Fusion 360's ShopBot PostProcessor Mods

[sbd1]

I've been using F360 for occasional, complex 3D milling for a few years now with a hobbled together PostP I made from F360's default PP for SB, but it still has problems that force me to edit every cut file manually before running. I've recently starting inquiring how to fix these & came across this app & wondered if anyone here knows how to use it.

Visual Studio Code

This page on NYCCNC (https://www.nyccnc.com/vs-code-editing-posts/) has a video where John explains how to use Visual Studio Code to modify his PostP files. I love the way it shows live editing of the PostP next to the linked cut file. It's like MAGIC!

But I've tried for hours to get it to work with SBP files (as opposed to NC files) & I couldn't figure it out. I'd be willing to pay someone to assist me in setting this up if it's possible for SBP files.
Daren

[robtown]

I've been using F360 for occasional, complex 3D milling for a few years now with a hobbled together PostP I made from F360's default PP for SB, but it still has problems that force me to edit every cut file manually before running. I've recently starting inquiring how to fix these & came across this app & wondered if anyone here knows how to use it.

Visual Studio Code

This page on NYCCNC (https://www.nyccnc.com/vs-code-editing-posts/) has a video where John explains how to use Visual Studio Code to modify his PostP files. I love the way it shows live editing of the PostP next to the linked cut file. It's like MAGIC!

But I've tried for hours to get it to work with SBP files (as opposed to NC files) & I couldn't figure it out. I'd be willing to pay someone to assist me in setting this up if it's possible for SBP files.
Daren
It's just a text editor that allows code highlighting via extensions.
It can edit .sbp files just fine, but if you want it to recognize the .sbp extension and highlight and give cose hints, then you'll need to have VS code extension for that.

[EricSchimel]

What are you trying to accomplish with the edits?

[sbd1]

What are you trying to accomplish with the edits?

I need to fix a few things. I've listed them in detail here (https://forums.autodesk.com/t5/hsm-post-processor-forum/looking-to-hire-someone-to-mod-a-shopbot-post-processor/td-p/9484003) on the Fusion 360 forum.

[sbd1]

@Robtown. I really want to be able to see changes I make to the PostP change the cut file in real-time like in the NYCCNC video. Are you saying that the VS code extension will allow me to do that with .sbp files?

[robtown]

@Robtown. I really want to be able to see changes I make to the PostP change the cut file in real-time like in the NYCCNC video. Are you saying that the VS code extension will allow me to do that with .sbp files?

No, I didn't watch the video.
I seriously doubt there's a VS code extension for shopbot cutting code.

[EricSchimel]

I need to fix a few things. I've listed them in detail here on the Fusion 360 forum.

If you lay out some specifics I, and others may be able to help

[sbd1]

Specifically, I want to use VSC so that it has a real-time-link (probably not the correct term) between my PostP and a .sbp cut file as shown in the NYCCNC video.

[EricSchimel]

Specifically, I want to use VSC so that it has a real-time-link (probably not the correct term) between my PostP and a .sbp cut file as shown in the NYCCNC video.

I should have been more specific.. I've seen the video and I understand how to edit the code, but what things do want to change about the post processor?

I've done a fair bit of tweaking and I may be able to offer some suggestions, I just need to know what you're trying to change :)

[sbd1]

Thanks for your offer Eric, it's very likely you are more experienced than I am at editing Posts. Over the years I've done some basic Post editing for various CAM apps (with help from some awesome guys on this forum), but if you know Fusion you know nothing is simple there. More than actually fixing the few issues I listed on the Fusion forum, I really wanted to let everyone here know about VSC & also see if anyone was experienced in using it. For me it's been a HUGE improvement in reviewing & editing posts. I've already fixed the issues I had, and I've finally figured out how to get the real-time-link working between my Post and a .sbp cut file. Along the way I stumbled on something possibly even more helpful: The ability to compare two posts side-by-side with highlighted differences. If you're experienced in coding I'm sure I'm not telling you anything new, but if you're a DIY person this is a great tool to have in your toolbox.

Having said all that, I'd still be interested in hearing any tips from experienced VSC users in here.
Cheers,
Daren

[EricSchimel]

I got the part about the real time link and that's really cool for advanced edits to posts, but let be re-ask my original question:

What changes are you trying to make to the stock SBP post processor in Fusion? Specifically what was it not doing that you wanted it to do? That's what I'm after.

[sbd1]

What changes are you trying to make to the stock SBP post processor in Fusion? Specifically what was it not doing that you wanted it to do? That's what I'm after.

Problems I've now fixed:
1) Remove unwanted JH & J5 jogs at start & end of file. I was manually deleting these from every cut file, but I think a newer release of the post from Fusion may have already fixed the JH.
33808

2) X & Y feeds (possibly Z also) limited to 3 IPS. For some reason my cut files are limited to 3 IPS (180 IPM) regardless of what feeds are set to in F360. ie: This TP's feed is set to 270 IPM (4.5 IPS) in F360, but the cut file is only 3 IPS.


Wish list: Second Z axis router
1) My 3 axis CNC has two Z axis routers, which I often use with other CAM apps (ie: head 1 [Z] for routing, head 2 [A] for drilling). The post for those apps use to the X Y offsets in my machine's config file (CN90). Wondering if it's possible to add this functionality to a F360 post & then somehow define those setups in CAM?

[EricSchimel]

I think you can solve all of this by simply using the properties setting when you post out a file in Fusion:

With these settings you get proper move/cut speeds, and you don't get the tool returning to home after a cut. Jog speeds are set on your ShopBot control. (look under rotary move speeds)

33809

As far as the dual Z's, I have the same thing too. For that you just number the tools in Fusion. Tool 1 should be the first Z and tool 31 should be the second Z, unless you have it setup differently in your machine. The offsets are pulled from the SB control, not Fusion (or any other CAM)

While editing the post processor in that way is super cool, I don't think you need to do it.

[sbd1]

I think you can solve all of this by simply using the properties setting when you post out a file in Fusion:
With these settings you get proper move/cut speeds, and you don't get the tool returning to home after a cut. Jog speeds are set on your ShopBot control. (look under rotary move speeds)

Your attachment is too small & blurry to see, but I know what you're trying to show.
PS: I just tried attaching a PNG file & it was converted into a blurry, small unreadable JPG like yours. When I uploaded the same image as a JPG it's nice & clear, so it must be happening during the forum's file conversion process.

I make sure to set all feeds correctly in every F360 toolpath. The max feed rate was actually a coded line in the F360 post, it's not controlled by the property selections: I fixed that.

As for speeds being limited by the SB control settings....
Move Speed: Nope, I've confirmed the SB uses the move speeds defined in the cut file.
Jog speeds: Since JS isn't specifically set in the cut file, you could be right. But aside from the JZ at the start & end of the cut file, I'm not sure how or if F360 even uses it. I need to learn more about rapid & max feedrates. I see them in F360's machine config & as settings in toolpaths, but I'm not sure if/how that info gets used by the post.
33827


As far as the dual Z's, I have the same thing too. For that you just number the tools in Fusion. Tool 1 should be the first Z and tool 31 should be the second Z, unless you have it setup differently in your machine. The offsets are pulled from the SB control, not Fusion (or any other CAM)

I know the eCabinets SB Link uses tool numbers to define which head is running, but don't think that applies to F360 posts. I create cut files from Aspire for both heads without anything to do with tool numbers. I do know about the offsets for head 2 in 'my_variables' config file though. Haven't really had a need to dig into this yet.


While editing the post processor in that way is super cool, I don't think you need to do it.

No, I suppose you're right, it'll edit code just like the SB Editor or even Notepad. But even as a non-coder, newbie VSC user, I can tell you that it's awesome for doing a direct comparison between two posts (image below). This becomes super handy when trying to identify what they've changed in newer releases of their post & if I should integrate them into mine.
33828

[EricSchimel]

As for speeds being limited by the SB control settings....
Move Speed: Nope, I've confirmed the SB uses the move speeds defined in the cut file.
Jog speeds: Since JS isn't specifically set in the cut file, you could be right. But aside from the JZ at the start & end of the cut file, I'm not sure how or if F360 even uses it. I need to learn more about rapid & max feedrates. I see them in F360's machine config & as settings in toolpaths, but I'm not sure if/how that info gets used by the post.

Check this settings panel:

https://photos.app.goo.gl/q5KKreMyUEEyw2iW8

There you can decide if you want the speed to be set using the VS or the MS command. If you choose VS I believe the settings are permanent until they are changed again. The MS can be called line by line if you want. I'd go with MS because it will respect the speed you have set per tool in Fusion (fusion will convert IPM to IPS)

Regarding rapid feedrate thing, look at the "high feedrate mapping" I suspect that one setting will respect what you have set as default in SB, and another will respect what you have set in the per job/tool setup.


I know the eCabinets SB Link uses tool numbers to define which head is running, but don't think that applies to F360 posts. I create cut files from Aspire for both heads without anything to do with tool numbers. I do know about the offsets for head 2 in 'my_variables' config file though. Haven't really had a need to dig into this yet.

If you're creating cut files in Aspire and don't do anything with tool numbers are you sending a multiple head/tool job to your machine as one file? If so, you have to be dealing with tool numbers. When you send a file in that way the ShopBot file has a command that goes something like &tool XX (that's not the exact command but it's something like that) when a job is running along and it sees a tool number, it will change the offset that is set in your SB software.

You say you're not doing that, so you must be saving toolpaths for head 1 and head 2 separately? If that's the case you must be manually doing the offsets, if I'm right about all of that Fusion's tool numbering won't work for you. You definitely want to get the tool numbering thing setup. There's a wizard in SB3 for it. When you do get it setup right when you send a job from Apsire/Vcarvve/Fusion it'll grab the tool numbers as the file runs along and engage whatever offset you need on the fly.

[sbd1]

Check this settings panel:
There you can decide if you want the speed to be set using the VS or the MS command. If you choose VS I believe the settings are permanent until they are changed again. The MS can be called line by line if you want. I'd go with MS because it will respect the speed you have set per tool in Fusion (fusion will convert IPM to IPS)

Where in the world did you find that dialog box in F360?


Regarding rapid feedrate thing, look at the "high feedrate mapping" I suspect that one setting will respect what you have set as default in SB, and another will respect what you have set in the per job/tool setup.

Yeah, high feedrate mapping is on my list of things to look into. Haven't been able to get my head wrapped around that yet. Do you know anything specific about it?


If you're creating cut files in Aspire and don't do anything with tool numbers are you sending a multiple head/tool job to your machine as one file? If so, you have to be dealing with tool numbers. When you send a file in that way the ShopBot file has a command that goes something like &tool XX (that's not the exact command but it's something like that) when a job is running along and it sees a tool number, it will change the offset that is set in your SB software.

You say you're not doing that, so you must be saving toolpaths for head 1 and head 2 separately? If that's the case you must be manually doing the offsets, if I'm right about all of that Fusion's tool numbering won't work for you. You definitely want to get the tool numbering thing setup. There's a wizard in SB3 for it. When you do get it setup right when you send a job from Apsire/Vcarvve/Fusion it'll grab the tool numbers as the file runs along and engage whatever offset you need on the fly.

Correct, I use two separate posts in Aspire for the two heads, as opposed to eCabs which uses them consecutively. I didn't know I could do that with ASP or F360. The second Z head offsets are in the 'my.variables' file. It sounds like you're more competent in these issues than I. How do you use two Z heads in your various apps?

Thanks for sharing your knowledge on this voodoo.

[EricSchimel]

Where in the world did you find that dialog box in F360?

It's in the settings panel that pops up when you post a job out of Fusion. You just click the little triangle to expand it to see the settings, just like all of the other toolpath menus.


Correct, I use two separate posts in Aspire for the two heads, as opposed to eCabs which uses them consecutively. I didn't know I could do that with ASP or F360. The second Z head offsets are in the 'my.variables' file. It sounds like you're more competent in these issues than I. How do you use two Z heads in your various apps?

Thanks for sharing your knowledge on this voodoo.

Don't do it that way in Aspire, use the tool numbers. If you already have the offsets setup in your my variables in SB3 all you need to do is call the correct tool number on the stock SB post out of Aspire (make sure you're using a tool changer post, they're in Aspire). If you do it this way you can send a two headed toolpath as one file to your machine and it will drop whatever head is called for on the fly.

Same goes for any other CAM, as soon as it sees that tool number it'll drop the head and engage the offset. Big proviso is that you have everything setup in SB3 correctly. If it's working with eCabinets you likely do have it setup right.

[sbd1]

It's in the settings panel that pops up when you post a job out of Fusion. You just click the little triangle to expand it to see the settings, just like all of the other toolpath menus.

That's not what I see on my Windows 7 PC. Are you on a Mac? Looks like the same info just in a different format (I like yours better).

33831

[EricSchimel]

Yes I was on a Mac. I always post jobs on a PC though.

Fool with the settings there.. in particular that first setting. You're likely on SB3.6 or later, not an earlier version like you currently have set

[sbd1]

You're right, I am running SB3.6 but I leave that set to No because that's the fork in the road I chose a few years ago when I first started using F360 & that post produced the most 'workable' cut file at the time, when there was virtually nobody available to get advice from about SB posts, and I knew virtually nothing about F360 but I had a job waiting to be machined. I also recall making significant changes to my SB files when I setup the SB Link several years before that & I'm very weary of breaking something that works.

What you've told me in this thread though makes me think I need to review & likely re-do my all my Posts someday to get more value from them & my SB. But it still feels a little like voodoo to me.

[sbd1]

And judging by the lack of contributors on this thread, there aren't many SB owners using Fusion & tweaking their own post processors. Thanks for your contributions Eric.

[EricSchimel]

No, I think you've interpreted what I'm saying wrong... There aren't too many cases where someone needs to edit a post for Fusion, or Aspire/VCarve. What I'm trying to steer you towards is just setting up your CAM right. Those toggles in the post screen on Fusion are there for a reason, to make common things that you need to change readily available without the need for coding. From what I can gather everything you need can easily be changed by just a couple of toggles, and understanding the tool numbering system that's already in SB3 (and that you're already using and have setup)

You're just a few toggles away from having a really slick setup, do it! You'll appreciate it every time you post a job from any CAM software! :)

I suspect the lack of contribution is there is really almost no need to edit a post.

[EricSchimel]

PS, just re-reading this and I hope my tone came across as encouraging. You're really close and I think you might be thinking that the things you want to do are harder than they actually are.

Just break the problem down into a few steps and you'll figure it out.

You can learn a lot by posting something of out any CAM software and either looking at the ShopBot Command Reference, or just punching commands into SB3 to see what they do.

[Marc F. Lupien]

Excuse me but there are users of Fusion. ;-P Don't be so fast to «judge»... Maybe the way you use your machine is «special» and others did not encounter the same problems...

Also, Eric is giving you very competent and helpfull information here. I don't see what others could add that would help that much.

signed: «a Fusion 360 user».

[sbd1]

You're both right, maybe my setup or use is not normal or even correct. I've been known to take the long way around a problem to figure it out before. And yes, I appreciate all the patience Eric has shown & the info & insight he has added here. I'll figure it out eventually.

I would be interested in hearing how many SB owners use Fusion, how they've configured their posts to suit their needs.

[Marc F. Lupien]

Personally, I use the post processors as is (both for Vectric VCarve and Fusion).

However, I did change some shopbot files (MTC.sbp and MTCon.sbp) to get rid of some restrictions regarding tool numbers. After a fair bit of reverse engineering on the shopbot files (due to lack of documentation), I found out that tool number is used to drive some CNC operation. Since the CNC can have different tools hooked up to it, Shopbot used a clever hack to start and stop different tools when executing a tool path by assigning tool number to specific tools. For example, tools 1 to 19 are used for the main spindle/router on the Z axis. Other numbers are for drills, etc.

The problem I had was that I wanted to assign different tool numbers for my tools but the shopbot software restricted me to numbers 1 to 19. So the mentionned files were changed to allow me to use tool numbers 100-599 for my CNC router on the Z axis - same as the 1-19 tool numbers. That made more sense when organizing my tool database.

Also, I did create a new post processor for Vectric VCarve to handle my small engraving laser.

[sbd1]

Good to know Marc, thanks. So that means out of 4 people in this thread so far, 3 of us have edited our SB file(s) or CAM software post(s) to suit our needs.

[EricSchimel]

Marc, do you have a big toolchanger on your machine? I'm curious as to why you'd do that... If not an ATC do you have collars on your tools or something like that that would necessitate all of those tool numbers?

SBD, in my experience most people most of the time don't have to edit posts, or other SB files unless they're fairly off the beaten path in terms of what they want to do.