Vcarve toolpath depth question

[wilkigr]

I'm attaching a .crv file.

As shown, I drew 3 rectangles of the same size.

I ran 3 vcarve tool paths using the same 60° v-bit.

In the first, I simply selected the rectangle and created a vcarve toolpath. No starting depth, max depth, no clearance tool. The max depth is shown as .2165". When looking at the path in 2D view using solid view, the bit cuts to the edges of the rectangle, as expected.

In the third path, I selected the third rectangle and created a third vcarve path. This time, I set a flat depth of .25". However, the max depth is shown as .2165" - the same as in the first path. I expected this because the bit again touched the edges of the rectangle when at a depth of .2165, so it disregarded the flat depth setting.

Now, to the reason for this post and my confusion.

In the second, I selected the second rectangle and created a second vcarve toolpath. This time, I set a starting depth of .02". Again, no flat depth, no clearance tool. This time, the max depth is shown as .2365". This would seem to be the depth as shown in the first path = .2165 + the starting depth of .02. However, this is where my confusion comes in. When I look at the 2D view using solid view, the bit is still cutting only to the edges of the rectangle. How is it possible that the v-bit cut deeper by .02" than in the first toolpath, but did not cut any wider?

Thank you

vcarve test.crv

(43.5 KiB) Downloaded 18 times

[Adrian]

The solid preview is showing what the toolpath will cut without the material above it. Whenever you use a start depth the software is assuming there is no material above it.

Think of the vector for the middle rectangle being set 0.02" below the surface.

You can see the result of the material actually being there in the 3D preview.

[sharkcutup]

by wilkigr -- How is it possible that the v-bit cut deeper by .02" than in the first toolpath, but did not cut any wider?

The Second is actually a tad wider than the others. Measure it by hovering over edges and reading the Y: from data at bottom of drawing window. Second and Third Rectangles Subtract dimensions. The first you will need to ADD the dimensions because it is centered on the XY Datum. It is not an accurate measurement but it does in my opinion show that the Middle (Second) Rectangle is slightly WIDER than the other two.

Sharkcutup

[Adrian]

It isn't any wider in the 2D window only in the 3D which is correct. Change the start depth to a much larger figure and you will see the 2D preview doesn't change.

[sharkcutup]

It isn't any wider in the 2D window only in the 3D which is correct. Change the start depth to a much larger figure and you will see the 2D preview doesn't change.

+1 Agreed

2D -- What program is telling machine to do
3D -- Reality of the Carve with all Conditions (parameters) combined

Sharkcutup

[wilkigr]

Thanks much to you all. I must confess that I did not actually cut material. If I had, I likely would have seen that the path using a start depth ended up being wider than the others. Since this is the objective, it worked! Now that you all have confirmed that, I will do a short test cut, just to get an idea as to what start depth I need to set to get the results that I want, then go from there.

Thank you again.

grant

[martin54]

What is it that you are trying to accomplish? using a start depth so you can cut to a certain depth probably isn't the best way
Something you also need to take into account is that the software assumes there is no material above the start depth so your first pass with be whatever start depth you use plus the depth of cut set for the bit

[wilkigr]

That's an excellent question, Martin.

I am asking this for another CNC user - really.

The situation is this. The user v carves letters onto rough barn board type lumber. These are to be things like cottage signs. The problem is that, if he uses a touch plate to set Z0, since the plate rests on the highest part of the rough lumber, the cuts on the deeper part of the "grain" are too shallow. They do not touch the inner and outer vector of the part of the text that is being cut on the deeper part of the grain. So, the cut is too narrow.

To date, his solution has been to set Z0 as usual, but then actually lower the bit manually by turning the Z axis pulley. He does not reset Z0 at this new height. This does achieve his objective of getting a deeper cut. However, to me this is not an optimal way to achieve it, since the machine and controlling software no longer "know" where the bit is.

I was playing with the idea of achieving his objective by setting a start depth. I realize that Vectric assumes that the bit is cutting air for that depth, and in this case, it is only intermittently cutting air, but with a small enough start depth, I thought this would not cause a problem.

I am certainly open to be proven wrong. In hindsight, I should have explained all this at the outset. I apologize to all of you who offered advice without me providing all the facts.

[adze_cnc]

Can he not: set the Z0 with the touchplate on the board. Remove the board. Move the Z down via pendant / control pad to negative whatever he figures is fair. Then set that as the Z0. Replace the board. Cut away to his heart's content (making sure VCarve raises his normal clearance plus the amount of material that is actually above the new ZO).

I have it good in that our machine has a function which sets a value that is added to the actual Z0 to temporarily move the Z0 higher or lower than it really is. e.g. Your material is sitting on a 1/2" platen? F27 = 0.500 now the Z0 is 1/2" higher than it was until F27 is reset to 0.

[Tex_Lawrence]

… They do not touch the inner and outer vector of the part of the text that is being cut on the deeper part of the grain. So, the cut is too narrow….

With the thickness of the wood in mind, one way to solve some of this is to change the angle of the bit doing the cutting.

[SteveNelson46]

You could also set z-zero to the bottom of the material (spoilboard) and regulate the depth of cut by adjusting the material thickness. Of course this will affect all toopaths until the material thickness is reset and the toolpaths are recalculated.

[martin54]

If the letters are carving to different depths then then setting the z zero once is always going to give you different depths with the letters, moving the z axis down will cut those letters that are very shallow deeper but it will also cut the letters that are the correct depth deeper.

I have done a similar thing on a couple of occasions & my method was a bit time-consuming. I carved the letters 2 or 3 at a time & for each set of letters I reset the z zero on the material in the area that the next set of letters was going (if that makes sense)

[wilkigr]

Excellent option suggestions. Thanks much.

IMHO, if he is getting the results that he wants by lowering his Z gantry manually, his better approach would simply be to follow adze's suggestion and use the jogging feature of his controlling software to lower the gantry, then resetting Z0.

That said, I will pass along all your suggestions.

Thank you again for your usual excellent responses.