I'm new to CNC and I typically cut out 3d models I've downloaded from the web. I use Meshcam to generate gcode. When sizing my projects many are beyond 19 mm. I decided to start purchasing 2 inch slabs off Facebook Marketplace and plain to thickness for project. I have deep cutting end mills for rough cut but when when it comes to ball nose for final pass most bits have a 1 inch cut depth. Thinking about this for some time. I think that once rough cut is made in most cases 1 inch cut depth for final pass should be OK except cutting around edges of projects and some pockets. Can anyone provide advice on how they accomplish cuts/3D with wood thicker than 3/4" (19mm)?
If your machine can take a 6mm or 1/4" bit, then tapered ball-nose bits are available that have a decent long reach (30mm+ of fluting is not uncommon) and many can run with a longer stick-out of 50mm or so. The taper makes for a nice rigid bit, but sometimes the taper angle can mean straight sides on some models have a slight slope, so it is a trade-off against a long-thin straight sided ball-nose. With either tapered or straight ball-noses, luckily most of the finish cutting is close to the tip region of the tool, so low regions of the model that are nominally beyond the length of the flutes can still be cut, although crashing the collet into the higher regions can be an issue too. Yes rough-cutting away as much as possible really helps if your flute length is limited. Sometimes just changing the direction of the cutting path (i.e. whether X or Y does the main pass) can help with handling steep edges. I had one bird-skull model on a rotary axis where the eye sockets were small but crazy deep. I did a rough cut with a large normal end mill first (which did nothing to clear the pockets), and then isolated the sections of the model with the deep pockets and used a taper ball-nose with a reasonably large tip diameter to then to a 'rough' pass of just the cavity regions. I then did a full pass with a much finer taper ball-nose. The advantage of using a 'roughing pass' with the slightly larger taper ball nose was that I could limit the cut-depth per-pass more easily with the roughing cycle setup options than with the finishing cut options (Vectric Vcarve software). With the long stick-out of the tool, tool deflection was a major worry, and I did break a bit when I first tried the cut and did not rough out the eye pockets where the finishing pass plunged right in. For other cuts where there are deep pockets, but only deep enough that the tool will deflect lots and not break, I just wear ear plugs under my ear defenders so that I cannot hear the bit screaming so much
If your endmill is short enough where your collet may hit the surface of the uncarved wood perimeter, you can cut a wide profile around the model that clears a wide and deep enough path for the collet but not too deep you cut though the material necessary for your tabs. This way you can get down with a shorter endmill. If it is a single sided carve you can also create a mounting board where you fasten your work stock to it from the underside in an area of a carve that is guaranteed to be thick enough that you won't carve into them like this: This piece is then fastened to the spoil board. Then rough and profile cut. No tabs necessary. Throw away the scrap and move on to finishing. Because you profiled first and tossed the scrap, it is out of the way of your collet. The screws that were put in from the back hold the material securely. This is how I have started doing all my single sided carves. It was not necessary for me in this one because as you can see from the photo, my 150mm long 3mm diameter ball nose endmill will get where I need it, but it will quickly become a 100mm long or shorter endmill if you screw up because they break easily. In 3D caves you are only using a 10% or less stepover, so there is not a lot of force. I am cutting at 3000mm/min with these endmills. I have also broke end mills when the roughing pass did not clear a deep hole.
