First Sign Carve - "V" Bit - Problems

[blackte]

I attempted to make my first Sign. 3D model looked good, but when I attempted to run the GCode on my CNC, the "V" bit went through my sign material 3/4" and into my spoil board about a 1/2" before I could hit the emergency shut-off. I have looked at everything and I'm unable to see what might have caused this. The GCode file is attached. "CRV" is https://www.dropbox.com/s/ed4e1cutzyfmwmt/Logo.zip?dl=0. Unfortunately I now have to re-Tram my spindle because of it.


Any help with this would be greatly appreciated.

[James-C]

Have you set the Z zero position to the material surface or machine bed?
Have you remembered to set the zero the tool length before making the cut?

I have made both mistakes with similar results.

[blackte]

Yes, Z - Top of Material, Measured Tool before proceeding. Checked Z depth in GCode looks correct.

[ger21]

Looks like an issue with your machine control, as the code appears to only cut 1/4" deep.

[blackte]

ger21 - I'm thinking the same thing, but wanted to see what others thought.

[Leo]

Yes, Z - Top of Material, Measured Tool before proceeding. Checked Z depth in GCode looks correct.

When you say "measured tool before proceeding" ---- what do you mean?

When I think of setting tool to top of material I will move the tool tip to the top of the material and zero out the control for that tool.

How did you set zero on top of material?

[blackte]

Leo - my machine is set-up with a spoil board bolted down to my phenolic table. My cutting material then sit's on top of the spoil board. All tools are measured for their length once loaded into the spindle. I have an automated process that measures each tool that is in the carrier. I have a 8 tool holder carousel that carries all of my tools I need for each job that I'm running. All of my runs within V-Carve I set the "Z" to top of Material. I have run several things before without any issues except circles, which I just changed them to Beziers and they worked perfectly. I have not run anything using a "V" bit. Which in my opinion should really not make much difference. But unfortunately it did. I think there is an issue with my PP, but I have not had the time to look into that yet.

[ger21]

I don't think anything in the post will affect your V Carve issues.

Was the circle issue that there were a bunch of large circles? It appears the post you used used absolute IJ mode. Most machines use Incremental IJ mode.

[TReischl]

No, there is not an issue with your post processor. The only Z depth below zero is Z-.25. So if you zero is set to the top of the material the tool will not go below Z-.25.

You may be measuring all the tools for your auto tool changer but that does NOT set a zero reference for the material. Think about, you can say is tool is 2 inches long. So what? If you put a 3 inch thick piece of material on the machine how does it know that? It doesn't. So you need to set a zero to the top of your material. You need to read up a bit on your control and how it works with an ATC.

[blackte]

ger21 - One circle to cut-out a shape. When using circle's it would not cut properly. It would start fine, and then go off course. So I switched it over to Beziers and worked perfectly(Adrian suggested this change). From talking with my machine manufacturer it has to do with the controller. I miss stated, and should have said controller.

TReischl - My machine always has knows at what depth the top of Spoil Board is in the machine control. So when I swap tools and measure them, it will still know where top of spoil board is at all time. If my job specs are 3/4" or 4" thick, it should still know where the top of the spoil board is no matter what. All materials are different, but that should not effect top of spoil board. I normally work with sheet goods for cabinets all are around .748 - .760, that is my main business. I have been playing with V-Carve for a while and like the ability to create new things. I'm not blaming the software or the GCode. I think the issue is in the machine control that it's getting messed up. I just need to work through that side with my machines manufacturer and go from there.

[TReischl]

Black, now we are getting somewhere.

Your machine "knows" where the top of the spoilboard is in reference to machine Z zero.

When do you tell it how thick the material is? Or where do you that?

From what you have now said it sounds like it is definitely something to do with what you are telling the machine, or failing to tell the machine, a procedural error if you will.

If you are not telling the control about material thickness then it has to be done in Vcarve. Make darn sure you have the zero set to the bottom of the material (spoilboard) and check that you have set the material thickness correctly.

[Leo]

opps - didn't mean to post


Hmmmmm - I agree with Ted.

Sounds like the machine did everything it was told to do.

Go to Z Zero and start machining.

Sounds like Z zero is the machine bed NOT top of material.

So - what you described in your initial post makes sense based on this.

[ger21]

Yep, sounds like Z zero is your spoilboard, and you need to tell V Carve Pro that it's the bottom of the material.

[blackte]

Here are my settings for this CRV file. To me this is correct. It has the material as 3/4" thick and "Z" is top of material.

[ger21]

Try checking "Machine Bed" under Z Zero. From what your saying, that's what we think it should be.