point me at so I can get these guys up and running?

Thank you for your time.

[Les Newell]

Could you post a few examples of code generated by the old CAM. I can probably match a post to it.

[LogicIndustries]

Could you post a few examples of code generated by the old CAM. I can probably match a post to it.

I can probably do that, but I'll have to contact my buddy and have him send something over, so it'll be a day or two.

I can also post a link to the Fanuc programming manual that I've got here if you think that would help (it's a pretty big PDF though, so I'd probably just upload it to my webspace and link to it here instead of trying to attach it).

Anything else you might need?

Thank you for your time.

[LogicIndustries]

I'm going to try attaching a RAR archive with a folder full of sample programs that are known good.

We'll see how it goes.

Example Programs.rar

KOMO/Fanuc Router Sample Program Files

(6.69 KiB) Downloaded 64 times

EDIT: One thing I'd like to see changed in the new post would be to add spaces between the words inside the blocks (IE N102 G01 X5.6 Y4.3 F300.; instead of N102G01X5.6Y4.3F300.; like the sample files show) just for readability's sake. They DNC everything to this machine anyway, so program length is not a concern.

Also, just as a housekeeping issue and again for readability's sake, I would like to order the code such that the movement G codes fall directly before the geometry/coordinate words and to keep the M codes out of movement blocks (IE N130 G91 G80 G00 X5.3 Y3.1; N131 S15000 M3 M8; instead of N130 G00 G91 G80 M3 S15000 M8 X5.3 Y3.1; like is done in the sample files).

Currently it is VERY difficult to read and edit/troubleshoot the output code because it's all smashed together.

I understand that's how it used to be done when you had 15k of non-volatile memory on the board, but they're DNC'ing over gigabit ethernet now, so even doubling the file size from 5k to 10k makes zero difference to the performance of the machine.

Let me know if you need that manual from Fanuc and I'll get you a copy uploaded.

Thank you for your time.

[Les Newell]

This should be pretty close. Obviously be very careful the first few times you run code generated with this post.
To install the post, save the attachment to any convenient folder on your computer then run SheetCam and go to Options->machine->post processor. Click on the 'Import post' button. Using the box that appears, navigate to your post and open it. Go back to Options->machine->post processor and make sure your post is selected.

[LogicIndustries]

Excellent!

I will DL a copy and get to testing ASAP. As you say, we will be VERY careful and inspect the code thoroughly before running anything on the actual machine.

Thank you for taking the time to write us a special post, and for doing so in almost no time at all.

That's some serious customer service, even before the sale is made (I myself do own a copy of Sheetcam already, which is how I knew what it was capable of, but these guys haven't bought anything yet), and I/we greatly appreciate it.

I will report back with results once we've done some testing.

Thank you again for your time and effort here.

[LogicIndustries]

OK, so we wailed away at the problem for ~12hrs on Thurs and got the post to be somewhat usable with the machine. There are still issues, but we got it to spit out code that would make the machine do something.

The big issue that remains is that the post spits out an unnecessary spindle speed command (S word) in the comments that go along with the tool name, type, notes, etc that happen before a tool change, and the control on the router can't handle it at all. Doesn't throw an alarm, it just sits there and grinds forever, doing nothing because that S command happened without an M3/M4 before it (IE spindle wasn't running when the speed was commanded). Took us about three hours to figure out that was what the problem was, because no alarm code, but that was it.

I looked and looked but couldn't find anywhere in the post file that I could disable the output of this S word with those comments, so I added a "DELETE THIS ENTIRE LINE" note in the tool setup screen to at least remind me to delete it manually, but that's a Rube Goldberg solution.

I have attached the modified post processor file that we finally got to work. I did not think to highlight the changes I made when I was making them, red mist having descended and all that, but I'm sure you can see what few things I changed.

Thank you for your time.

Komo Fanuc(EDITED by LogicIndustries).scpost

(7.15 KiB) Downloaded 65 times

[djreiswig]

The speed appears several times in the post. Try removing each one individually and see which one is causing your issue. It looks like in the first two functions the speed is before the M3/M4 as you describe, so maybe that line just needs to be moved after the M line.
If it's appealing in the comments section then it might be the third function running when the tool is changed.

function OnSpindleCW()
post.ModalNumber (" S", spindleSpeed, "0.##")
post.Text (" M3")
post.Eol()
end

function OnSpindleCCW()
post.ModalNumber (" S", spindleSpeed, "0.##")
post.Text (" M4")
post.Eol()
end

function OnSpindleChanged()
post.ModalNumber (" S", spindleSpeed, "0.##")
if (spindleSpeed <= 0) then
post.Warning("WARNING: Spindle speed is zero")
end
end

[LogicIndustries]

OK, I will have a go with those suggestions and see what happens.

Thank you for your assistance.

[Les Newell]

Replace your spindle CW and spindle CCW functions with these:

Code: Select all

function OnSpindleCW()
   post.Text (" M3")
   post.ModalNumber (" S", spindleSpeed, "0.##")
   post.Eol()
end

function OnSpindleCCW()
   post.Text (" M4")
   post.ModalNumber (" S", spindleSpeed, "0.##")
   post.Eol()
end

Hopefully that should fix it.

[LogicIndustries]

Replace your spindle CW and spindle CCW functions with these:

Code: Select all

function OnSpindleCW()
   post.Text (" M3")
   post.ModalNumber (" S", spindleSpeed, "0.##")
   post.Eol()
end

function OnSpindleCCW()
   post.Text (" M4")
   post.ModalNumber (" S", spindleSpeed, "0.##")
   post.Eol()
end

Hopefully that should fix it.

Actually, the suggestion from the fellow above you fixed the problem.

It wasn't that the spindle speed was before the M3/4 in the same block, but rather that third function was outputting an S word all by itself, without an M3/4 at all, before the spindle had been started the first time, which was causing the control to lock up.

By commenting out that section of the post, that extra (and unnecessary) S word was not output, and all appears to be well now.

I've attached the current working version of the post so you've got the most current one.

Thank you for your assistance.

Komo Fanuc - Logic Style (2019-12-07).scpost

(7.16 KiB) Downloaded 59 times

[Les Newell]

Just something to be aware of - you need the OnSpindleChanged function if you use path rules or action points to modify your feed rate.

[LogicIndustries]

Just something to be aware of - you need the OnSpindleChanged function if you use path rules or action points to modify your feed rate.

Yeah, I suspected that would be the case, but the way these guys use their router, that just never comes up.

They set up one cut, output code to make that cut, then make the cut and discard the program.

They never change the feedrate or spindle speed from one shape in a setup to the next. Hell, they almost never use more than one tool in a setup. In the rare instances that they do, it's just one more tool (IE two total).

It's all super simple work, and I doubt very seriously that they'll ever use the path rules functionality at all.

Their current CAM (if you can call it that) is just an AutoLISP script plugin for AutoCAD that applies offsets and generates code from canned recipes. SheetCAM is far more powerful CAM IMO.

Anyway, if it comes back up in the future where they need the function, we can always remove the comment marks and go back to how it was before. That's why I didn't delete it outright.

Thank you for your assistance.

[Les Newell]

This version should fix the problem properly so spindle override will work. It only outputs spindle speed if the spindle is on.

[LogicIndustries]

This version should fix the problem properly so spindle override will work. It only outputs spindle speed if the spindle is on.

Excellent!

I will get this new version to them and let you know how it shakes out.

Thank you for your assistance.