Quick question on my XXL with Z-Plus. I have a 1/4" compression endmill and a 1/4" down cut (among many others). My understanding with the compression endmills is that you have to start your depth of cut at the depth of the directional change, so basically where it changes from an upcut to a downcut. On mine, that’s about a quarter inch. My question is, I have quite a bit of work to do on 12 mm Baltic Birch, it seems like just plunging 1/4" is a little aggressive on that material. When I enable ramping, as I usually do, it obviously defeats the purpose of using the compression endmill since it uses the upcut portion for the distance of the ramp resulting in poor surface finish over the ramp.
What’s the consensus? Is it better to go a little less aggressive with a downtown endmill (e.g. .125 DOC) or plunge the compression endmill at the full .25"? Or, is there some better strategy like using an upcut endmill, then a finishing pass with the compression?
Compression bits work well on high powered cnc machines because they have the power to make a full depth cut; n plywood. This full depth cut takes advantage of the up/down capability of the bit. For a Shapeoko that is not possible due to the limitations of power and strength. I think you would be better off with a up or down cut bit and small depth of cut. Compression bits are designed for full depth cuts and that defeats thier purpose on Shapeoko.
Yeah, that’s kind of my feeling as well. There seems to be some talk of using a quarter inch depth of cut (i.e. official feeds and speeds chart), but that feels just a tad bit aggressive to me. From my understanding, and limited experience, the minimum depth of cut seems to be the directional change.
You could use the roughing and finishing approach: first cut slightly oversized profiles (using the offset feature in CC) with any endmill and the usual depth of cut limitations, and then use the compression endmill to do a single, full depth pass (actually more than full depth, overcut the bottom slightly). The finishing pass with the compression endmill will only shave off little material left from the roughing pass, so it will not be a pb to run at full depth. And you benefit from clean bottom and top edges due to the compression endmill geometry.
I might give that a shot, that’s one of the options I was considering. Are you roughing with a downcut or upcut? I found that even with a conservative depth of cut, the upcut can really tear out some of the fine pocket details that I need. In other words, the top ply between a couple of pockets might get torn off when I use an upcut bit.
It depends on how detailed the features are, if I have small areas in the top veneer which can get pulled up easily I use a low helix downcut, cut reasonably shallow passes (3-6mm) and keep the machine moving fast (>1,000mm / min) to avoid recutting chips or heating up the bottom of the cut, dust extraction really helps with that as the slot is empty for the next pass.
I have had good success with these cheap cutters from Amazon
But since wearing the sharp off the ones I got last year I’ve grabbed some of these from a proper local tool supplier
and they’re nice and sharp, closer to the stated diameter and sail through ply.
I’ll probably get my down cut a shot, I think it’s a Whiteside so it’ll probably hold up fine. I may test one of my up cut bits as well just to see how it performs, most of the tear out I was having was during the ramping while using my 1/4" compression.
I’d suggest trying a contour toolpath for roughing with 1mm stock to leave, multiple depths at 3mm or so, then come back with a finishing contour toolpath, no stock to leave, multiple finishing passes, 0.5mm stepover per finishing pass, all full depth.
I had good results with that approach. If I really care about the final finish then I use the compression cutter but using the low helix downcut, if the spoilboard is good and flat the bottom finish is pretty good anyway.
Carbide3d bits are good bits but I use Whiteside 2 flute 1/4 bits in place of #201 bit with good results. RU 2100 up and RD2100 down cut. I have a lot of Whiteside bits and all work great.
Compression bits with very short upcut sections are available. The ‘Jenny’ from Cody’s CNC (https://www.cadencemfgdesign.com/shop) has an up cut section of about .1". The upcut and downcut sections overlap, so a DOC of .08" gives a compression cut.
I use a cheap 1/8” compression bit in birch all the time. What I’ve found is that if you don’t go down at least equal to the dia you will get tear out. What works for me is 3 passes of 0.168” for 1/2” (12mm) at 75ipm (1905mm/m)
This always gives me great results with very little sanding.
That’s good to know. I have a 1/8" compression as well, I guess that’s a good point that the compression switch is shorter on that bit, I guess I just always reach for my 1/4" bits when I can. I’m assuming you are just plunging with that, no ramping?
May I recommend using a straight cut endmill. It leaves a clean top and bottom, it throws the chips evenly around meaning my dust show can pick up the majority of it.
Amana Tool 43824 - This is what I use on my plywood merchandise that I sell.
The Amana is a 2 flute straight bit with no shear up or down. Recently I had an outdoor project with 2by material. I only had one upcut bit with 1.5 inch cut capacity. I ordered two straight bits with 1.5 in cut capacity and did not use them yet. I have seen several youtube videos that compared up/down and straight bits and the straight bits did better on plywood than either up or down bits did. I dont cut plywood very much so I will use then if I get a plywood project.
You know, I’ve always stayed away from straight bits in my cnc. I’ve used many over the years in my routers, but they always seemed a little rudimentary for a cnc. That’s definitely great if they work for your uses though. This video is pretty informative and kind of illustrates my issues with straight bits:
