Carve letters depth

Are you using vectric v carve?? If so you can set the start depth to a setting lower than the top i.e. set start depth to .025 and it will make them deeper but do so slowly or you may end up making it look kind of funky.

1 Like

Chad… I think I’m just doing a basic V carve. Please explain vectric.
Thanks!
Don

Vectric V-carve is a very popular CAM package. One of the better ones for wood working, or art.

Jim,
I was about ready to try tweaking the Z setting , but it was suggested that F-Engrave might be a better approach?
Have you used it?
Thanks!
Don

F engrave is easy to use, and pretty nice to have in your tool box.
I used to use it a lot, but it gave me some weird toolpaths sometimes.
It’s nice tho, and free and simple.

1 Like

Yes F-engrave does work well but CC does a good job also. It’s important to understand what’s going on with any V carving program and operation. Here’s another sketch to consider. It’s snowing here today so I’m on a drawing roll rather than working :slight_smile:

11 Likes

Jared, fortunate (for me) that it is snowing there today!

Thank you for the detailed explanation of the V carving logic and I do understand. Putting conventional logic aside, I think there will be times when I would like to just push a little further into the material to create bolder and deeper text without having to revisit my original art file. I also understand that if I push too deep, the text grow too much and letters could touch.

I know it obvious I am a beginner, but I am trying hard to lose that distinction!

Thanks again for your help.

Don

3 Likes

Thanks Jerry… I’m going to check out this program.
Don

Don -

Looks like you have plenty of options and info from others here… as you mention,pushing a little further into your material is easy to do by offsetting your Z zero depth, just ensure you don’t overload you cutter. I have F-engrave bookmarked but I’ve not used it yet.

1 Like

2 things to keep in mind, you CAN do it any ways simply by offsetting Z down a bit (Make 0 below the top surface) but doing this make sure the Clearance Z height is enough to get OVER the material between paths.

Also, the text WILL distort fairly quickly. I have tried and found it’s better to find a better bolder font or make the text larger or change the bit, then it is to move the Z offset lower. When you do move the Z lower what happens almost immediately is sharp corners no longer look like flat corners. Take the letter i for instance the top period(dot) becomes an X and the solid bar becomes funny looking also the corners start becoming protruding lines sticking out.

4 Likes

Thanks Roger, I have been in the graphics business for many years, including engraving that started with a manual pantograph to a computer engraver. Those systems used multi-line fonts to create beautiful carvings with crisp corners and edges. I am guessing the software to do this with a CNC V bit would be very pricey, if even possible?
Thanks.
Don

Thanks Jim, I just downloaded F-Engrave last night. I am hopeful this software addresses this problem.
Don

You’ll find that F-engrave V carving works the same way that CC does. What Roger said above is good advice. If you want a bolder font choose one from the thousands available out there rather than having the machine distort one (which usually ends up with unexpected and often ugly results). If you want deeper cuts then use a bit with a sharper angle.

1 Like

Thanks again Jared, your drawings are excellent & I understand what you are illustrating. I just cannot understand why CC or CM does not allow me to adjust the maximum depth.
Will said that feature has been requested by others and he thought F-Engrave might allow it.
I haven’t had a chance activate F-Engrave yet…
Thanks.
Don

What all V-carve programs work at doing is to make the cutter edges meet the shapes outline as the tool bit point follows the shape’s centerline. They all automatically vary the depth of cut to accomplish this. If you try to override this automatic function you’ll end up with either the bit not meeting the outline or going beyond it.

2 Likes

I know in more expensive CAMs you can v carve wider widths than your bit, and add a max depth settings. Like this Ram, the widest points are .32, but the bit is only 1/4".

I was using Artcam 2011, and Vectric is pretty much the same (designed by the same guy).
The bit just does a 10 percent step over, which you can not change.
May not help right now, but if you decide to get a really good CAM, Vectric is great.
It’ll spoil you pretty bad tho :wink:

1 Like

Engraving is actually a simpler process because the depth is minimal and the lines you see are just drawn on to the surface. VCarving is an attempt to mimic the look of the font (on the surface) with the V bit pushed through the material accordingly. If you want a deeper cut look for larger angle V bits OR fatter fonts.

One could easily take any font and offset it’s edges larger in CAD and then save as .SVG file and then import that and V-Carve the fatter font OUTLINE. This would be fairly easy to accomplish and the end result would be a deeper cut and a fatter font.

The calculation for the VCarve assumes the exact outline of the font is on the surface and then calculates the max width that the VBit can be driven down to in order to touch those lines.

2 Likes

I wasn’t clear about the two types of multi-line engraving I do. One is the diamond point drag across a hard surface but the other is the routed variety creating the thick & thin effect e.g. Times Roman. Admittedly however, all areas are routed to exactly the same depth… not a true carving such as what we are doing with our CNC machines.

A possible option may be Estlcam’s carve option. Link = https://www.youtube.com/watch?v=LEFFogenSvo will give you an idea of the options of V- carving with different depths.

Also, F-engrave using the “inlay capabilities” (V-bit outline of the letters and pocket mill with a straight bit to clear-out the area between the outlines.

1 Like

Apologies if someone in the thread already mentioned this. The Vectric software (I own Vcarve Pro) gives the option of setting a “flat depth” and a “flat clearing tool”. The result is a kind of hybrid between a straight vcarve and a pocket cut of the interior of the letters or other carved artwork: the sides are angled via the v-bit and the bottom is cut flat, typically using an endmill.

2 Likes