Fusion 360 - Post Processor Error

[angusstevenson123]

Hi,

I have created a part in Fusion 360 - with machining paths. I have tried a number of different post processors.

I have an ALUMINX CNC Router and the machine uses NC Studio.

When I create the G Code - it returns an error in NC Studio.

Any help much appreciated.

Thanks - Angus

[Steinwerks]

What's the error?

[angusstevenson123]

A PDF showing the error is attached

[George-Roberts]

Could you upload some sample code that runs correctly in NC Studio? This would help identify the issue

[angusstevenson123]

Absolutely - attached is some code that runs no problems with NC studio. It created it using CAMBAM.

[George-Roberts]

Thanks for the info. Do you have a list of Gcodes the machine can use? Also, do you have a toolchanger? If so, do you have some sample code which uses it?

Cheers

[HughesTooling]

I found a couple of manuals for your control on Google but no useful info in them like what G-Codes it supports. Do you have a better manual with the machine.

Mark

[Anonymous]

I found this: https://docs.google.com/file/d/0B26SgTyDJ3GNOWdrNzMzMVRGQlE/preview

And according to that manual comments should start with a single quote so it makes sense that it would see a problem with line 3, but the posted code that works has comments in parenthesis and apparently isn't an issue...

Dave

[George-Roberts]

It's also strange it's giving a G0 error on line 3.. G0 doesn't appear until quite a bit later..

[HughesTooling]

On line 3 there's a G94, doing a search of the manual for G94 comes up blank so try removing the G94 and see if that helps.

Mark

[angusstevenson123]

Hello - sorry about the time delay - time got away.

Anyway - yes - the CNC table has 2 spindles.

Here is some code drawn up in CAMBAM (file attached) - using the generic post processor from CAMBAM - and it works fine.

I played around tonight - deleting G94 from the code - and a few other things - but still no luck going from Fusion 360 to finding a suitable post processor that my machine is happy with.

Thanks in advance.

[angusstevenson123]

Also - the machine didn't come with a manual.......and I've researched the online NC Studio manual - with no fruit to bear.

[LibertyMachine]

Well, looking at your sample programs and comparing what is and is not there in the code (compared to your Fanuc generic attempt) I see a few things that jump out at me.

Sample programs are in G21 (metric) and the Fanuc is in G20 (imperial). Does the machine support imperial? Crazy question, but I wouldn't doubt that a control exists that only supports one measurement system.

Sample code does not contain a spindle speed, simply an M3. Does your spindle not have a speed control, or is the spindle speed defined in the control on your tooling page? (assuming you have a more "conversational" tooling offset page)

Lastly, both sample programs have one more thing in common, and this might be the issue: Every line has the required G00, G1, G2, G3, even if it's redundant. I know controls exist that require that callout every line, even if the previous line called it out .

The Fanuc post does not default to redundant Gxx calls.

[HughesTooling]

I'm not sure the Fanuc post it the best place to start.

Here's your code that runs. So there's no % or program number, no line numbers and no spindle speeds.

( CUSTOM POST PROCESSOR 63A - TWIN SPINDLE )
( TEST 6/22/2016 7:52:42 PM )
G21 G90 G40
( T1 : 9.53 )
T1 M6
G00 Z20.0
( PROFILE1 )
G17
M3
G00 X18.235 Y23.1754
G00 Z6.0
G1 F500.0 Z5.0
G1 F1500.0 Y12.0 Z2.0056
G3 X23.0 Y7.235 Z0.0 I4.765 J0.0
G1 X48.0
G3 X52.765 Y12.0 I0.0 J4.765
G1 Y36.0
G3 X48.0 Y40.765 I-4.765 J0.0
G1 X23.0
G3 X18.235 Y36.0 I0.0 J-4.765
G1 Y12.0
G3 X23.0 Y7.235 I4.765 J0.0

I've modified the RS274 post to give something similar to above. There are a couple of differences that might need removing. It still outputs M8 M9 for coolant and there's a line G28 G90 Z0.0, if your machine has no limit switches and is not homed this will need to be removed.

Mark

Edit don't put this post in the generic post folder put it in the personal post folded or if you're using a PC you can click the icon next to SetUp and run from any directory.

[HughesTooling]

There is a manual here.

https://docs.google.com/file/d/0B26SgTyDJ3GNOWdrNzMzMVRGQlE/preview

Looks like I need to remove the G28 line as the control doesn't support G28 or G53 so no home\tool change position!

I make a few more changes.

Mark

Edit just figured out search was not working in the preview above, I downloaded the PDF and found it does support G28 so give the post above a try.

[angusstevenson123]

Hello - thanks very much for your help.

IT WORKS!!! - Awesome........

When I simulate it in NC Studio - it has no problems - but - gives and invalid code for M8 and M9. I manually remove these from the code and NC Studio simulates it no problem.

Would you mind re-posting the NC Studio post processor that you posted above - but so the output file doesn't include M8 and M9.

.......also - it simulates fine - but I've been watching the "current tool" in NC Studio - and it is stays on Tool 2 - the entire time.

So - I'm still fiddling to try and get NC studio to realise there are 2 tools.

For test example purposes - lets say I am machining this pocke and contourt:

I then use the NC Studio post processor.....................

.......then manually remove all M8 and M9..........it simulates fine.

But the thing that has got me bugged at the moment is:

.........I take it that means it will only use Tool 2 for the full job. In Fusion 360 the pocket is cut with Tool 1 and the profile is cut with Tool 2. Anyway - I'll keep wrestling this.

Thanks so much for your help.

Angus

[angusstevenson123]

Just ran a similar model with CAMBAM (which I know works - and physically does use different spindles when required) - with 2 different tools - and NC studio stays with "Tool 2" the entire simulation. So - I was interpreting the NC Studio incorrectly.

So - no need to worry about that.

Just the last refinement of making the post processor not output any M8 or M9 codes - is all that is required - that would be awesome. 

Thanks again - Angus

[HughesTooling · Accepted solution]

Here's an update, I added a user parameter that shows on the post dialog as outPutCoolant set to No.

Mark

[angusstevenson123]

Mark - thanks very much - I'll get back to you shortly.

[angusstevenson123 · Accepted solution]

Consider this post closed. Thanks to everyone for contributing.

Mark - thanks for the post processor file.