Troubleshooting Bit Breakage in Hardwood

Pros investigate a bit breakage problem. This time, it seems the downshear bit was packing chips into the work. June 17, 2009

I'm routing maple and oak solid wood with a 1/2" 3 flute down cut rougher (Onsrud/Festool) at 16,000RPM and 400inch/minute. At this feed the router bits are breaking. I have tried reducing the feed by half and increasing the RPM but occasionally it still breaks brand new bits. depth of cut is 7/8" or less. Fixturing is with both vacuum and steel pins to hold the parts in place. Based on the specs from the manufacturer I should be running at 18,000 RPM’s and between 700-1,200 inch/min. I realize that I'm already under-feeding it but I have no choice.

What am I missing here? Could this be an issue with the toolholder or spindle? I was forced to use a 3/4" rougher which I can get to the recommend feed with no breakage, but I would like to know why I'm getting the problem with 1/2" breaking. I change the collet every time the bit breaks to a new one. I use 1/2 compression router bits in melamine and never had bit breakage even at 2,000 inc/min feed.

Forum Responses
(CNC Forum)
From contributor J:
I'm no expert, but your feed should be about 720 IPM at 16,000 RPM. Maybe because of the low feed speed the bits are getting hot, and that's what really causing them to break. Have you tried running faster? I'm running all day long making a single pass, 1.25" deep cut into soft wood at 16,000 RPM and 500 IPM with a 1/2" two flute, finish bit.

From contributor K:
I first tried at 800inch/min 16,000 RPM and the bits were breaking like crazy. I'm getting chips not dust even at 400 but it breaks. I keep stepping down to avoid breaking.

From contributor J:
How much of the bit protrudes from the collet?

From the original questioner:
2-1/8" is the cutting length. Most of the material I cut is 1.375" - 1.875" thick.

From contributor J:
If the cut is only 7/8", then you might try a shorter bit with a C.L. of 1" or slightly more so less of it protrudes from the collet.

From contributor M:
I am a little unclear - are you on a spoilboard or pods here? If it's on pods, I haven't a lot to say, but if on a spoilboard, you are likely getting way too much heat packing the chip down against the spoilboard. A compression bit would help a lot in this regard.

From the original questioner:
No pods or spoil board only dedicated fixture.

From contributor J:
I don't understand why it would make any difference if was on pods or a spoilboard because his 7/8" deep cut is less than the board thickness of 1.375" - 1.875". If he is in fact making a complete cut through the board, then he would be hitting the pods if he had them. Also, I doubt the chip removal efficiency of a compression bit versus a downshear bit. It seems to me that the downshear portion of a compression bit would block the removal of the chips anyway. If he could switch to an upshear bit, then that's a different story.

From contributor T:
Are you torquing your toolholders to specification? Where are the bits breaking at, up on the shank by the collet or down in the flutes?

From contributor K:
They all break at the point where the shank ends and the cutting area begins. They never break by the collet. I think I will change to an upcut rougher instead of the down cut.

From contributor H:
All we cut is hardwood and softwood parts held with dedicated fixtures or pods. My first suggestion is to try a new collet if you haven't already done so. Proper torque setting for the nut is also important. Is your spindle an ISO30? If so, check the trueness of the taper fit. Make sure there it is tight and there is not vibration being generated from that component.

After checking that, I would look at your hold down fixture. Is it at all possible the part is vibrating as its being cut? If so, that is almost certainly the cause of your problem. We fight bit breakage as a regular problem. This is because we hold most of our curved hardwood parts on pods with rubber gaskets. This makes for a lot of part vibration of the part when cutting. We use HSS bits instead of carbide for several reasons, one of which it is less brittle then carbide.

We also cut at 150 to 300 IPM at 18,000 RPM. If we used a lower RPM or faster feed rate we would blow our parts off the pods. We typically get 35 to 40 mouldings out of a 3/8" downcut spiral bit with 15/16" to 1 1/8" thick hardwoods. This is whether we use HSS or carbide tooling.

From the original questioner:
I took a three flute 1/2" up cut rougher I and set the feed to 800in/min at 18,000rpm and it cut with no problems or breakage or part movement. I always change the collets after a tool break.

From the original questioner:
It sounds like your downcut bit was loading. You probably have little or no chip clearance below your parts. This would cause the flutes of your bit to become packed with chips and preventing proper chip flow. More problems would be seen in applications were the bit is buried doing cut out operations. I typically only recommend downcut tools in applications were the parts are setup on pods and there is a great deal of clearance below the part. You should always use upcut tools for spoilboard and limited clearance applications.

However, proper torque on the collet nut could still be a problem. If the nut is under or over tightened you risk the bit slipping in the collet. This applies even to new collets. If you have not already you should invest in a torque wrench for your toolholders. It is a small investment if you consider the cost of replacing 3/4" solid carbide bits. A torque wrench can be purchased for about the cost of 4 to 5 of the style bits you are using. Torque specifications will depend on the type of collets you use. Check with which ever tool supplier you buy your torque wrench from for the proper specifications.

From contributor J:
To the original questioner: was the bit that didn't break the same length as those that did?

From the original questioner:
1/8" shorter overall. But I think the up-cut is what made the difference.

From contributor B:
Been there done that. The downspiral bit has no place to put the chips. If you have to run a down shear bit you need to be up on a pod and cut all the way through. The chips add a load to the bit. Put your parts up on pods and run comp spirals and get some parts cut.