Profile cuts requiring tight inside radius

I need to make several of these out of Oak that are 1" thick. I can cut out the profile with a 1/4" End Mill but it won’t give me a tight enough inside radius at the locations where I put an arrow. Is there a trick to achieve this or do I have to go over it a 2nd time using an 1/8" bit, doubling my carve time and carving mostly air. I have some 1/8" Up Cut End Mills where the fluting is long enough for 1" material but I would prefer not to have the tear out even if it’s only at the inside corners. How would you solve my issue? Thanks in advance.

So you have a couple options here

  1. you can run a finishing pass with a smaller tools like the 1/8" to clean up those tight radius but being 1" thick you will be hard pressed to find it unless you have it custom made

  2. you can switch to a 3/16" tool to get you a little closer

  3. you can drill a 1/8" holes and the exact spot of the tight corner and hope that the bigger tool will clean it up

  4. re-design your project to be more cnc router friendly inside corner radius are always a huge hassle when designing but just keep in mind tool diameters when designing items


do you have the measurements for the radius’s that you show in the picture? what are they?

The star pattern is about 15" in diameter with the little circles being just under 1.5" in diameter. What the angles are, I don’t know. I have successfully cut this out using the 1/8" up cut bit I have and I would continue to use it but it takes 45 minutes to cut it out because I don’t want to snap the End Mill and there’s tear out using the up cut End Mill. I would just continue with the 1/8" if I could stop the tear out. Painters tape over the whole piece or spray poly to harden the surface to help with tear out? I’m open to any suggestions


would you mind sharing the svg or dxf? I would like to take a look at something for you

WorkininWoods, I’ll send you a PM.

sounds good

So I am a little confused on the difference between a .0625" radius (.125" tool) and .125" radius (.25" tool)

are you wanting to use this star for inlay? or is it just a cutout ?

in the file I sent back to you I made the star with 2 fillets in those corners .0625" and .125" and they are coming out really close to each other

also I think one reason that your carve is taking so long is because your feedrate is extremely slow

I would start at

18000 rpm

with a 1/8" tool

also if you want to cut faster than cut the profile with a .03" offset with a .25" tool and then once thats finished change your tool to the .125" and then go back and clean it up

This is just a cutout. In the file I sent you, the work piece is only .875" thick (7/8") but the new batch I have to make it has been requested I use 1" thick work pieces so I will need to make that change in the file when I have the angle issue resolved.

Ideally, I would use a 1/8" Down Cut End Mill but I can’t find any that will allow me to cut 1" deep. I know you shouldn’t cut deeper than the fluting provides, especially with a down cut End Mill so I’m stuck using the up cut one I have that allows for a 1-1/8" depth of cut.

My speed and feed rate is so slow because even though the formula says I can use faster speed and feed rates, I snap the End Mills off so the rate I have it set to cut is the fastest real world settings I’ve been able to use without snapping an End Mill. Even at the rate I have it, it’s like fingernails on a chalkboard. I have to wear hearing protection just to be in the shop when I’m cutting them out. I’ll give your 18000 rpm / 60-8- ipm a try and see what happens.

I’m also going to run one using my 1/4" End Mill and see what happens. It’s a little hard to see actual results from the VCarve rendering.

Worst case scenario is I could use the 1/4" End Mill and then clean up the angles on my bandsaw.

In theory, you can start the profile with the down-cut end mill so it creates the top edge then switch to your longer up-cut bit for the rest. If the edge is already established, it shouldn’t be removing the material there, only at the bottom and then, once you get to the bottom edge, the upcut will make a clean edge.

Justin, that’s certainly a good option. I may end up doing that!

imo no matter what you do if try cutting 1" thick stock with a 1/8" tool you are causing unnecessary problems on yourself

you need clearance for the chips to come out

I cut thick pine hearts and wings all the time and here is what I do to get the correct radius on them

I can’t really tell. Are you using a 1/4" End Mill on the Hearts and Wings?

on those I use

.375" to clear out the material
then a .25" to rough out the shape
then .125" to finish the shape with tight corner radius

Ok, So by the time you get to the .125 finish, there’s an exposed area for the chips to go

yes sir thats the game plan

plus you can run the .125" tool at full depth just to do a .02" finish pass with out worrying about breaking your tools all the time


this is the tool I use to do that

Where would I buy that specific bit?


1 Like

Thank you. That’s a compression End Mill. You don’t get any tear out in your Pine with that bit?