Fusion 360's ShopBot PostProcessor Mods

[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.
Remove jogs.jpg

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)

2020-05-07 at 1.29 PM.jpg

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.
Machine Config.jpg

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.
VSC Compare.jpg

[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).

Daren Post Dialog.jpg

[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.