topic Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c in Fusion Manufacture Forum

Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 codes

Jay_Bolyard — Mon, 24 Oct 2016 15:41:24 GMT

Fusion 360 - Posting for Mach 3 Mill and Tormach PCNC 1100

I have searched the forum and failed so far - I apologize if this has been covered already. I'm an enthusiast user - Not for Hire.

- In my reading and attempting to learn about posting for Mach 3 and Tormach, I read about post process configuration settings for SOME post processors which will then result in the operations being written as subroutines. I really like this option because I can have one NC file and quickly comment out the operation calls I don't want to run with the tool currently installed and then run. Doesn't seem this option exists in the standard Mach 3 mill configuration?

- Also - I want to turn off any manner of tool compensation - No G41 through G49 in my code whatsoever. I'm using a shared Tormach and I'm not able to set tools and use tool compensation - I must manually insert and rezero each tool as I go.

- I would rather not have to edit the NC out of F360 to delete any references to G41-G49 manually - that's recipe for making a mistake and crashing something or ruining a workpiece

Question:

- Is there a way to get the Mach3 Mill post processor configured to act this way in F360?

- Don't use any tool compensation (Absolutely no G41-G49's)

- Output individual operations as subroutines

- Should I try using a different postprocessor configuration? Suggestions?

- Has anyone done this or similar already?

- I'm not a JAVA programmer.... should I try to learn?

Thank you,

Jay Bolyard

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

daniel_lyall — Mon, 24 Oct 2016 19:13:04 GMT

it's all doable with Mach3.

does the tormach have the ATC ???

you need to go on the mach3 web site and forum to get the info for the sub programming it's all in there for what Mach3 needs, all programs are a tickle different.

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

daniel_lyall — Mon, 24 Oct 2016 21:08:46 GMT

@Jay_Bolyard

I forgot to add you use the manual NC to put the code into your G code it's under setup.

one of the other Guys hopefully will chime in and say how to use it.

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

Jay_Bolyard — Tue, 25 Oct 2016 11:59:23 GMT

No - the Tormach I'm using does not have an ATC. Each tool must be manually inserted into an R8 collet in the spindle and re- Z- Zero.

I know that Mach 3 can do subroutines - I'm trying to get F360 to write them.

Also trying to ensure no G41-G49's are written to the NC code.

Anyone written a custom post for this or know of the best surrogate I could use? Fanuc?

Thanks,

Jay

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

daniel_lyall — Tue, 25 Oct 2016 18:21:50 GMT

No fusion can not write subroutines, you have to do that.

sinces you have to manually change tools, you don't need to remove anything you set Mach3 to stop on M6 in general logic config also under axis dro properties turn everything off, if it is your screen set you are useing.

if not I will do it soon

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

daniel_lyall — Tue, 25 Oct 2016 23:18:43 GMT

@Jay_Bolyard

That was quite easy to do I just block deleted the G41, 42 and 43 (@HughesTooling or @LibertyMachineis this ok to do it this way)

I have left the cancel codes in if the last person had a offset set and it did not get cancelled it can make things go wrong for you.

The work offsets in setup under post processes have the wcs offset set to 0, then when you set the wcs (what is zeroing the machine to the part after you have homed it (work Zero)) on the machine that will take care of that.

but before I post the changed post processor are you useing your own profile on the machine what only you use and no one else if you are doing it this way you don't need to change anything.

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

Jay_Bolyard — Wed, 26 Oct 2016 02:08:56 GMT

Thank you very much for helping me with a post customization.

On the Tormach machine I use there are not any unique profiles - everyone uses a single setup. The details of Mach 3 settings etc are not well understood by me at least.

Regarding subroutines - with all due respect - Fusion 360 post processing will write subroutines. For example - the Haas generic post (haas.cps) has a configuration setting "useSubroutines" - which if set to yes will result in M98 calls and M99 returns like below code. This is what I would like to do within the mach post process as well. Perhaps we need to dive into the haas.cps JAVA and see if we can bring it together with the mach3mill.cps?

Example output with subroutines written:

(Drill1)
N30 T4 M6
N35 S1400 M3
N40 G54
N55 G0 X0.5 Y-0.25
N60 G43 Z0.6 H4
N65 T5
N70 M98 P01002 (Drill1)
N105 M5
N110 G53 G0 Z0.

(2D Adaptive1)
N120 M1
N125 T5 M6
N130 S5000 M3
N135 G54
N150 G0 X0.5 Y-0.25
N155 G43 Z0.5 H5
N160 T4
N165 M98 P01003 (2D Adaptive1)

(2D Contour1)
N7230 G0 Z0.6
N7235 G1 X0.5125 Y-0.2484 F500.
N7240 M98 P01004 (2D Contour1)

N7320 M5
N7325 G53 G0 Z0.
N7330 X0.75
N7335 G53 Y0.
N7340 M30

O01002
N80 G0 Z0.2
N85 G98 G73 X0.5 Y-0.25 Z-0.3594 R0.2 Q0.025 F2.
N90 G80
N95 G0 Z0.6
N100 M99

O01003
N170 G0 Z0.113
N175 G1 Z-0.27 F3.
N180 X0.5008 F2.
N185 Y-0.2496
N190 X0.5007 Y-0.2493
N195 X0.5004 Y-0.249
N200 X0.5 Y-0.2489
N205 X0.4997 Y-0.249
N210 X0.4993 Y-0.2491
N215 X0.4991 Y-0.2494
N220 X0.4989 Y-0.2497
N225 Y-0.2501
N230 X0.499 Y-0.2505

etc. etc.

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

daniel_lyall — Wed, 26 Oct 2016 05:56:19 GMT

@Jay_Bolyard yes I know that Haas can out put it and so does fanuc, and a few others, sub programming is more for older machine what have a very small amount of memory.

Also you can not just chuck any code you fell like at it, Mach3 is based off the way fanuc does it, if you use a Haas sub program it may run or it will just stop so that is a no go for a start.

you can also use Macro B codes the fanuc style but not all and not many of the haas ones will work. Art did not added them all in nor did Brian The owners of mach3 old and new

The Haas version is there own way of doing it yes it's based of Fanuc sub programming but it has G codes in it Mach does not know. so does the fanuc one but that can be edited easier.

the best thing to do is down load a copy of Mach3 to play with. play around with some codes output by the fanuc with subprograms.cps just turn use smoothing off mach3 does not know what G5.1 is.

Now why do you wont to use sub programming (it's so 1990 )

I will be able to do the editing it does not look to hard, but it will take time.

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

daniel_lyall — Tue, 01 Nov 2016 04:31:07 GMT

@Jay_Bolyard Do you still want the post changed.

I have worked on the fanuc post and commented out the bits you wanted done, I have tested it on all the toolpaths fusion puts out it seems ok, I have run it through Mach3 as well, there is still a couple of changes need nothing that will affect you useing it now.

the attached G code is for you to test if it comes up on the machine fine it's good to go.

disclaimer use at your own risk

Re: Mach 3 Mill Posting from F - Using Subroutines and Eliminating any G41-G49 c

Jay_Bolyard — Mon, 07 Nov 2016 12:33:07 GMT

Hello,

Thank you for the assistance with the changed post. Between this file, a bit of assistance from another person also, and some head scratching on my own I'm all set.

Again - thank you for the assistance!

Jay