Bit only "cutting air" above board!

[LindaC]

Hi

I am trying to figure out what is going wrong with job:

I have taken a vectorart3d sample file and set it up in Machinist, then imported it into VCarve Pro 6.

From there I set up some text around the image and output the toolpaths for the text as well as the toolpaths brought in with the VectorArt3d file.

Now, in Mach3, all initials setting were made (X0,Y0,Z0). Then the toolpath for the rough out was opened in Mach3. The file was run on a Romaxx CNC.

Here's the problem: no cutting happened because the bit was going right along cutting air, at about 1/8 above the board surface/Z0.

Any ideas out there?

I'm including the gcode files, in case anyone wants to take a look. Machinist and VCarvePro files are too large to upload here.

Thanks in advance for any help!
Linda

[Paul Z]

Linda,

The most likely cause is not having the Z Zero correct. In V Carve you have the option of setting the Z Zero point either on the top of your design or the bottom (actually the top of your spoil board). This has to match your method of z zeroing your machine.

If you selected a z zero at the machine surface and the z zeroed your machine at the top of your work piece,you will get an "air cut".

Paul Z

[LindaC]

Thanks Paul, but...I set my Z-0 at the top surface of my material, and it corresponds to the setting in the software...argh

[dangre]

Linda,
Your gcode contains a lot of positive Z moves (air cuts if Z was set to top of material). Somehow you have either set your VCP or Machinist with positive Z settings. This is only present in your first file. The other two are fine but they only go down a couple thousandths. We will have to see your VCP files, maybe you can zip them?

[LindaC]

Thanks Dan...I checked everything, but have looked at it so often, maybe I overlooked something! I will zip the program files as soon as I get a way to do it...then hopefully I will be able to upload

[Paul Z]

I also noticed that the first file has mostly (all?) positive z values but there might be some sort of overall Z offset. I am not familiar with this specific controller so I am just guessing.

Linda,

You might consider regenerating your toolpaths. Is it possible that you started with Z zero at the bottom, calculated the toolpaths, then switched Z zero to the top and forgot to recalculate?

[BessieHunter]

Check your Mach3 tool offsets, and make sure that it is not loading a tool offset when you load your g-code.

[LindaC]

I always use the surface of the material for my Z0.

Where do I look for the Mach3 tool offsets?

I am uploading the VCarvePro 6. The gcode files are in my first post on this. The VectorArt3d file is too large to upload, even after zipping it. I could email it to anyone who would like to look at it.

Thanks,
Linda

[Paul Z]

Linda,

I looked at your .crv file. It goes .234 inches max into the 0.5 inch material. Everything looks normal. There may be some offset for your controller (such as a bit offset) of which you are unaware?

Paul Z

[LindaC]

Well, I'll try anything!!

Where do I look for the offset in Mach3?

thanks,
Linda

[metalworkz]

Hello Linda,
I've just read this post and the other one where the cutting seems to be inverted. In mach3 you can click the tab labeled 'Offsets(Alt5)' to get the Offsets window where you can view the 'Work offsets' and the 'Tool offsets'. Click the button to the lower right hand side labeled 'Save work offsets' and the on labeled 'Save Tool offsets' and you can view the list that pops up to see if and what any offsets that have been saved are. There is also a list that will pop up if you use the Config button on the top toolbar, and select 'Fixtures' from the drop down list to show the Work offsets. If you do not see any offsets set up in the lists then I think you will need to look elsewhere to find a solution. I hope this helps some.

[Tony Mac]

Linda,

Looking at your toolpath files and I would say that the Allowance for the Roughing toolpath is forcing the cutter to initially run above the material surface. If you leave the toolpath running it should eventually cut into the material as there are negative moves in the file.

As this project is relatively shallow you could just run the Finishing toolpath without a roughing pass.

The Finishing toolpath should raster across the surface slowly dropping into the material.

Tony

[dangre]

Linda,
I will have to agree with Tony. The only issue is with your first tool path (*ctp-r) which appears to be a roughing pass. It does do a lot of positive z moves which may have something to do with allowance. I see that it was imported so I can't see how it was created. And like Tony said, the file still looks like it would work, just some wasted moves in space and because of the small cuts, just running the finish might be all you need to do.