Troubleshooting Breakage of Bits
CNC operators help a colleague figure out why his 1/4-inch bits keep breaking in 3/4-inch-thick hardwood. August 29, 2006
Why am I repeatedly breaking 1/4" carbide bits in 3/4" thick hardwoods on my Record 130 CNC? I am running a clockwise roughing pass with either a single 1/2" spiral compression or downcut bit, leaving 1/16" stock to be trimmed, and following up with a similar single finishing pass with a 1/4" spiral downcut. The feed and dropdown speeds are both 300 FPM. Is spiral upshear and lowered FPM the solution?
From contributor A:
Why are you using a 1/4 for the finishing pass? Can you use a larger diameter tool, say 3/8 or even stay with the 1/2? I break 1/4 tools all the time in 3/4 MDF. I'm going to 3/8 exclusively.
From contributor C:
It sounds like your part might be moving. If it is, you will be progressively cutting more material until your bit breaks. Slower feed on the .25 cutter, maybe 200 ipm, would help. Upshear cutter might have a tendency to lift your part, which would cause bit breakage.
I am sure you know, but to be safe, remember to adjust your rpm as you lower your feed speed.
From contributor D:
Maybe the diameter offset for the 1/4" bit is incorrect in the controller, causing the bit to get too close to the material. It's worth a look.
From contributor M:
I agree with the poster who asked why the small diameter tool. Regardless, you only need to remove enough stock to load the tool, say .025 to .03 for a small tool like that. For a good finish, I like to use 1/2" to 3/4" diameter 3 flute upshears for solids, depending on stock thickness. If you are spending the time to do the roughing pass with another tool, the finish tool will last a long time if you are only making a finish pass.
From contributor S:
I assume you need the 1/4" for an inside corner radius. We use 1/4" DS in solid wood a lot. It screams in the corners, but typically it works okay with similar feeds/speeds to yours. Therefore, I'd check hold down, collet flaws, vibration, etc.
From contributor M:
The reason your tools are breaking is because of the amount of engagement in material. I assume you are going the full 3/4" depth. You have 25% engagement, which causes more deflection than 50% engagement. I would try leaving between .010" - .025" for a cleanup pass - this will cause less deflection, thus reducing tool fatigue and ultimately less breakage.
From contributor O:
I had the same problem with 1/4 bits. I went through quite a lot on one job, until I tried a 1/4 bit with a 3/8 shank from Onsurd. I did not break one of these bits, where I broke over 50 of the 1/4 shank ones. Also, I thought that the upspiral would be the way to go to remove the waste material, but it did have a tendency to lift the board and cause chatter. I ended up with a down spiral and cut out the bottom of the holding jigs to allow the waste to fall out the bottom. I am not a big fan of second machining unless absolutely necessary. To me, it seems that by the time you did your second cut, you could have produced another part. If we did that on our last big job, that would have made the job go from six weeks to twelve, and I think we would have lost money at that rate. It is similar to slowing down the feed rate. There is a reason these machines can move so fast: production. It would be like buying a Porsche to drive through school zones.
From contributor G:
It seems everyone had some good input. Most 1/4 tools have a maximum cut length of 3/4". Tools that we (at Courmatt) have seen breaking the shanks are rubbing on the material, causing a non-cut edge to heat and break. Use a tool with a min 7/8" cut length. Your feed speeds should be around 200-250, taking off about 3mm (.125 " of material ). Taking a .062 trim pass will also heat up the tool, as the chips are smaller and the heat will stay on the tool. Also, as mentioned, if you do not have a new collet in the holder, you will also get breakage.