Shopbot PRS post issue

[mcobb]

I've been preparing a couple toolpaths for milling on my Shopbot PRS Standard and it has been brought to my attention by Shopbot technical support that there are some unnecessary MS commands included in the OpenSBP post processing included with Fusion 360.  Apparently this was remedied in a previous version but now these unnecessary commands are included in the post-processing again and have been associated with freezing the machine's operation.  To be clear: Only one MS command needs to exist at the beginning of these files and all other MS commands should be eliminated.  Could we please include this in an update of the next OpenSBP Post Configuration?

[bob.schultz · Accepted solution]

Hello Mike,

For 3-axis parts, as long as you use a single feed rate for all move types you should only see one MS block in the operation.

If you have a 4 or 5-axis machine, then you can set a property to only output the programmed feed rates in the latest version of the post, so that multiple MS/VS blocks are not output.

[mcobb]

Thanks. I'm not sure I understand why a shopbot 3 axis machine is
outputting all this other MS info. Are you saying there is a setting I
should change to avoid this happening. According to tech support at
Shopbot, the answer to the question in the attached image is "yes."

[mcobb]

I'm afraid my previous reponse to your post did not have the benefit of seeing your graphics.  I was looking at it on a phone.  I see what you are saying!  Thank you! 

The plunge rate will probably want to be different.  What happens then?  Can I simply change this one parameter and still expect a single MS line.  I guess the second number in the MS command is the plunge rate so hopefully there will not be the need for additional MS commands even with this second value.  Any thoughts on this are appreciated and would spare me further experimentation.  Thanks again for the advice.

[mcobb]

So I tried entering the numbers as you described and still seem to be getting a bit of a problem.  I believe Shopbot would like to have the output read as indicated on the far right in the attached image.  Do you agree?

[bob.schultz]

Outputting a single MS command when cutting only in the XY-plane and the Z-axis is only used for plunging and retracting, then your example output would be fine.  In your sample output I see that the XYZ-axes all move at the same time, so what will happen here when the XY and Z feed rates are different?

I believe that the output from Fusion should work as desired on the machine, as it follows the feed rates that you define in the operation and allows for different feeds for lead-ins/lead-outs, cutting, plunging, etc.

Have you tried this output on the machine?  If it does cause issues, we can always add a property that outputs only the cutting and plunging feed rates, as it is not difficult to do, but I don't think that this is the proper solution.  Please try it on the machine and let me know what you find.

Thanks

[mcobb]

So I've been in a little bit of quandary.  Shopbot's tech support instructions have been quite clear.  Without entirely understanding the subtleties of their firmware, they have said they handle any other values (other than the prevailing feed and speed) internally in their device. No doubt Autodesk, in its coordination with many different vendors, is seeing things they are not.  Nevertheless, their advice for their machine appears to be sound in recommending I eliminate all but the first MS command.

No doubt this is because many of the people using their machines are beginners and this is all the bandwidth we can handle. Having said that, I think it might make sense for Autodesk to be a little more clear that many of the values you are requesting of the user are simply irrelevant if they are using a shopbot. It would not surprise me if this user experience was turning off a lot of people from using Fusion 360 instead of VCarve. 

I'm a little embarrassed to say how many hours I spent dialing in the various rates...only to discover the toolpath did just fine when I opened up notepad++ and eliminated ALL the MS commands except the first one.  Also, in previous toolpaths I have generated in Fusion I have seen the machine choke on the cut file.  While I will never ultimately know the reason for those file's failures at this point, it does seem plausible that, as the Shopbot tech support mentioned, there are many extraneous commands that conspire to make the flow of data less efficient.  On on toolpath that had 600K lines, I found I could eliminate 13K MS commands from the post and it executed just fine. I also know that adjusting smoothing and tolerances has also helped. 

Here is a link to the five toolpaths I just ran. I replaced all the various subsidiary feedrates with the main feedrate and this greatly improved the output files.  Nevertheless, I went into all of these and eliminated MS commands in 3 out of 5 of them .  One toolpath (a steep and shallow one) still had 3329 MS commands.  Having eliminated all the commands but the first one in all the files, these files ran fine.  It is also worth noting this constituted about 24 hours of milling and the odds of it choking previously would have been high.

I hope this helps the Shopbot user experience with Fusion 360.  Shopbot is a great gateway for many people trying to enter the world of CNC milling and your support of their hardware is greatly appreciated.

Regards,

Mike

[bob.schultz]

Thanks Mike for the detailed explanation on how the feed rate output affects the actual machining of the part.  You did more than your fair share of diligence in testing the output and reporting the results that you found.  Here are changes you can make to the shopbot post to only output the feed rate at the start of an operation.  It uses the cutting feed rate for XY moves and the Plunge feed rate for the Z moves.  Please let me know if this works as expected on the machine and we will put an option into the post to use this style of feed rate output.

At the end of onSection please add the following logic.

  if (currentSection.isMultiAxis()) {
    xOutput.offset = 0;
    yOutput.offset = 0;
    zOutput.offset = 0;
  }

  // ADD THE FOLLOWING CODE
  if (hasParameter("operation:tool_feedCutting") && hasParameter("operation:tool_feedPlunge")) {
    var f = feedOutput.format(getParameter("operation:tool_feedCutting"));
    var z = feedZOutput.format(Math.min(getParameter("operation:tool_feedPlunge"), maxZFeed));
    if (f || z) {
      writeBlock("MS", f, z);
    }
  }
}

And in the writeFeed function just return upon entry.

function writeFeed(feed, moveInZ, multiAxis) {
  return; // ADD THIS LINE