I’m looking for suggestions. As the title says, I’m in search of an 1/8” extra long end mill to cut through 1.75” thick pine. It needs to be that diameter in order to maintain some inside cut detail otherwise I would use 1/4”. Any advise would be great, also If anyone does this could you share your bit parameters?
Thank you in advance
I’ve personally never seen one that long, but I bet you could find one… However it’s going to be VERY delicate.
What’s the design that needs this? Could you do dogbone inside corners instead with a larger bit?
Thanks for the response Eric. The job is a decorative architectural corbel so all inside corners will be visible. I plan on making multiple cuts for the full thickness. If an upcut is used is it necessary for the cutting flutes to be the full length or will the chips be ejected enough from each pass to not cause an issue?
If you do find a bit like that, I would recommend doing a multitool pass where you take out most everything with a 1/4” or 3/8” bit first, then follow up with the fine bit to get the corners. As Eric said, that would be delicate and will require you to go very slow.
This is the longest 1/8 bit I could find:
https://www.mscdirect.com/product/details/48129795
Personally I’d use a chisel instead to square up the corners… A bit like this is very very likely to break easily, and at $70 each…
Thanks again Eric, I tend to agree with you. I was hopeful there would be a solution but I didn’t really think so. There could be many of these so reducing hand tool work was attractive but not a deal breaker.
On thing that might help with the hand work, is to use an 1/8” DRILL to pre-drill all those inside corners. At least then when you’re doing the final chiseling you have a target to aim for.
Obviously, do the drilling before the milling 
Interesting idea! I’ll give that a try. Thanks for the creative info.
Not sure I understand the workflow but I would not cut to a depth below the flutes.
OK, help me out here. I’m pretty new at this but I’ve been a woodworker for 40+. If I use a .25” cutter with a CL of 1.5” is it ok to cut 1.75” in multiple passes? I would think so and have done it lots(not on a cnc) Please educate me. I’m planning on a .25 upcut or compression and making 4 passes at .437”. I understand there will be a .25” of smooth shank below the surface. Will this be ok?
Is it a profile cut? You talked about using a .125 endmill previously.
Correct. It is a profile cut in 1.75 solid wood, kiln dried eastern white pine specifically. I figured the .125” endmill should probably be ruled out, so upped it to .25”.
If you just want to give it a try, titan has something for $16 - https://www.mscdirect.com/product/details/07259435?orderedAs=TC17008&pxno=31650598
Usual preface: I’m with PreciseBits, so while I try to only post general information take everything I say with the understanding that I have a bias.
Not really. You can get away with it if you babysit it. However, any tool that is the same diameter as shank size is actually slightly smaller than the shank (other than tools with “land"). This is because in order to grind the edge you have to take off some of the material. So you are functionally rubbing a smooth shank in a slot that is slightly smaller.
That said people do still do it when they have to. I’d be nearby and have a fire extinguisher just in case though. This is also the one case I can think of where having a lot of angular runout might actually help. As that would make the tool functionally “bigger” as you go towards the tip.
Keep in mind for the below that I’m speaking as someone that works for a company that makes these. We even have what you were originally asking for. But I wouldn’t recommend this unless there was no other way or you are removing the bulk of the material before using these kinds of cutters.
Generally speaking these kinds of tools are “high aspect ratio” tooling. Where the ratio of length of cut to diameter is high. They are not really ever meant for slotting/profiling or even bulk material removal as those are much higher stress to put on the tool than ideal. There is necked or reach tooling where the shank is “necked” back at the end of the cutting length to allow more strength but not rub. You can get away with more that way but it’s still an issue.
No matter how well designed you still have a fundamental issue with this kind of tooling and that’s deflection related to stickout (the amount of tool sticking out of the collet). It looks something like this.
The force required to deflect (bend) the tool 0.001" per stickout and shank size:
1/8” shank, 1/8” diameter, 0.25” LOC
2.5" - 0.2lbf
2.0" - 0.4lbf
1.5" - 0.9lbf
1.0" - 3.0lbf
0.8" - 5.7lbf
1/4" shank, 1/4" diameter, 0.50" LOC
2.5" - 3.1lbf
2.0" - 6.0lbf
1.5" - 13.6lbf
1.0" - 39.0lbf
1/2" shank, 1/2" diameter, 1" LOC
2.5" - 44.6lbf
2.0" - 77.9lbf
1.5" - 142.5lbf
Numbers pulled from Millalyzer (Link)
Hope that’s useful. Let me know if there’s something I can help with.
A regular item in our shop is playdough stamps. They are 1.5” circles that are cut out of 1.5” thick cherry and to maximize yield I use a .25” upcut bit. We cut 50+ a day out of each board. I have used both 1” CL and 1.25” CL with zero issues. This is running 0.25” depth of cut per pass and 200 ipm @ 16k rpm. You obviously cannot do a “final pass” but that doesn’t matter as long you’re ok sanding the machine marks after. The suggestion about using an .125 drill toolpath seems like a great idea to get those tight corners. Hope this helps!