Cutting through thick wood

[phealey]

Hello,

I am relatively new to ShopBot and have a project at work that requires us to cut through 3"-4" thick pieces of oak. We have a PRSalpha unit, and are not sure what kind of bit would be the best choice to cut through wood this thick. If anyone on here has any suggestions about what would be the best way to go about this, it would be greatly appreciated.

Thank you,

Pat

[dana_swift]

In order to cut through 4" of wood you need about 4.5" of bit protruding below the collet. The bit will have a lot of torque on it trying to twist it out of the collet, so it needs to be firmly set with at least one inch in the collet. So the bit needs to be 5.5 or 6" long. If your wood is actually 3.5 inches thick at the deepest point, adjust the calculations accordingly. It will require a much more affordable and easier to find 5" bit.

There must be some air between the work and the collet, as collet collisions ruin collets. (You have spares in all sizes you use don't you?)

Given a 5.5" bit length with significant cutting forces happening down at the tip, the next problem is bit flexing. A quarter inch bit will flex so much it may break into oscillation and "chatter". So a 3/8, or 1/2" is a practical minimum thickness for the bit.

The longest 1/4" bit I own is 4" (I had those custom made) and that is for cutting foam and soft things with very low cut forces. So that pretty much means a 1/2" bit, and you will have to hunt around because a bit as long as 5", 6" are very uncommon.

If you need a custom bit, call the guys at CenturionTools.com I have had them make customs for me, like the 4" 1/4 diameter bits I spoke of earlier.

If 4" of bit are below the collet, and safe Z height is 4.5", the Z travel needs to be 4+4.5". Thats 8.5" of Z travel. Be sure your bot is set up to give you 8.5" between the collet and the table. That should be ok, but its worth checking with a measuring tape. The typical bot will have right at 8.5" between the collet and the table, but check to be sure it is set up right!

Hope that helps-

D

[phealey]

Thanks Dana, that helps me out a lot

[chiloquinruss]

I did a job awhile back and didn't have long enough bits. Fortunately only the face and edge were to be 'finished'. So I cut with what I had then did the final cuts on the big band saw. Lots more sanding than if I had the 'correct bits' as has been suggested but I did get the job done on time. Russ

[waynelocke]

Use the longest 1/2" straight bit that you have and cut as deeply as you can. Trim the remaining material with a bandsaw within a 1/16" or so of the line as Russ suggested, and then use a pilot bit on a router table for the final cleanup without much extra sanding. You can probably get a 3/" diameter 2" cutting length pilot bit. You can screw the material to the SB table through the waste.

[phealey]

Thanks everybody, I appreciate your help. I've never used a ShopBot to cut wood before, and I have another question.

Say I pick up a 6'' OAL bit to cut with, would there be any issues with the top part of the bit (the area above the flutes) rubbing on the wood while the tip of the bit is deep into the cut? or any other major issues I have to worry about?

Thanks in advance,

Pat

[dana_swift]

Pat- that is no problem at all. Deep cuts often go past the CEL depth of the bit. What happens is the chips get left in the cut unless your dust collector has a lot of suction. Sometimes I run a few inches behind the cut with a shopvac hose to pull out the chips, otherwise they are an obstacle for the next pass.

Leaving the chips in the cut just makes a rougher cut, but it will still work. I have done that a lot of times too!

Sounds like you are doing some interesting cutting! Glad to know I am not the only one using my shopbot for demanding applications.

Blaze forward, and dont fear the CEL as long is it is much greater than your pass depth. If the bit OAL is 6" and the CEL is something like 2", usually your pass depth will be no more than the bit radius 0.250. Lots of room for the flutes to pull out the chips and deposit them in the channel behind the bit.

If the chips are packed in the channel, things are going badly. That is when you need to stop the bot and clear the chips. If they just blow out with compressed air, or vacuum, then all is well.

D

[dana_swift]

Additional thought about pass depth when you are new to the tool and CNC. Start with no more than the radius of the bit. Later you will find you can go much more agressively, however in the meantime you will find out how to hold down with that much cutting force. Materials vary also, if you are working with osage orange, use extremely shallow pass depth, like you might use for a metal! That is one tough wood!

Oak should go great at .25 with a 1/2" bit. If you have any concern do the the long extended bit, try 0.125 to begin with. If the bit chatters any back off the cut depth NOT the feed rate.

Feed rates are determined by the rpm, # flutes, and chip thickness desired ONLY. The horsepower, material, and other loading factors like how far the bit is sticking out of the collet determine the pass depth. That cannot be predicted from any formula I know of. Experience! Start shallow, and increase until you have the first signs of trouble, then back off a little!

Too shallow just takes extra time, but doesn't hurt anything. Too deep can break things - like the wood you are trying to cut, or the bit.

Hope that helps-

D

[Burkhardt]

I ordered similar extra long carbide bits here (http://www.the-carbide-end-mill-store.com/m5/170-2500--1-2-square-end-mill-extra-long-htc-170-2500-2-flute-gp-30-uncoated.html)

HTC has a good selection of extra long and tremendously long (http://www.the-carbide-end-mill-store.com/m5/770-2507--1-2-square-end-mill-extra-extra-long-htc-770-2507-2-fl-gp-30-uncoated.html) bits (square and ball) at reasonable price.

[jerry_stanek]

I got some 5 inch long 1/4 bits with a 2 inch cutting from one of my suppliers Cleveland Tool and Cutter Inc

[rhfurniture]

Hi, We have done cutting shapes to 140mm deep. I had some 170mm x 16mm spirals made for it, which worked OK, but found that there was a lot of burning above the flute (and sharpening made it impossible). The best was to use replacement tip straight cutters where possible, as they keep diameter, and the cut is wider than the body and the shank. I found it best to bandsaw to rough shape and cut in 2mm increments from the outside in, as this allowed using more of the cut length (eg 30mm), and overcame the lack of safe Z isssues, as it could (with care) be programmed with the cutter always below the top surface of the work. It was fine provided you kept the collet at least 2mm above the work. You will definitely need a spindle for it. Have fun, but tread carefully. R.