[md63825]

I am programming my parts with V24. Everything looks fine in the CAM Tree, I am using the "Bridgeport_DX-32_VMC_Rev1" mill post from the BobCAD website like I have been since I installed the software, and it looks fine in the Predator simulator. But when I run it in the machine it goes crazy. Mainly when doing interpolations. It should be machining a small radius on a corner in the X/Z plane, instead it is performing a large sweeping arcs in the X/Y plane. I posted it to a different machine (EZTrak) with the post processor for that machine and it runs fine. Thought it may be the machine, but on other machine, no problem. Then I ran it in V21 simulation and it performs the same erratic moves that it does on the Torq-cut. I deleted the post processor and re-installed and no change. It has something to do with the post processor I think. Any thoughts? I have attached the g-code txt file created from the Bridgeport_DX-32_VMC_Rev1 post processor.

[Machineit]

I ran it and I see what you mean. I think it involves some small arc that are incorrect. Each machine may handle them differently.

Can you post the drawing file for us to see? Just zip it before sending it up.

Mike

[md63825]

Don't program to drawings typically. I program to solid models. Part was designed with Autodesk Inventor and saved it as STEP file to import into BobCAD. I have attached zip file with the step file.

Strange thing is, I got a good program from it about 2 weeks ago. Part still the same. I just changed the diameter of tool #1. Re-calculated toolpath and posted. Tool #3 is where the problem is.

[BurrMan]

It would be good to attach your post processor here too... The we can re-create and look at your issue.

[md63825]

Sorry for the delayed response.

Any guesses as to what you think it might be?

[Toolbit]

In the post processor lines 221 and 223 deal with arcs. Some machines have trouble with arcs greater than 90 degrees. If you change the n's to y's it will help crop circles. You can always change back if it doesn't help

[BurrMan]

Sorry for the delayed response.

Any guesses as to what you think it might be?

A good start would be your line 64.. It should have a z_f in it just before the arc_center entry.

This line will cause certain ramping and spiral issues with arcs...

Let us know if this fixes it.

[md63825]

Thanks for the input. I changed lines 221 and 223 to "y" and nothing changed. I even changed them separately. I also looked at line 64. Line 64 is for arc moves in the XY plane. These moves should be in the XZ plane, which is addressed on line 66. This is the first time I have looked at the Post Processor files. If you look at the updated program I attached (just added comments), sequence number 3940 (Z-LEVEL FINISH) is where the problem begins. I noticed sequence 3950 calls out G18 (XZ Plane Designation) along with G02 (Circular Interpolation CW). Two things I noticed, first, in the post processor file on line 205, "Are the xy (or yz or xz) coordinates modal in arc milling?", it was marked "n" and I changed it to "y" because G18 (or G17 and G19) should be Modal, because on line 3958, another arc move is called and there is no Plane Designation called up. Secondly, I would think that it should be G03 (CCW) instead of G02 (CW) for that arc move. Not sure how to fix the later. After changing line 205 to "y", it still had no effect. Not sure where to go from here.

[md63825]

Need to correct myself. Looked in my machine manual G18 and G19 are NOT Modal. I think this poses the root problem which is, why is BobCAD not calling another G18 on sequence 3958 for that arc move or any of the subsequent arc moves since they are in the XZ plane? I changed the post processor line 205 back to "n" but BobCAD still does not insert a G18 into the XZ plane arc moves.

[BurrMan]

I also looked at line 64. Line 64 is for arc moves in the XY plane. These moves should be in the XZ plane, which is addressed on line 66.

So did you change it???? Here's your original quote:

It should be machining a small radius on a corner in the X/Z plane, instead it is performing a large sweeping arcs in the X/Y plane.

You have to be willing to start from the obvious changes needed to whittle it down... Your response seemed to dismiss the change as not needed?

I also downloaded the STEP file, but need to have the feature setup as you to reproduce your toolpath. You could either upload the bbcd file zipped up with a feature added and the geometry selected for the toolpath (not computing will make the file smaller)

If the file is too large, you could save the feature and zip it up, with a description of the geometry selection for it...

[md63825]

Sorry to leave you hanging on the line 64 issue BurrMan. I did add the z_f to line 64 and it had no effect. I even changed line 65 and 66. I looked at several post processors and it was common to have x,y,and z data on each of those plane designation command lines.

I still think the root issue here is why BobCAD is not inserting the G18 command on each line where an arc move in the XZ plane is being made. I plan on using other post processors to see if they produce the G18 code where needed. I'll keep you posted.

bbcd file is attached.

[BurrMan]

Hey md,
I backplotted the file you posted and it looked ok (only the z-level rough, correct?) Rememeber that for that rough op, it will clean areas in a pattern, then "Return out for tiny leftover fragments"... Not sure if this is what we are talking about...

Before moving to the posted code, I looked at the toolpath and noticed it violating the set boundry, down here at the bottom...



If I offset the boundry out by .25 then it goes away.. I'm not sure if the large .75 tool in such a small confinment should work or not???

We can look at this more. The Z-level is looking at the stock removal. Maybe we can optimize it more by defining a stock.

With the output code, I just ran through it quick to get the "looks ok" statement. Maybe you can get more specific about the move that you think is out, so I can look directly at it.

[md63825]

Hey BurrMan,

I have attached 2 pics. Pic 1 shows the features in BobCAD that I am having issues with. The large cutout radius and the (4) corner radii. In BobCAD V24 it looks fine when it displays the toolpath. Pic 2 shows the geometry when extracted from the NC path when I run it from the NC window on V21. These are the same large sweeping arc paths I get at the machine when it attempts to run these features.

I talked to an applications tech at Hardinge and they indicated that the Bridgeport DX-32 controller on my machine requires a G18 in the command line where a G02 or G03 is called. Line N3950 in my code has G18G02... but line N3958 only has G02. It should also have G18 since G18 is a non-modal command. BobCAD is treating those lines as a G17, which is modal on this controller. I am trying to get BobCAD to insert G18 on these lines.

N3939;JOB 10 ZLEVEL FINISH
N3940;FEATURE Z-LEVEL FINISH
N3941G54X2.1776Y2.4844
N3942G1Z-0.003F6.88
N3943X2.1777Y2.25F11.46
N3944X0.635
N3945X0.6351Y2.7181
N3946X0.635Y2.7188
N3947X2.1775
N3948X2.1774Y2.7181
N3949X2.1776Y2.4844
N3950G18G2X2.089Z-0.053I2.2642K-0.26 (G18 present)
N3951G1X2.0891Y2.25
N3952X0.7231
N3953X0.7236Y2.2872
N3954X0.7233Y2.7188
N3955X2.0892
N3956X2.0889Y2.7032
N3957X2.089Y2.4844
N3958G2X2.0441Z-0.103I2.2918K-0.2801 (No G18 and needs it)

Submitted an Issue Report to BobCAD and they will not address the issue. Of course if I pay the Support Fee they would oblige.

Thanks for sticking with me on the issue BurrMan.

BTW, I manually added the G18 and performs the move as it should. I just can't understand why the post doesn't do this.

[md63825]

BurrMan,

Did your toolpaths look anything like the toolpath pics I have attached when you ran my program?

[dwood]

in your post see what lines 204 & 205 are

[md63825]

Both are "n" currently. I have changed them both to "y" and then 204 to "n" and 205 "y" and then 204 "y" and 205 "n". I have added "z_f" to line 64, "x_f" to line 65, "y_f" to line 66, changed line 203 to "n". Nothing seems to be working. I have even tried other post processors from other machines and get the same exact thing. I think my BobCAD software is screwed up. I have even had others run the program that BobCAD created and it has these crazy sweeping arcs that it shouldn't. And of course BobCAD won't help until I pay their service support fee. Think I will uninstall and reinstall the software and see if that works.

[dwood]

maybe burr will hit on something
i ran your file as it uploaded your tools etc in preditor, part looked ok
only i thing changed was the post to my haas
set 203,204,205 to yes and try
can you turn off g18&g19 in your control ?
i will try on a machine if i get time

[BurrMan]

I wasnt backplotting the part.. I was just paying attention to your requirement to have the G18 output on that line and why it doesnt on those line...

The 2 different lines are a feed move and an arc move.. The feed move with the G01 outputs the G18 but the arc move and the G02 dont...

I couldnt get it to output a G02 G18 as you want, and dont know enough about it to make it happen or tell you it cant.

The backplot circles are the post issue that dwood is refering too. Although, you are mentioning that it is the lack of a G18 on your arc output moves, so I think that is your answer.

The only way I can get the subsequent G18's that you want to output is to hardcode the G18 into Line 66.

But I dont know enough about it to know the longterm affects of this along with other ops, with your controller.. Seems that if your controller needs it there, then putting it there "ALWAYS" wont be a bad thing. The only other thing with that, is you then get the first line with 2. But you could also put a NUL value as the identifier for the G18 and just have the hardcode output it always....

[BurrMan]

BurrMan,

Did your toolpaths look anything like the toolpath pics I have attached when you ran my program?

And just to answer this, I can post it out with my post processor and backplot it ok.



For the backplot, it will be a combination of the post output along with the machine/reverse post used to do the backplot.

I dont know enough about this type of code to help set something up for you that works. A request to the BobCad post creation may be in order:

Post Request | BobCAD-CAM

Along with some discussion about what RP you are using.

[BurrMan]

I just ran the code from your post processor and used a different program to backplot the output.. The only odd arcs I got were on those slice planar parts with a vertical loop.... Let me look at that a little closer.