O/T Router Bits For Wood

[mowens]

I come from a metal machining background, so I need some help. We have been using Onsrud router bits to cut hardwood molding for aircraft interiors. These bits are fairly expensive as router bits go, the catalogue says they're for wood, but we are not having good luck with them. They dull quickly and don't leave a good finish. Does anyone have any suggestions for a good hardwood router bit? Thanks for any help.

[Colin Gilchrist]

Go with a diamond coating. What size of bits are you using? Try Carolina Speciality Tools or Diamond Tool Coating (this is a coating service and you would have to send them your bits).

 

HTH,

 

Colin Gilchrist

The Boeing Company

MR2 and Beta test site

[mowens]

We have (or used to) pcd bits in several sizes, but our moron 3rd shift operator is, shall we say, clumsy and has broken or chipped most of them. We use mostly 3/8 and 1/2 inch solid carbide. I'm thinking the problem we're having is not so much the bit but the feeds and speeds. It's hard to convince the operator not to run everything slow.

[Josh Kinney -Elite Engineering]

What Onsrud bit are you using?

Feeds, speeds, depths, etc..

[mowens]

Onsrud 57-395 3/4" dia.

Programmed feed rate was 250 at 21000 rpm, and I think that feedrate was too slow. However, I found out that the operator edited it down to 90 IPM. That's why I think it's a feed and speed issue. He just burned it up.

[Josh Kinney -Elite Engineering]

depending on the depth, tool length and machine rigidity I would say anywhere from 200IPM to 400IPM would be OK. does indeed sound like the slow feedrate overheated the bit and scorched it.

 

I've done 400IPM in Aluminum at 0.200" depth, 3/8" single flute with no coolant...

[Josh Kinney -Elite Engineering]

I would try the Onsrud 63-625.

 

It's for aluminum but I think you'll be suprised!

[Westgate Hardwoods]

How thick is the material that you are cutting? How many passes to you make?

 

We use FSTool bits. I would stay with the down spiral, but you might want to go to a 3 flute for better finish. Josh is right about the speed. If you go too slow you will dull the bit from excess heat build-up. I would suggest several depth cuts to get to the final depth and then a finish pass to take off the last 1/32". I have also found that when cutting solid woods, climb cutting reduces chip-out and produces a smoother finish.

 

I would also turn down the rpm to about 18,000 at around 200-300ipm.

[mowens]

We ran 250-300 IPM at 18000 rpm and that worked well. We are cutting hardwood about an inch thick, but we are only going about .2 deep per pass. The part has a thin wall with a radius on top, so we are taking shallow depths of cut and melting it down like I've done on high speed aluminum parts. So far so good, thanks for all the help.

-

-

You are right, climb cutting does reduce chip-out; We found that out the hard way. Same thing if you are cutting solid surface.

[mowens]

We have been using the pcd (pollychrystalline diamond) bits from Onsrud a lot the last few days. They are far and away better than any other bit we've used, including solid carbide. Also, they seem to run forever, if you can keep from chipping or breaking them. We have run them in wood, fiberglass, aluminum and solid surface successfully. If you can get passed the initial investment ($300-$450 a piece), I think they are well worth it.