Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Syntec 6MB Post not working on CNC Router with no ATC

10 REPLIES 10
SOLVED
Reply
Message 1 of 11
FMWfablab
327 Views, 10 Replies

Syntec 6MB Post not working on CNC Router with no ATC

I have a Blue Elephant ELECNC-1530 type machine with a Syntec 6MB controller. I have unchecked the box that says I have an ATC in my machine setup because all my tools are manually changed since I don't have an ATC. However, When I generate the NC code my machine gets hung up on the T3 M6 line. It always calls out for a tool change.

 

I have been using Vectric up to this point with no issues whatsoever but have been learning Fusion 360 to try and put all operations under one umbrella.

 

I have attached three files: one is the post that works presently with vectric software and the second is what fusion 360 is giving me. The last one is the generic Syntec post in the Fusion 360 Post Library.

 

Does anyone have any suggestions as to where I may start looking? Thanks in advance!

---Ford

 

10 REPLIES 10
Message 2 of 11
engineguy
in reply to: FMWfablab

@FMWfablab 

 

Do you just want the T** without the M06 ?? If so then you can simply stop the M06 being generated by making the change in your Post Processor shown below, hope this helps 🙂

Stop M06 Generation.jpg

 

Change the line 870 to what is shown above and the T** number will be generated but no M06.

Message 3 of 11
FMWfablab
in reply to: engineguy

Well that did do what I asked but it didn't have the intended effect. It definitely removed M6 from the line but my CNC still pauses right there and goes no further. It did spit out an error of "MLC 76 (R44.11)ATC Push Out Failure Alarm".

 

I do appreciate the effort.

 

Message 4 of 11
seth.madore
in reply to: FMWfablab

Do you have g-code that you're run successfully on your machine that's come from your Vectric software? The Vectric post you shared doesn't give us a lot of easily-digested information, so actual g-code would be handy.

 

When it comes time for a tool change, I assume you'd want to see an M0 (program stop) in place?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 11
FMWfablab
in reply to: seth.madore

I do. I'll attach it here. I cut this bowl last night using this file from Vcarve.

 

And yes, the desired outcome would be an M0 after the toolpath has been completed so that I could manually change bits and then load the next toolpath .nc file if there was one.

 

Thank you for looking!

Message 6 of 11
seth.madore
in reply to: FMWfablab

In the file you shared, there are no Tool or Height offset callouts, save for a lone G49H0 at the end.

 

With Vectric, have you any programs that utilize multiple tools, or could you whip one up quickly?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 7 of 11
FMWfablab
in reply to: seth.madore

Honestly, I don't think I can. When I opt to save multiple toolpaths using different tools to one file I get an error that reads "The visible toolpaths use different tools and the selected Post-Processor does not support toolchanging."

 

Using Vcarve, if I run a job that requires 10 different tools, I have to make 10 different .nc files. Now, if I so choose, it will join all .nc files in the instances where the tool doesn't actually change though. I can make a file like that if you think it'd help.

 

Can the processes developed by Fusion be split up into multiple files like that? I'm not running a production shop. We have 1 CNC table that might run half the day. Having to load separate files for each operation isn't a hassle as far as we're concerned. I mean we have to change bits manually as it is --- pressing a few extra buttons isn't life-altering.

Message 8 of 11
seth.madore
in reply to: FMWfablab


@FMWfablab wrote:

 

Can the processes developed by Fusion be split up into multiple files like that? 


There are some posts that permit separating out the code per tool, I think GRBL does this currently.

 

Before we get to far into the post edit, could you confirm that by removing the Txx, M06 and the G43 Hxx line that everything else works as expected?
You can do this by making a very simple program, could be as basic as a line or circle.

Remove the characters in red:

N30 T1 M06
N35 S5000 M03
N40 G17 G90 G94
N45 G54
N50 G00 X3.1496 Y-0.9596
N55 G43 Z0.5906 H01
N60 M08
N65 G00 Z0.1969
N70 G01 Z-0.0394 F39.4
N75 X-3.1496
N80 G02 Y0.0374 J0.4985
N85 G01 X3.1496
N90 G00 Z0.5906
N95 M09
N100 M05
N105 G49
N110 G28 G91 Z0.
N115 G90
N120 G28 G91 X0. Y0.
N125 G90
N130 M30
%

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 9 of 11
FMWfablab
in reply to: seth.madore

Sorry it took a while to get back to you. I was actually finishing up a project and couldn't run the edited program. 

Fantastic news! It worked exactly as desired. Even so much as bringing my spindle back to home position instead of just raising it out of the workpiece. 

 

I'll attach the edited file just in case.

Message 10 of 11
seth.madore
in reply to: FMWfablab

Give this post a try, let me know how you get along!

 


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 11 of 11
FMWfablab
in reply to: seth.madore

Well that seems to have worked! I didn't actually cut anything but I set my z real high and ran a program. Everything spun up, tracked correctly and shut off as expected. Thank you so much Seth. You are a superstar!

---Ford

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report