Can Mach4 (maybe Mach4-Industrial?) perform Fusion 360's in-process inspection? I have Mach4 Hobby and maybe my OEM post processor is just incomplete?

I see all of the commands are supported with the exception for conditionals and that appears to be in Industrial. If I upgrade to Industrial is there a post processor for Fusion that supports the inspections?

This would be a huge advantage for my shop. Especially with all of the aircraft parts we produce. The ability to programatically QA would be a huge money saver.

Thanks!

Since most of the machines that use probing use mostly the renishaw stuff; I would say no, not out of the box.
You could edit the post processor to output the the probing routines, but you would have to obtain the routines or write them yourself and make sure that the post processor puts out the correct code and arguments for your routines.

Another way you could do this.... Mach 4 emulates a fanuc 21i (I think that is the correct one); so you could just try the fanuc post processor that Fusion has and then add in the probing routines into your sub routine folder in the mach4 directory.  Again, you will have to supply the probing routines.

If you could get ahold of the renishaw probing routines for a fanuc, this second route might actually work. 

Chad,

Thanks for the response. The probing routines are actually written out as g-code from Fusion, I don't see any macros in the output. It doesn't look like (as I have read the code so far) there is anything out of the ordinary other than a whole lot of gcode conditionals and expressions. I can see the code when I used the Haas or Func PP.

There are GOTO and WHILE and IF and all of that makes Mach4 Hobby go barf. Expressions are also though out that. So the gcode seems to have Autodesk's probing routines and the data collected is either written out to a file and/or terminates the job.

All of the actual probe gcode is boiler plate stuff and supported by Mach4. If I just cut those parts out everything compiles in Mach4. Its that WHILE and GOTO and IF [#100 EQ 0] THEN #100 = 1 (Avoid dividing by zero!)

Is that sort of stuff supported in Mach4 Industrial?


Thanks,

--jb

I didn’t get it to post anything on my end. What exactly are you posting out of fusion?

Can you add a the code it outputs?  I’m curious now.

The industrial version of Mach4 can read all of the macro programming that it outputs.  Conditional statements, if, while, etc are all ok in mach4 industrial.

I couldn't find the stuff I did back a while ago when Autodesk gave me credits for the plugins but the standard work offsets probe is the same kind of stuff, minus the 2000 lines of ifs, gotos and whiles.

So take a peek at this file and that is exactly like the full inspections.

If Mach4 Industrial does the conditionals then I will buy more credits and get a nice inspection going and post the gcode. See how hard it would be to write the post processor for Mach4.

Here is some stuff with custom Func commands I suspect! Looks like the file operations is custom code;

Ahhhh! G65 is a sub-program. That might be what you are talking about. And that would be easy enough to write if Mach4 supports it.

N70 G65 P9812 Z-4.175 X50. R6.35 Q10. H1. M1. S1.
So that is parameters to a sub-program already present on specific machine you are using. In this case it is a outer/inner edge measurement in Fanuc system.

Yeah, that's what I was talking about.  The G65 is a sub program call.  The P9810 and P9812 are the programs for Safe Moves (9810) and for the work offset (9812) with the arguments on the same line (the letters and numbers).  Mach4 industrial supports G65 sub programs. 

Mach4 industrial supports G65 sub programs.

I can make all the sub stuff myself all day but the IF, WHILE, GOTO, is that also supported in Mach4 Industrial?

In-process inspection is just the killer app. I would so love to get this on my smaller machines.

Yes.  I've got OD Grinders that I made the code for that utilize all of those; I'm using Mach4 industrial on those machines.