Tails on Engraving Toolpath

[AndyBerry]

I recently was making a sign (pine to be painted) for a friend. We used block letters and received some odd results. We used a 45 degree V-Bit 1 inch wide. I have done this before, with success.

This is the result.

Here are the measurements from V-Carve pro.

Showing the result with measuring tape.

Finally the V-Carve Pro cutting parameters for engraving toolpath.

So, originally I thought it was a z-axis zero error. Nope. Validated numerous times.
Then I thought maybe it was not setting the cut depth deep enough (see cutting parameters above) - nope.
Finally I thought maybe the tool database was jacked up. So I downloaded directly from the manufacturer. Redid on scrap wood with same result.

Any suggestions or what I might be missing? Like I said we had done this before with expected results. This is new??? Maybe in this version?

Andy Berry

[adze_cnc]

For the "Finally the V-Carve Pro cutting parameters for engraving toolpath” image click on “Edit” and take a screenshot of the tool’s parameters.

I have a sneaking suspicion that there is a disconnect between the included angle of the bit specified in the program and the actual angle of inclusion for the v-bit.

[FixitMike]

If a the actual V-bit angle is less than what was specified for the tool, this is the result you will get. I suspect that the bit actually used has a 60 degree included angle rather than the 90 degree angle displayed in the cutting parameters posted, based on the dimensions shown.

[FixitMike]

Which bit did you use? The 45 degrees specified in your posted description, or the 90 degree specified in the toolpath picture?
I think I see the problem.

[AboveCreations]

You are using a 45 degree V bit (as you stated), but your settings are showing a 90 degree V bit. Which V bit are you using (make and model # if possible). I would think that vcarve is thinking you have a 90 degree for the cut, but you are cutting with a 45 degree which is not actually cutting the whole amount that vcarve computed with the 90 degree.

[martin54]

If you could post the CRV file it would be helpful, it's not a problem with the software or the version you are using, I can say that because if it were then the forum would be full of posts by people having the same problem

As others have said this is most likely because the V bit you are using is not the correct angle, if your actual vcarve file used a 45 deg bit rather than the 90 deg bit shown in your screenshot then I would test the v bit to make sure it is actually the angle it claims to be, there is a sticky post about checking vbit angles & how you can test them

The other thing I would mention is not to go by the manufacturer's settings for all your cutting bits, you need to test cutting bits & make adjustments to make sure the settings are right for your machine, the manufacturer's recommended settings may not be right for your machine & set up for a number of different reasons.

[wilkigr]

I don't have a solution, so I hope that you will all bear with me with a question. The bit is 1" wide, and the flat depth is set to 1". Will the width of the letter prevent it from carving down to 1"? I guess that I'm saying that I don't quite understand why the flat depth is set that deep.
It's hard to tell by the way the tape measure is placed, but it looks like the letter is about the width that is shown, except for the ends. That may mean absolutely nothing, though.

[Tex_Lawrence]

… Will the width of the letter prevent it from carving down to 1"? …

You are correct, Grant. The flat depth being set is a superfluous setting, because the bit will never cut that deep in this project.

[martin54]

I don't have a solution, so I hope that you will all bear with me with a question. The bit is 1" wide, and the flat depth is set to 1". Will the width of the letter prevent it from carving down to 1"? I guess that I'm saying that I don't quite understand why the flat depth is set that deep.
It's hard to tell by the way the tape measure is placed, but it looks like the letter is about the width that is shown, except for the ends. That may mean absolutely nothing, though.

It is the very bottom (& top) that the OP is asking about, if you look at the screenshot of the letter P then you will see that the bottom is square & so is the top left corner but the picture of the carving shows a triangular shape on each of the corners that should be square. You are correct in that setting a flat depth that is deeper than the bit will carve between the vectors will have absolutely no effect but it shouldn't cause the sort of problem that the OP is seeing. That is normally due to incorrect setting of z zero or the angle of the v bit used not matching the selected bit in the software. The OP says that the z zero setting has been checked & is correct which really only leaves the incorrect angle bit

[wilkigr]

Thanks guys. I'm getting there; very slowly but surely.

[adze_cnc]

The bit is 1" wide, and the flat depth is set to 1". Will the width of the letter prevent it from carving down to 1"?

 
The flat depth might be unnecessary. But, if this was cut with a 45 degree included angle cutter while the toolpath was calculated as if using a 90 degree cutter then when it is recalculated using a 45 degree cutter there is every possibility that the depth of cut will exceed 1".

The diameter of the cutter won't really affect things as the "V-Carve / Engraving Toolpath" is quite clever about properly sloping the cuts.

For example the widest sloped slot in the attached image is 2.25 inches and the flat depth is set to 1". The cutter was said to be a 90 degree cutter with a 3/4" diameter.
 

[AndyBerry]

For the "Finally the V-Carve Pro cutting parameters for engraving toolpath” image click on “Edit” and take a screenshot of the tool’s parameters.

I have a sneaking suspicion that there is a disconnect between the included angle of the bit specified in the program and the actual angle of inclusion for the v-bit.

Thank you. I don't think anything is wrong here. ???

[AndyBerry]

Which bit did you use? The 45 degrees specified in your posted description, or the 90 degree specified in the toolpath picture?
I think I see the problem.

Mike, super good point. I said 45 degree bit, but it is actually a 90 degree bit. I said 45 measured from the 90 line, but I do mean a 90 degree bit. See photo.

[AndyBerry]

If you could post the CRV file it would be helpful, it's not a problem with the software or the version you are using, I can say that because if it were then the forum would be full of posts by people having the same problem

As others have said this is most likely because the V bit you are using is not the correct angle, if your actual vcarve file used a 45 deg bit rather than the 90 deg bit shown in your screenshot then I would test the v bit to make sure it is actually the angle it claims to be, there is a sticky post about checking vbit angles & how you can test them

The other thing I would mention is not to go by the manufacturer's settings for all your cutting bits, you need to test cutting bits & make adjustments to make sure the settings are right for your machine, the manufacturer's recommended settings may not be right for your machine & set up for a number of different reasons.

here is the crv file. Thanks much for all the help!

PLD.crv

(73 KiB) Downloaded 13 times

[FixitMike]

The file preview looks good, so I'm going to say that the bit that was actually used was not a 90° V-bit. The photo shows a 90° bit, but the actual carving is what happens when a 45° or 60° bit is used where a 90° bit was specified. The tape measure picture agrees with this.

One thing that is contributing to the confusion is that the tape measure marks appear to be spaced at 1/32", rather than the 1/16" that is the usual for most.