How do you cut out 3/4" stock with small diameter cutters? Or don't you :)

[bking1836]

Hi everyone,

Looking for wisdom. I tried searching the forum, but I struggle with the search function being vastly over-inclusive unless the search terms are pretty unique and obvious.

I am trying to cut out some relatively complex vectors out of 3/4" stock (think profiles of a state or a lake). If the material size is large enough, it's not a problem to use a 1/4" cutter and maintain detail. At smaller sizes, though, I need a 1/8" cutter. Mine has a 1/2" cut length. I know Amana sells one with a 13/16" cut length, but I would worry about fragility and deflection.

Only thing I can think of is to break up the cut into two parts: first a rough profile cut out of an offset vector with a 1/4" cutter; and then slowly pocket out the rest with a smaller bit up to the actual vector profile. Would that work as long as the collet nut isn't in the way, because pocketing essentially reduces the cut depth with each pass?

Thanks!
Brian

[khaos]

You can get the longer 1/8" bits. I use the ones sold by dremel for this its ~1USD each for an 8 or 10 pack. When you make the cut you will have to work your feeds and speeds and cut depth to get your results. Slower and shallower cuts will stop the worst of the deflection once you get deeper in the work.

[Burkhardt]

I cut 3/4" all the time with 1/8" bits (fishtail preferred) and there are inexpensive carbide bits with 22mm flute length (1.5" OAL). They are a bit fragile but with 1/8" depth of cut I can run them with 2-3 ips feed rate depending on the wood species without breaking. Not super fast but O.K. Speed is typically 14krpm.
You can in principle cut with a shorter flute but the slot is deep and narrow and the longer spiral flute helps excavating the chips from the bottom. Prevents recutting and running hot.

[khaos]

If this is 3D you have other options that include the tapered 1/8 and smaller bits. http://www.talkshopbot.com/forum/attachment.php?attachmentid=31102&stc=1

[srwtlc]

Try a 5/32" or 5mm to get the extra length and a bit more strength. Run 3 (maybe 2 depending on the material and spindle or router) passes with an allowance around 0.018-0.020 on the edge and 0.030 left on the bottom. Then do a full depth pass right up to the profile with a little higher RPM and slower feed rate for a cleaner edge.

Centurion tools has them in up, down, and the 5mm in compression as well.

[chiloquinruss]

I use 1/8th all the time for 3/4 cabinet grade ply. Trick is multi passes. 1/8th bits will flex when pushed to hard or cut to much. The flex will cause loss of resolution in the piece and bad edges of the cuts. A good hold down helps too! Russ

[bking1836]

This is all helpful. Thank you! I see a variety of cheap options on Amazon. Would you recommend staying away from 1 flute bits?

[Brady Watson]

Avoid single flute tools at 1/8" diameter if you intend to cut deep.

As Scott eludes to, try something in between. Not sure why everybody forgets about 3/16" dia tools, but they are great for times when you need the tool to be stiff enough to avoid side-gouging (waterline stepdown marks) and small enough to get the detail. A 2-flute solid carbide end mill will work fine. If you want a fishtail you can get that too. They are especially trick when it comes to 3D when 1/4" doesn't resolve enough detail and 1/8" takes forever.

If you're stuck on it being .125" dia, you can get it up to 1.875" flute length, but you're gonna pay for it: Harvey Long Flute (http://www.harveytool.com/prod/Square-Miniature-End-Mills/Miniature-End-Mills/Browse-Our-Products_255/Miniature-End-Mills----Square-Long-Flute_52.aspx) Everything Harvey makes is excellent & lasts a really long time unless you abuse them.

Additionally, if your design 'breaks' at the right place, you may want to consider using 2pcs of 3/8" material or say 1/2" & 1/4" to make up your 3/4" total.

-B

[Walt_S]

I have the same issue as the OP. I've been searching for longer 1/8" bits myself. I have been using an 1/8" bit with a cut length of 1/2" with success but would really like something a little bit longer. I run it around 16000 at 2-3 IPS in cedar with good success. I use a spiral ramp. Takes awhile but the outcome is good. I might look at some 3/16" bits, but a lot of my templates are right on the edge when using an 1/8" bit. Yeah, I'm stingy, I hate to waste just another fraction of an inch of wood. :/

[evan]

Great success cutting 3/4 PreFinished ApplyPly with AMANA #46180-K (K indicates ceramic coating) run @ 12k rpm, 2.5 - 3" per sec. (depending on part geometry), 5 passes.