Issues with plasma cutting

[timothy.erickson]

I am cutting on an older plasma machine, the computer is a Burny Phantom ii. I am able to export out of Fusion 360's post processor. It loads up into the machine no problem, it also cuts very well. My only issue is when the machine comes to cut a corner my torch speed speeds up rapidly and then slows back down after its out of the corner. Does anyone have any information, or solutions to this problem?

[bob.schultz]

It is strange that it would accelerate into a corner and the decelerate out of the corner.  This is usually reversed.  I have looked at the 'burny plasma' post processor (which I am assuming you are using) and do not see anything that would cause this.  Can you provide a simple part that demonstrates this problem along with the output it generates.  It would also be helpful if you can provide output that does not have this problem, even if it is from a source other than Fusion.

Thanks.

[timothy.erickson]

I am very new to using Fusion for plasma cutting. Is there a specific Burny plasma post processor? I have been using the Generic Burny post processor. The problem only seems to present itself when it is cutting an angle that is smaller then 90 degrees. I will provide parts when I can.

[bob.schultz]

The only generic post we have for Burny is burny plasma.cps, which of course is for a plasma cutter.  Are the corners being cut correctly, or are they rounded?  It is possible that the control "smooths" sharp corners rather than performing an exact stop at the corner.  If you have output from another system that works as you expect on the machine, I would be interested in seeing that also.

[timothy.erickson]

I apologize to getting back to you so late. The 2002.cnc is one of the files done on fusion 360, this one has the speed up issues on the corners. The 204332.cnc is from a different drawing program, I have no information about the post processor. I do know however that this part does not have the speed up issue.

[timothy.erickson]

If anybody has any ideas, I'm free to suggestions. I'm very new to all of this, any help would be greatly appreciated!

[bob.schultz]

Thanks for supplying the output files for comparison.  I noticed in the Fusion output that the feed rate is slowing down on the lead-in and lead-out moves.  You can control this in the Tool tab of the 2D Profile operation.  If you want a constant speed, then all three feed rate values must match.  I also noticed that your "good" sample does not contain any feed rates.  If you do not want feed rates output, then add the following line to the top of the onOpen() function in the post processor.

   feedOutput.disable();

[timothy.erickson]

Is this the area on the post processor that you were talking about? If so it will not allow me to change the code in the post processor, I just get an error message every time.

[bob.schultz]

Yes, this is the correct area (after the function onOpen() line.  I am guessing that you are getting an error when trying to save the post.  Preferably you should store modified posts in a local folder rather back in the production location so that they do not get overwritten with an update.  You can then choose the local folder when post processing.  Please refer to the following forum discussion for more information.

https://forums.autodesk.com/t5/hsm-post-processor-forum/where-to-put-cps-files-for-fusion-360/td-p/6...

[timothy.erickson]

Bob thank you for the help, however I have a few other questions. When I disable the feed rate it did let me enter out at the controller, however it still followed the feed rate that was set in fusion 360. Our cutter also lets us input the kerf at the controller, I would like to be able to do that as well and not in fusion the same goes for torch height. I appreciate the help.

[bob.schultz · Accepted solution]

Hello Timothy,

If you made the feed rate modification previously suggested and you are still getting feed rate numbers output to the cnc file, then make sure you select the folder where you saved the modified post when post processing.

I also noticed some small differences in the output that you say works for you and the output from the burny plasma post processor.  If you would like to have the output match exactly, then you can make the following modifications to the post processor.

var gMotionModal = createModal({}, gFormat); // modal group 1

function onOpen() {
  
  feedOutput.disable();

  writeBlock("G92YX");
}

function onComment(message) {
  writeComment(message);
}

writeBlock(
    gAbsIncModal.format(90),
    gMotionModal.format(0),
    xOutput.format(initialPosition.x), yOutput.format(initialPosition.y)
  );

writeBlock(gMotionModal.format(0), x, y); // fast linear move

writeBlock(gMotionModal.format(1), x, y, f); // linear without G-word

  var start = getCurrentPosition();
  gMotionModal.reset();

  if (isFullCircle()) {

  var homeOffset = 1; // 1-4
  //writeBlock(mFormat.format(79), "T" + homeOffset); // go home
  writeBlock(gFormat.format(40));
  writeBlock(gMotionModal.format(0));

You should be able to easily find the places in the code that matches these changes.  The changes are marked in bold.  As far as entering the kerf and torch height in the control, these should still be available to you with the output from the post.

[timothy.erickson]

The output file does not have feed rates after it has gone through the post processor. If I am in fusion and set my cutting speeds to 40 in/s for example, and use the modified post processor there is no speed within the code it generates. I then bring the file out to the machine, and I enter the feed rate in the machine that I want to use is 150 in/s, the machine will still cut at 40in/s even with no code telling it to do so on the program.  

[bob.schultz]

Well ..., I do know that your machine is not getting the 40ipm from Fusion if there are no feed rate numbers in the output.  The only thing I can suggest is to implement my previous recommended changes so that the output matches your sample output, especially concerning the G0/G1 codes.  You can provide me the generated output from Fusion if you are still having these problems on the machine.

[timothy.erickson]

Bob,I made the suggested changes to the post processor and that solved almost all of my issues. I have another thing I need some help figuring out. When I take a new program into the machine I can enter my feed rate as well as kerf. When I enter the kerf in the machine, the kerf shows up red. I do not know how familiar you are with the Burny Phantom controller, but if you have any answers I'd greatly appreciate it.  

[bob.schultz]

---

@timothy.erickson wrote:

Bob,I made the suggested changes to the post processor and that solved almost all of my issues. I have another thing I need some help figuring out. When I take a new program into the machine I can enter my feed rate as well as kerf. When I enter the kerf in the machine, the kerf shows up red. I do not know how familiar you are with the Burny Phantom controller, but if you have any answers I'd greatly appreciate it.  

---

Hello Timothy,

I am not familiar with the Burny Phantom controller, so would not know why the kerf shows up red.  If you load the sample output that you previously provided and can enter kerf values without problem, then I would suggest you compare the output from Fusion with your sample output and see what the differences are.  Just a guess, but I would pay attention to the G40/G41/G42 codes.

[timothy.erickson]

The 1702 image is an example of the files already on the machine being loaded up. Everything at this point is normal. The second image (1704) is a drawing that was done in Fusion. If you notice the Kerf setting turns red. The machine will cut the part, but the kerf is wrong. I would really like to be able to give that power back to the operator instead of having it preset in Fusion when I export the file. The machine runs on Windows XP embedded. It is on the older side, but it works for what we needed to do. The final image is a comparison between a Fusion drawing and a drawing from the machine. The one on the left is Fusion, on the right is the other. Why do the Fusion codes start with N? I am not familiar with the which G codes do what, but if you have an answer to this that would be great.

[bob.schultz]

Hello Timothy,

You can set the following properties when you run the post to get rid of the M15 and the N sequence numbers.

   showSequenceNumbers: no

   useHeightSensor: no

If this does not solve your problem, then you should edit the output file from Fusion to align the G40/G41 codes as they are on your sample program, so that G41 is output just prior to the M04 line and G40 is output directly after the M03 line.  If this works as expected on the control then the post should be able to be modified to output the codes in this sequence.

[timothy.erickson]

Bob, attached is a post processor that is from our old drawing program. Is there anyway I can integrate this with fusion 360?

[bob.schultz]

---

@timothy.erickson wrote:

Bob, attached is a post processor that is from our old drawing program. Is there anyway I can integrate this with fusion 360?

---

No, you cannot take a post from another system and integrate it into Fusion.

[timothy.erickson]

I figured this was not possible. Is there any possible way I can modify the Burny post allow Kerf compensation to be in the control? I have searched around for quite some time and I cannot seem to find a post that supports my machine.