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: 

Help with Bridgeport Post

13 REPLIES 13
Reply
Message 1 of 14
skiptonsheetmetal
226 Views, 13 Replies

Help with Bridgeport Post

Hi

I'm having trouble with running a post with a drilling cycle, wondering if anyone could de-bug it for me. I've attached the post processor, the log file and the file. The machine is a Bridgeport running EZ trak dx. I've managed to post and run files to the machine, this is the first time attempting a drill cycle.

 

Thanks

13 REPLIES 13
Message 2 of 14

That's quite the old post you've got there (from 2016 by the looks of it). Would you consider going the slightly easier route and adopting the use of the new Bridgeport post processor?

 


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 14
CNC_Lee
in reply to: skiptonsheetmetal

@skiptonsheetmetal 

If the generic posts are not providing the required output, I offer post processor development services and happy to work out a solution for your machine! Message me if I can be of further assistance.

If my post answers your question, please use Accept as Solution.

CNC Lee
Fusion 360 CAM Post Processor Expert
https://linktr.ee/cnclee
Message 4 of 14

It was the first post processor that I found to be able to talk to the EZtrak system I tried the generic conversational post for EZtrak but the mill wouldn't open the files. After a bit of a search on the forums I found the post I attached above so went with it. I have just tried the new post processor that you listed above and so far that seems to work. I haven't tried running anything complex, but it did run a drilling cycle test so it is promising. I'll hopefully get more time to play tomorrow. Thanks

Message 5 of 14

I have been playing with the more up to date post and so far so good. I have found something in the nc post that is confusing me, where a new tool is called up, the immediate line following is a different tool number, I've pasted a snippet below. Can anybody explain why this line of text is in there?

 

'2D Adaptive5';
N12T5M6
N13T4
N14S2000M3
N15G90G44G17
N16M8

 

I've not noticed anything strange happen on the machine, just strange to see that line of text in the code.

 

Thanks

Message 6 of 14

That is the "next tool pre-call". Most modern machines that have a side-mount tool magazine also have the ability to stage the next tool and this allows for some time savings when running parts. If you have an umbrella style carousel, you wouldn't be able to do a pre-call. This should be an option in the post, called "preload tool". Set it to "no" and that will go away.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 7 of 14

Aha, that makes sense. We certainly don't have a tool changer on our year 2000 Bridgeport 😄

I'll look into the post file tomorrow and try tweak it. Next question while we're talking about post processors, is it possible to set a max line number at which point it automatically puts a program stop in, and then creates a new program to follow on. Basically, the post processor will get to a max line number or 9999 at which point it starts again, however the machine will only run another 2000 lines before automatically stopping, presumably a memory issue. I was hoping that I could post process 9999 lines into one program, then a second program would start, following on from where it left off. The latest program I've been trying has 40,000 lines pretty much so I am manually splitting it into 4 programs. (I've already had to post out some of the operations on a second post due to it being to big for the floppy disk file)

Long winded message I'm afraid, hopefully someone will make sense of it. Thanks 

Message 8 of 14

It makes sense, but I'm not aware of a method off hand that would do what you're looking (although I do suspect it's possible). For program size, use Smoothing on any Adaptive or 3D toolpath and that will knock down the line count a large bit.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 9 of 14

@skiptonsheetmetal You might want to look at adding a G09 at the start of adaptive toolpaths to turn off exact stop mode. Looking at my post I have it after each G0 so not sure if a rapid disables it. If not you'd need a G08 at the end of the adaptive op. You might even need the do a G08 G09 before and after each G00 in the adaptive op. I only have a 2 axis EZTrak so don't need to worry about rapid Z moves being rounded.

 

Mark

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 10 of 14

@HughesTooling thanks for the information. What does it achieve having the G08 or G09 in the code? And how would I input that into the post. Very much new to all this so it's all learning. 

Thanks

Message 11 of 14

keep in mind you can also use a 2D contour or Pocket toolpath LIKE an adaptive, but with MUCH smaller code but a pretty similar toolpath. 

Please click "Accept Solution" if what I wrote solved your issue!
Message 12 of 14


@skiptonsheetmetal wrote:

@HughesTooling thanks for the information. What does it achieve having the G08 or G09 in the code? And how would I input that into the post. Very much new to all this so it's all learning. 

Thanks


In G08 (Exact stop) mode the machine pauses at the end of each move. In G09 (Exact stop off) mode the machine doesn't pause and any sharp moves will be rounded and you lose a bit of accuracy but code runs faster. For adaptive changes in direction are smooth and you generally leave some stock so you don't notice any problems with accuracy.

 

It's a long time since I setup my post but from what I can see it looks like G00 rapid moves cancel the G09 so it needs to be output after each G00.

 

What I did in my post was create a variable to keep track of the state (G08/G09).

HughesTooling_0-1696504192847.png

Then in the onLinear function added this.

HughesTooling_1-1696504326020.png

function onLinear(_x, _y, _z, feed) {
  // at least one axis is required
  if (pendingRadiusCompensation >= 0) {
    // ensure that we end at desired position when compensation is turned off
    xOutput.reset();
    yOutput.reset();
  }
  var x = xOutput.format(_x);
  var y = yOutput.format(_y);
  var z = zOutput.format(_z);
  var f = feedOutput.format(feed);
  if (x || y || z) {
    if (pendingRadiusCompensation >= 0) {
      pendingRadiusCompensation = -1;
      var d = tool.diameterOffset;
      if (d > numberOfToolSlots) {
        warning(localize("The diameter offset exceeds the maximum value."));
      }
      writeBlock(gPlaneModal.format(17));
      switch (radiusCompensation) {
      case RADIUS_COMPENSATION_LEFT:
        writeBlock(gMotionModal.format(1), gFormat.format(41), x, y, z, f);
        break;
      case RADIUS_COMPENSATION_RIGHT:
        writeBlock(gMotionModal.format(1), gFormat.format(42), x, y, z, f);
        break;
      default:
        writeBlock(gMotionModal.format(1), gFormat.format(40), gFormat.format(08), x, y, z, f);
      }
    } else {
	  if ((GC9 == false) && ((getParameter("operation:strategy") == "adaptive" ) ||(getParameter("operation:strategy") == "adaptive2d" ))){
			GC9 = true;
			writeBlock(gFormat.format(9), gMotionModal.format(1), x, y, z, f);
	    } else {
      writeBlock(gMotionModal.format(1), x, y, z, f);
		}
    }
  } else if (f) {
    if (getNextRecord().isMotion()) { // try not to output feed without motion
      feedOutput.reset(); // force feed on next line
    } else {
      writeBlock(gMotionModal.format(1), f);
    }
  }
}

 Then modify onRapid adding GC9 = false. I think the rapid cancels the G09 in the control but you could add a gFormat.format(08) to make sure.

HughesTooling_2-1696504474435.png

So the line would be.

    writeBlock(gMotionModal.format(0), gFormat.format(08), x, y, z);

 

 

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 13 of 14

@HughesTooling , wow, mind blown 😁

I've read through that and think I've got the gist of what your code is doing, but excuse the inexperienced question, why would I need to put it in? The machine isn't stopping after an adaptive tool path command. 

I've attached a picture of what I've managed to machine, not perfect but for only the third thing I've ever machined CNC I'm quite happy. I had to split the NC  program into 9 separate programs using notepad to be able to load them onto the Bridgeport (4 on one floppy and 5 on another)

Looking into it now I can see how I could have reduced the code quite dramatically and I will certainly be trying plan future jobs to be less code intense. Would still be nice to have a post processor that will automatically break it up into separate programs over 10,000 lines.

A lot to keep learning.

Message 14 of 14


@skiptonsheetmetal wrote:

@HughesTooling , wow, mind blown 😁

I've read through that and think I've got the gist of what your code is doing, but excuse the inexperienced question, why would I need to put it in?


You should get a faster and smoother feedrate with the G09 in the code. The exact stop mode will pause after each move, might not notice too much with slower feeds but if you're using an adaptive toolpath with stay down enabled you could use quite high feeds for the no enjoyment feeds.

HughesTooling_0-1696600241141.png

 

Did you enable Smoothing to reduce code size? Normally I'd set the tolerance to 0.01 and the smoothing tolerance to 0.015 - 0.03 to get a good reduction in code size.

HughesTooling_1-1696600358865.png

 

Mark

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


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

Post to forums  

Autodesk Design & Make Report