Chip build up cutting grooves

this is the second time happening during similar cuts. after two or three passes the chips get packed in the slot, They’re so packed that I’m digging them out with a small screwdriver and sucking up with shop vac. I’m cutting out strips in maple 1" deep. I’m using a 1/4 compression end mill, 80ipm feed, .125 stepdown and around 14000-15000 rpm. I have a jet 610 dc using a 4" hose. Is it feeds ,doc, dust collector, Would a straight up cut bit be better. I don’t want to have to sit there for hours digging out chips. for the record chip size seemed to be ok. Any thoughts would be appreciated. Here’s what I’m doing. This was a program test . In the future I would be cutting double that amount. I will cut off the ends to make strips


Yep, I can confirm that a compression bit will pack the sawdust into the cut, in fact, your dust collection won’t have any chips to suck up as you have already seen. Just a point, a compression bit is designed to cut at full depth in a single pass, i.e., if you have a 3/4 inch board, you should cut at 3/4 depth per pass + about .005" into the spoil board.

I know that sounds scary, and it alarmed me for the first 10 times I did it, but you just have to get used to it, as it works. BTW, you’ll still need the screw driver afterward, or just pick up a hammer to knock out pocket cut extras.

If you mean by straight up cut, an upcut spiral, then sure, it won’t pack the chips in, but a warning, you better have a very strong hold down (no blue tape and CA glue) as upcut spirals have a very strong uplift and can separate the tape at the worst time (ask me how I know, but I have cheated death a couple times, flying wood can be very annoying).

1 Like

That does sound scary. I can make the board longer an screw it down like I did with this one. Would you do a one inch cut, if so any idea on feeds and speeds I also want to make some 1.5" . what would you do for that. I thinking it would have to be multiple cuts thanks

@Pleased2fly, interesting that you go full material depth on your DoC. With compression bits I shoot for a first pass a reasonable bit past upcut at the tip, eg, 3/8” for a 1/4” tip. I also try to put the final pass with the bottom in the middle of the tip.

On a 1/4” wide bit, 3/8” is not as scary as .755” plunge and slot seems.

Interesting. I use a lot of Amana bits and their listed DOC isn’t the same as the LOC - generally they appear to be the same 1/2 the diameter that’s the rule of thumb I learned from Shopbot.

What they teach is that you need another measurement with a compression but - the length of the upcut portion. Then they have you set your first cut depth to be a bit more than that length so your top gets cut with the downcut portion of the bit.

Then when you get to the bottom, you make sure the last pass is less than the upcut portion length. That leaves the cut through the bottom surface with the upcut spiral which makes for a clean cut through.


Compression bits are intended to be run at the full depth of the material, the depth of the cut will determine the diameter of the bit you should use for strength purposes, with D >= 1/2 material thickness. As I understand this makes the 3/8" compression bit very common for most cabinet shop applications where 1/2" - 3/4" sheet goods are typically used. Using a 1/4" bit at a 3/4" DOC is possible but you need the speed and feed dialed in without much margin for error, and may be a bit much for the Makita router to push for long periods of time.

I have used the approach @JimHatch mentioned when smaller diameter bits are required for detail work in thick stock, make sure the first pass is deep enough to engage the downcut portion of the bit.


I’ll get an upcut and try that. how were my speeds and feeds?

You could probably go a little faster than you are but if the current settings are working for you and leave a good finish quality go with what works for that material. 1/4" DOC .25" step down 140 IPM @ 18,000 RPM would usually be my starting point for hardwood with a 1/4" diameter endmill.

If you are going to cut the ends off, why do you care?
They will separate then anyway…


not sure what you mean cymro99

Why clean out the chips before they are separated? If not impacting the carve, why not leave them clogged until you cut them apart at the end and then the chips will fall away? Or perhaps I am mis-reading your post/process.

Derek - I think 140ipm at 0.25" DOC is a little aggressive to start with – perhaps 100 or 120? I guess it depends on the wood – hard maple would be a little sketchy vs walnut or cherry IME.


1 Like

Depends heavily on the RPM to determine the chip load to speculate… if I use the specs from Amana they’ll tell me 180-240 for many of their 3 flute 1/4" bits .25 DOC @ 18k RPM

1 Like

It does depend on RPM – that said, Amana doesn’t specify DOC in their recommendations (that I am aware of). That’s why I recommended a slightly lower surface speed at that DOC. I wish speed recommendations specified the recommended DOC too, but they usually don’t since they are based on chip load. All that said, experimentation is key and knowing your material is essential (as you noted as well).


I see it in their recommendations:


Yes, OK - you got me :grin:

I had a simular cut and the the machine crashed into side of the piece. It might have been something else but I believe the packed chips caused it

@bkwoood how many cutting edges are on your 1/4” compression bit? I think you could go faster than 80ipm, especially if you have a 3 flute bit. Regardless, you’re chipload is .002”-.003” at the speeds and feeds you’re using. The 1F can hang from a rigidity standpoint. I’d shoot for a chip load in the .005”-.006” range and see if that helps. It’s not quite an industrial level machine, but I find it handles 50-75% of advertised chip loads no problem. Maybe even 100% in certain cases, although haven’t tested that myself.
Also, maybe you’ve tried this, but if you re-run the program does it get the chips out? Easier than a screwdriver and I bet a pretty quick run time. If that works, you could simply add a “finishing pass” at full depth with no offset that’s used as a chip clearing pass. Essentially repeating the last pass in each slot a second time. That could be a really quick solution.
One other thought, you may consider ramping into the material if you’re not already. Might be a little tricky with those nicely curved slots you’ve designed, but could help at the start to avoid a chain reaction of build-up for the rest of the cuts.
I run a 1/4” compression bit in birch ply and use the approach @JimHatch described. My first pass is deeper than the “mortise height” that Yonico advertises so that I take advantage of the down cut potion of the bit that’s higher up the tool. I try to keep my depth of cut less than 1 cutter diameter (.25” in this case) and maintain equal steps, but that’s not a requirement. Just my toolpath OCD :joy:.
I believe I ran that thing at 180ipm and 16K rpm. Lots of noise, but beautiful edge quality and no chips stuck in the slots. Room for improvement on those feeds and speeds. Loudest when the machine was slowing down to change directions. Quiet when going fast in the straight cuts. Maple will be different, but I still think 80ipm is the culprit here.
Cool part! What’s it for?


Compressed air nozzle with improve things and with some trial and error should remove the problem totally
A lot of the items we produce are profile cut shapes in British hardwoods to a depth of 40ish mm
I run an 8mm air line clipped to the flow and return cooling lines for the spindle this is fed by a regulator and gauge from the air compressor in the workshop
I run either a single or twin set up of this type of hose Coolant Hose Kits - Flexible Coolant System Hose Kit (
This is just an example many kits nozzles and valves are available
It will take a bit of tweaking to get the jets just so and very often its more efficient to either run without dust extraction or just use it intermittently
I pretty much us air on most of my production jobs on the onefinity

1 Like

Thanks. I make a cutting board with 4-5 different species. Cutting them out instead of bending in a jig will save me a ton of time. when finished the pattern forms a 3d wave effect. This was my first attemp cutting them so I know I have to play around with speeds and feeds. I just ordered a 7/32 up cut thinking i’ll run that as a rougher and follow up with the 1/4 for a finish cut taking about .015 per side.