Any successes with compression bits?

I’m trying a pretty big project in 1/2" baltic birch plywood and it’s not going great. I initially did it with a regular 1/4" upcut bit and the tearout was bad enough to scrap the project. I did some reading and decided to try a compression bit. I just got done with an attempt, and so far I cant even finish the run.

The issue is, for the compression bit to work properly you have to take a deep enough bite for the downcut portion of the bit to get into the surface. On my whiteside bit that look like about .25"

So, I set the DOC to .25, speed to ~18000 and feed to 40ipm and went for it. I found out real quick that either I’m way out of line on something or the machine just plain doesn’t have enough ass to get the job done. It cuts clean, but I can see it deflecting and I keep losing steps, especially on the Z axis.

I tried adjusting the feed all the way from 4ipm to 40ipm, and tweaked the speeds a little, but nothing seemed to help much. The cut is nice, but the chattering and deflection are still present with all the settings I tried.

I’m fixing to try separate upcut/downcut tool paths and do this in two parts with some tool changes. I’m just wondering if anyone else had much success with these compression bits - and if so, how? It seems like the obvious answer is a shallower DOC, but at that point it seems like you’re just using an overpriced upcut bit.

@David David: It took me quite a while to figure out compression bits. At first, they made no sense to me. The first part of the bit is an up cut, so I couldn’t figure out how that part would not lift the top surface before the down cut portion of the bit got involved. Then, I learned about ramps and leads.
I don’t know what software you are using, so all this may just be jibberish. In VCarvePro, the key is to use both ramps and leads. The lead starts outside the tool path for your parts, and the bit ramps in from that point. By the time the bit is actually at the start of the “real” tool path", it is deep enough that the down cut portion of the bit is engaged. This way, you get a clean top surface and a clean bottom surface, since only the up cut portion of the bit cuts through the material.
I’m sure that there are other ways of getting the best out of a compression bit, and I’ve very limited experience with them, so take this for what it’s worth. However, I get no deflection on a 1/8" compression bit owing to the easy ramp and I get clean surfaces thanks to the lead.

Hi David,

I’ve been experimenting with compression bits for a little while now. Do you have the part number for your particular bit that I could look up?

I’m actually running mine much faster than 40ipm but at a lower RPM and deeper. The inclination to run super shallow and slow isn’t as applicable to compression bits and can actually be detrimental from what my research has turned up.

I’ve been experimenting with 7mm-8mm depths. I also did some experimenting at full depth in some pretty crap 1/2" plywood (only 4-5 layers, nothing nearly as hard as baltic birch). Results were so-so but the wood is so bad I can’t draw any conclusion. It did sound nice and gave me nice chips instead of dust, but the super thin veneer was tearing a bit.

Working in 1" baltic birch recently, I had a decent experience using a 5mm step down (about 1mm beyond the upcut portion of my particular bit, a Yonico I got via Amazon) at a 2520 mm/s feed rate. Grant already spoke about ramps and leads, good info there.

I have read conflicting info about plunging - both that you should NOT plunge a compression bit (should ramp it) and that you should plunge a compression bit. I think the correct answer is to not plunge it as the downcut nature means no room for chip ejection so you can heat up the bit and wood pretty quickly. However, at a 5mm depth of cut I don’t think it’s a huge issue but I could be wrong.

I have had good luck with 2520 mm/s at 17,000 RPM (Makita 3 setting) and 5mm in baltic birch, with a ramp to start things. If you have some spare material to experiment in, you may want to try 3048 mm/s at 8mm ats 10,000 RPM to compare.

Let us know your results if you do try it.


1 Like

@jwoody18 Jeff: Do you use leads, too, or just ramps?

The bit I’m trying is whiteside’s UD2102

I think you mean to say mm/m, unless I’m messing up my conversion. I think 2520 mm/s would be something like 6000ipm, which is halfway to light speed. 2520mm/m works out to about 100ipm, which I have tried with other bits mostly unsuccessfully. I found that the machine will cut OK at that speed, but lose steps here and there even with a shallower DOC. The whole thing is confusing as heck to me, because all the reading I’ve done tells me that most of these bits NEED to go that fast to cut properly and not overheat, but these hobby machines just won’t do it. Some of them even call for 260+ipm. Which seems to leave us in pure trial and error mode, and just accepting that bit life is going to suck due to machine limitations.

I have been using ramping in VCarve on all these attempts, and trying a ramp length anywhere from .5 inch all the way to 4 inch. Not sure what a reasonable ramp length really is, though, and I havent seen a lot of difference yet in my trials.

Honestly, I don’t know what leads are and haven’t messed with that. That’ll have to go on my to-do list to figure out.

Edit: Just for more context, these attempts were made with a step down of 6.35mm, so right in the range you’re talking about. The top of the cut is definitely smooth, but the machine was deflecting and chattering and losing steps at 1000mm/m, all the way down to 100mm/m. I think what I’m hearing here is the solution might be to crank up the freed rate and see what happens. I’m a bit scared to do that - I was feeling like I was going to break the bit at 1000mm/m.

I upgraded my machine with the electric motors from a Tesla Model S and can now run at about 120 KM/h in the Y and 100 KM/h in the X. :stuck_out_tongue:

I really must stop making that mistake, you’re correct, mm/min was what I meant to say. Sorry for the confusion.

@David I did the same research you are doing about feeds and speeds for optimal performance and have reached the same conclusion you have - the machine just can’t go fast enough for some of the bits (at least at 1/4" diameters) that we would like to use. I’m about to order some 1/8" compression bits for this very reason. I believe if we drop down to 1/8" that we can run them at recommended feed & speed rate ranges on the Longmill. However I am concerned about their fragility and longevity and also about deflection. I’m seeing consistent issues with deflection at the moment and it’s giving me gouges where ever there are tabs, very frustrating.

The other thing I’m contemplating is upgrading to the higher torque (about 80% more) motor option that LDO offers in the same model/part range as the existing motors in the design. It’s a 76mm deep body instead of the current 57mm but otherwise shares the same bolt spacing etc.

I think for carving operations it seems like the machine works quite well and lots of people are using it in that area. I’m more interested in larger pieces, often tiled for longer lengths than 30", and from 3/4" and thicker materials. However, I’m also still struggling with maintaining consistent tightness on wheels and eccentric nuts etc. So maybe it just isn’t practical to push the machine further.

So those are my two directions of investigation - smaller compression bits running at full recommended feed and speed ranges and alternatively looking at larger motors. The motors aren’t very expensive and are easily swapped back to stock so both avenues are within reach.


Before I forget, you haven’t really mentioned RPM again. Try dropping your RPM down to 1 (10K RPM) and slowly increase it from there. I was running at 17K-18K previously, based on other recommendations and I find it actually works better at lower RPMs. If you’re running slower than recommended on feed you should really reduce your speed as well.

Make your own decisions, of course, but for feedback I ran a long tiled job (about 5’ long) last night (dado slots, circular dog holes and multiple finishing pass contours) and happyily ran the Sienci 1/4" Up cut bit at 3048 mm/min (120 ipm) with great accuracy at a 6.35mm depth of cut. Total cutting time was about 1h spread across about 7 toolpaths.

Granted, this was basically the first time I used the bit so it was super sharp, but the machine didn’t make any alarming noises or cause me any issues. I did find after the first half of the job that I had some play in my Z axis wheels that required tightening things up (I’m constantly chasing wheel tightness issues - not sure what I’m failing to do/understand there). I can’t say for sure that looseness was a result of this particular job since I didn’t check before starting (I will from now on). I ran the almost identical second half of the project (after moving the workpiece for the tiling operation) and it was tight as can be when the second half of the job was done.

Interestingly, I had virtually no tear out with the up cut bit in moderate quality 3/4" plywood and a 6.35mm DOC. I can only assume this was because it was super sharp and I don’t expect that to continue, but I didn’t even bother switching to my compression bit since the upcut was cutting so cleanly. Also, upcut and downcut bits have lower optimal feed rates so I think I was closer to the sweet spot (although I didn’t check mathmatically).

All that being said, I have a feeling a 1/8" compression bit (I’m going to order a 5 pack of Chinese ones from Amazon) may be a sweet spot but at the risk of serious deflection… I also have a 3/8" downcut finishing bit here I was intending to try but further research suggests that is the wrong direction to go. I think I’ll save that for use on the 4x8 machine.



I need to pay more attention to this. I got really in to setting leads and entry points about a year ago when I first started using the big machine but I’ve bee fairly lax and just accepting the Fusion 360 defaults for now. I’m noticing that I’m having gouging on my edges both at entry points and anywhere I have tabs so I need to figure out what is going on with that.

When I do use leads I like to feed past the entry point as well as that is supposed to smooth over the issues I’m seeing, but I think mechanical deflection is serious enough that isn’t happening. It may simply be a function of the depth of cut I’m using but I don’t think so.