I’m using a v-bit to carve a circuit board. I’m using Estlcam and after I save the project I use ctrl-A to select all the cuts and enter .3mm for the Depth limit. I check several traces to make sure they are all .3mm. Then I save the cnc program and open Repetier-Host. When I look at my gcode all the depths for z are.05mm. I try running the program anyway and the v-bit barely touches the board in some places. I used the Tiny touch plate to set Z axis first. I don’t know whats going wrong. Do I need to enter .3mm in Maximum Carve Width?

Clear Front Traces.gcode (768.4 KB)

You say you carve? Do you actually use the carve command? If so, it will only go as deep as it needs to carve out the specified carve area, since you can only set the max depth, not actual depth. If it’s very tiny, it won’t go that deep, because it already cleared everything with 0.05.

Yes. Estlcam’s instruction for Carve says: “This function requires a pointy engraving tool whose line width can be controlled by changing the cutting depth”. I’m using the 45 Degree V-Bit because I only need to go deep enough to remove the layer of copper plating on the board to create circuit traces. So .2 or .3mm should be enough. I’m just not sure how to set that depth for all carves.


The cross section of your V endmill seems off. You have to put the value in that it has on the thickest part and the angle, it then calculates the tip. The tooltip in Estlcam might help, but can’t check right now.

Edit: You can see some settings here. She has got a 3mm endmill with 45 degrees: Bit Settings on EstlCAM - #5 by scrounge79

Edit2: In Estlcam you use the full degree, not half of it like in some other programs. Have a 90° bit, put 90, not 45.


I would use the “Engraving” path tool instead of the “Carve” path tool. The Carve tool wants a parameter based on how wide you want the carve, not the depth. This is meant for 3D-ish contour carving. The Engraving tool you can specify if you want the tool path to be directly on the line, or one side of the line. Once you have all of the paths created, you can select all of them and modify the depth parameter so that they will all match. I would probably also use a V-bit with a much deeper angle, so that the tip is as small as possible at depth.

This is likely due to the workpiece not being level with the gantry. You are dealing with sub-mm depths, so your level tolerances are going to be very tight.


So i see a 1\16 bit in your list. Engrave and this bit wouldbe better. V carve would have a hardtime making your holes.

And that bit should be a 180 not 90

The circles on the board are pads with a 1/16 hole in the center. I’m using the V-Bit to cut either on or outside the line on the circle. I was going to change to a 1/16 bit to do the hole in the center. I have a separate file for those. I just have to make sure my 0 position doesn’t change when I switch to that file because the tolerance is very tight.


On Engraving I don’t understand what it means by left or right side. What does it do with a circle? Does left mean outside and right mean inside?


Guess I should have looked at your drawing. You have a lot of work to do on that. ESPECIALLY those long paths. I am not sure there is enough room between to carve out the pcb to not have continuity.

You may have to do a double sided pcb for that to work. On top every other path and on bottom the ones left. Evens and odds if you will.

You might get away with “parts” and “holes” which should clear up any ambiguity of which side of the line it’s cutting on. But you probably want to adjust the artwork to ensure a minimum distance between the traces.

Even better is if you can make it so the copper areas left behind are represented in the artwork so it won’t get confused and try to pocket out those areas.

This is actually the first side of a double sided pcb. Here is the other side.

Oh wow!! And this is about 6 inches??? I am not really sure how you are going to do this!!!

How deep do you have to go to sever contact?

Also the diameter of your v bit says .1mm are sure that is correct?

Looks like maybe a keypad and display. Not a lot of wires, so maybe display speaks I2C I would guess.

Jamie have yiu done pcbs? I just looked and youtube shows to etch the paths is that correct?

Shoot not etch ENGRAVE. sorry wrong terminology!

Heh, yeah, I don’t really know why that is named that way. But for a closed shape, it’s basically inside or outside like you said.

I have only done the ferric chloride method and only a couple times.

Engraving the perimeter of a copper area will probably be okay if the engraving is narrow (shallow) enough but the area will be a bit smaller than the original design. That could be okay but it’s harder to predict whether there might be some narrow traces that disappear, so that’s why I would tend to try for a more faithful reproduction of the copper/non-copper areas.

Another thing that’s possible is to lie to EstlCam about the bit that you have, where you give it a radius and cutting depth so it offsets appropriately. Then you don’t have to trust that it will carve properly based on the V-bit angle. I’m not sure that part/hole properly respects the V-bit angle.

This is what the pcb is for. I built one just using wire in between the tactile switches but its kind of a rats nest and I’m having some connection issues so I wanted to make something a little more clean and stable.


I tried that also. I even built an etching tank and a led exposure box. The ferric chloride would always take out part of the traces so I would wind up with a lot of bad connections. It was a lot of work and expense for nothing. I watched a lot of youtube videos of people who said it worked for them but I could never get it right.


I could have been using CTRL+a to select all the cuts this whole time?!? God damnit

It means if you have say a box, just 4 lines.

Example with 1/4” endmill:

you go center on line, and you’ll be cutting 1/8” on either side of the line.

If you go outside the line, you’ll leave the box with 1/4” cut outside the lines, like an outside pocket.

If you go inside the lines, you’ll have the cut on the inside, just like you would want with a pocket.

Because your tool has width, your selecting where you want the tool to be in relation to the line.

When I engrave with my 60d vcut I do on the line with good results.

It took me a little bit to figure it out on estlcam because it changes how things look. But you can do this to help see what it’s doing.

Make a box set to your grid size (view > grid). For example mine is 25.4mm (1inch). So I would make a 1” box in say fusion, just a drawing. Then open in estlcam, and select to engrave it, then play with the line options (inside, outside, on the line). You should be able to see easier where the line is moving. Try with making a 1/8 or 1/4” bit so the cut is bigger to help see it too.