Which bit to cut 3.5" thick wood?

[jim shula]

I have several pcs of 4x6 (3.5" thick) wood to cut to a given shape. I have a 6" long, .5" diameter ball nose bit with 3.5" of cutting area which I have been using, but I should get another bit for a spare. This bit came with the used shopbot I bought, and in looking for another bit, the longest cutting area I can find is 3". I am cutting with a 3hp PC router.

Does the cutting area need to be as long as the material being cut?
Can anyone suggest a good source for long bits?
Should I be using an upward or downward spiral?
What speeds and feeds should I be using?
How deep should I go for each pass?
Should I get carbide, cobalt or high speed steel?

Thanks

Jim

[GeneMpls]

Should be .net on that website, Brady.

[Brady Watson]

Does the cutting area need to be as long as the material being cut? Not necessarily. You may get some burnishing, but full length flute is preferred.

Can anyone suggest a good source for long bits?
ObergBrothers.net - ask for Andy - 2-flute 1/2" end mill (or ball) @ 4" CEL, 6" OAL Solid carbide

Should I be using an upward or downward spiral? UP

What speeds and feeds should I be using? Slow & careful. Listen to the tool & adjust accordingly. She will tell you where she wants to be. Start at 1,0.5 and work your way up. You may want to start with a shorter bit to allow more aggressive cutting/roughing before switching over to the long one. Run a simulation in software & find out how deep the tool really needs to go.

How deep should I go for each pass? Start .125" deep per pass. Listen & adjust as needed.

Should I get carbide, cobalt or high speed steel? Solid Carbide


Tricky stuff, Jim. Don't be too casual about cutting this deep - it takes serious vigilance.

Gene - thanks for catching the typo. Fived, but I had to delete original...

-B

[dlcw]

I use a 1/2" three flute up-cut spiral for deep cuts. I regularly make chair and stool legs (and other thick pieces) at 2.5" to 4" in thickness and have used this particular bit with excellent luck. I've used it in hickory, alder, oak, cherry, walnut, maple, cedar and fir with very good results.

My pass depth is .375" for softer woods and .25" for harder woods. My speed is 4.5IPS with spindle running at 10,000 rpm.

The problem is I can't remember where I got it from. I've got to go back through my purchasing records and figure it out... I know it wasn't cheap. :eek:

The important thing I learned (don't ask how) is that your spindle HAS to be EXACTLY perpendicular, in both X and Y, to the table when cutting to these depths. Otherwise your cuts turn out to be slightly tapered instead of straight up and down. Not good for precision work....

[kubotaman]

Another resource you can investigate is Her-Saf. I have used their bits to cut 3.5 inches with excellent results. They will make you a longer spindle than what is on their site. I have one of theirs that is 5 inches long. I use their insert bits that are replaceable and I find them to be excellent and great to buy from. I cut .375 per pass without any problem what so ever. If you find that the sawdust starts to not be expelled from the cut you can make the depth in two toopaths which will give you the ability to clean out the cut with a vacuum the proceed with the second cut. That's a deep cut but it is quite possible.

[danhamm]

Pay lots of "Attention" to what Brady says up above. long bits flex and will walk out of your chuck "quickly" the higher the speeds the worse it gets.

[jim shula]

Thanks to everyone for the advice. I ordered and received this bit from MSC today:
http://www.mscdirect.com/ItemQuickViewModal?storeId=10054&catalogId=10001&langId=-1&itemId=2059314&searchterm=33068677

I tried it and stopped the machine after it ran about 10" of toolpath moving at 1.5 IPS, 18k rpms, .375 deep. It was chattering real bad leaving jagged edges on both sides of the kerf. Maybe that's because the wood is so wet? I wish I could find some identifying info on the bit that came with the used cnc machine 7 years ago. It works pretty well and it's a two flute upward spiral .5x6" ball nose bit with a cutting length of 3.5".

I have to cut 32 parts 5.5"x3.5"x46" from wet 4x6 PT lumber for a manufacturing customer of mine. I've cut 22 already with my old bit. A couple times the bit has pulled itself down out of the collet, but it always gives out an audible sign first, so now I keep my ears peeled and the emergency shut off switch nearby.

[Brady Watson]

Jim,
You want solid carbide for that job. Cobalt is meant for high temperatures and work hardened metals - and is not as stiff as carbide tooling - hence the end flopping all around. 2-flute solid carbide end mill is what you want. No coating necessary.

-B

[jim shula]

Thanks Brady. I'll look around for a carbide tomorrow.

[Burkhardt]

HTC has XXL end mills for reasonable money. Even made in US....

http://www.endmilldiscount.com/end-mill/htc-end-mills-770.asp