So, I recently bit the bullet and bought vcarve desktop. I haven’t actually carved anything with it yet…
My question is about depth per pass when vcarving. It is my understanding that on a vcarve operation, the software doesn’t allow for multiple passes. That is, one single pass, that v bit is going to plunge to full depth, whether it is a 16th of an inch or half an inch.
Does that work well in practice? I have the Dewalt router, but just how deep can I really go with vcarve without having the forces just be too great? Suppose I’m carving a sign in cherry wood, or maple, not just mdf. Is that kinda a design flaw? Like, should they allow for multiple passes and this is a problem with using vcarve?
Let me know what you think. Carving in a single pass makes me nervous!
It all depends on the bit you’re using, the material hardness, your machine’s stiffness, etc.
You can cut 1/2" per pass or more with the x-carve, but you need to adjust your feed and rpm acordingly.
So, let’s say I’m going half an inch deep in a hardwood. Does that mean higher RPMs and slower feed rate? Am I understanding right? Or will that just burn my wood?
Not necessarily, you will burn your wood if you’re rubbing instead of cutting. Depending on the tool you’re using, for example, a 2 flute carbide V bit i have recomends a chip load of 0.005", using the formula:
Feed = RPM * chip load * flutes
16000 * 0.005" * 2 = 160 IPM
That should work ok, if your machine has enough stiffness and your spindle has enough power.
@StevenPaxman you don’t have to do full depth cutting especially at .5" Vcarve should allow you to set a depth per pass
I have the 24v spindle for now, so I have to take a more light approach while still keeping the chips big enough, but either way the depth per pass is set on a per tool basis, so you can see some screenshots of my rather conservative numbers below, but it should give you an idea for where you can go to set yours:
Sketch42 hit it on the head, Steven. You can set multiple depths in V-Carve, just like any other CAM software, no worries. It will just make the pass, come over the appropriate amount, and make the next one deeper so that the walls come out at the proper angle.
Thank you for this, @sketch42. I really need to keep diving into this software. So simple, but so complex at the same time!
You can “Copy” that bit and rename it describing settings for a particular material. So you could have a 60 degree half inch v-bit for HARDWOOD, that has a shallow depth per pass.
I did this for a keyhole slot cutter. I just copied a quarter inch end mill and increased the depth per pass to .25" and adjusted its plunge rate to 5 ipm and remembered to RENAME IT APPROPRIATELY.
THis is important because once you adjust your settings for that bit, they are saved. And you don’t want your MDF settings applied to your aluminum milling (been there!).
Also, once you select a bit, the EDIT button allows you to make changes to its settings.
As @Earwigger points out, Selecting the tool, loads that tool along with all it’s pre-configured speeds & settings.
It’s perhaps worth pointing out that when you select or load the tool in V Carve, just accept all the settings for the tool, then once its loaded, click on the “Edit” button (right next to the “Select” button). You can then change all the parameters you wish (pass per depth etc) to suit the work you’re doing on the current job, without affecting the original settings associated with that tool.
This way, you can keep the default (or preferred) settings for each tool unchanged in the database and just tweak them to suit the job you’re doing.
Like @Earwigger et all have said you’ll want to edit the tool on a per material per bit basis… every bit is different and requires a differen sweet spot for each material, so it would be handy to copy the original and save out a different tool setting for each type of material.