Plasma Cutter Kerf Width Has No Effect

[ben.griggs]

Ive noticed that adjusting the kerf width on a plasma cutter tool has no effect on the cut. All of my cuts appear to be a couple of millimeters too tight which is really frustrating!

I've adjusted the kerf width all the way up to 20mm to see if that has any effect, it only seems to adjust the lead in and lead out length. In Simulation mode, everything looks as I would expect, which leads me to belive there is something wrong with my post processor? I'm using the mach3 plasma processor downloaded from the autodesk website. 

Many Thanks,

Ben 

[julia.paganucci]

hi @ben.griggs , 

thanks for posting! I just tried recreating this on my end with the Mach 3 plasma post, and there were differences in the code with the different kerf widths when posting... Can you please attach your file here and I can take a look? 

Thanks,

[ben.griggs]

Hi Julia, 

Sorry for the delay in my reply. I have been playing around with it today and it appears that the G Code exported runs the toolpath directly on top of the perimiter regardless of what the simulation is showin. I have uploaded a screen shot where I have over exagerated the kerf to 50mm to make the issue clearer. 

I have also attached a photograph of the cut path in Mach3 - As you can see the lead in and lead out are compensating for the larger kerf.

Below is the G Code that is outputted from this setup:

N10 G90
N15 G71

(2D Profile1)
N20 G0 X33.827 Y-75.
N25 M3
N30 G4 P1.
N35 G1 G41 X55.478 Y-62.5 F1000.
N40 G1 X26.61 Y-12.5
N45 G1 X20.36 Y-1.675
N50 G1 X17.459 Y0.
N55 G1 X4.959
N60 G1 X0.
N65 G1 Y50.
N70 G1 X50.
N75 G1 Y0.
N80 G1 X4.959
N85 G1 X-7.541
N90 G1 X-10.441 Y-1.675
N95 G1 X-16.691 Y-12.5
N100 G1 X-19.191 Y-16.83
N105 G1 G40 X2.459 Y-29.33
N110 M5

N115 M30

[boopathi.sivakumar]

@ben.griggs 

Are you sure you are using the latest post ?

mach3_plasma 

Try with the above one and if it is not working then

Please attach the model file because we could not able to replicate your issue

File>Export>.F3d
save the file and reattach the file to this thread.

[ben.griggs]

Hi, please find attached a test .f3d file I have been using to show the problem. 

Thanks,

Ben.

[boopathi.sivakumar · Accepted solution]

@ben.griggs 

When the compensation type is set to In control then the toolpath does not calculate the kerf with from the tool kerf in fusion istead it posts G41 in the code where you can give the offset value in the machine.

So if you want to calculate the toolpath including the tool kerf in fusion then you need to set it to In computer the you can see the difference in the codes with respect to the tool kerf dia

You can see its already defined the description also

[JESwardstrom]

I am having similar issues as the original poster.  My issue is with a post for a ShopSabre Plasma table that uses a WinCNC post and Fusion 360 Manufacture tool paths.  In my situation, it doesn't accept cutting paths in tight areas and no matter what I do it won't generate a path.  I have checked to see if the path should fit and from basic measurements and a little math is should work.  I'm also finding that when I remove the lead in - lead out from my tool path Fusion 360 seems to put it in anyway.

Things I've tried:

1. altering the geometery by exploding the text and changing the geometry of the text to give what I though would be enough space to build a toolpath.

2. Removing the lead in... mentioned above.

3. changing cutter compensation in the tool description to .oo5 in.

I have also exported the text  from Fusion 360 and imported into Enroute, which I used to apply .100 in kerf and generate G code with cutter compensation.  So, I'm guessing the geometry is correct and that there's something messed up with how Fusion 360 manufacture generates tool paths for plasma cutters.

Thanks for viewing...

[engineguy]

@JESwardstrom 

Can you please upolad a file that you are having problems with as it may be an issue with the Model/Sketch being used.

What you may be seeing after removing the Lead In/Out could be the "Pierce Clearance", this value is added to the Lead In/Out so there is still a move in to the cut.

To upload a file go to :-

File > Export > Select f3d Format > Save to a location on your computer > Then attach to your reply

[JESwardstrom]

@engineguy thanks for offering to help.  I've added the file; however, I am currently at work and won't be able to try any solutions until I get home.  That said one thing I thought of was maybe just leaving things just sketched text and avoiding extruding.  My thoughts were that may simplify things when I go to select what I'm cutting.  I'm pretty new at this.  

[engineguy]

@JESwardstrom 

That`s OK, I looked at your file and it does appear to be the "Pierce Clearance" value that is too high, without changing any of your other settings I found that with your Lead In/Out of 0.045in that a "Pierce Clearance of 0.08in or less will allow all the toolpaths to generate correctly. So, you can adjust both the Lead In/Out and Pierce Clearance values to suit what you need to do, they are added together. Updated file attached for you as an example.

[JESwardstrom]

@engineguy 

Oh my word!  I fought with that for probably 2 hours.  And the crazy thing is I never messed with pierce height... I need to check, but I'm not sure the controller of my machine is using that anyway.  That's something I'll have to figure out when I get home.

Thanks for looking at that.