# "Climb Cutting" and Bit Rotation

A basic introduction to bit rotation, feed direction, and the meaning of left-handedness and right-handedness in CNC work, with some tips on controlling cutter rotation and feed direction. February 8, 2008

Question
Which way should the bit spin?

1- If (looking at the computer screen) I were to cut from the bottom middle to the top middle with my finished piece on the left, should my bit spin clockwise or counterclockwise?

2 - When cutting dados, should I cut with saw blade direction or against (like you would with a table saw)?

Feel free to correct my nomenclature.

Forum Responses
(CNC Forum)
From contributor G:
This would depend on the geometry of your cutter. All the cutters we use rotate clockwise. There are a few cutters out there such as Onsrud series (48-506) that are available when "left hand" rotation is required.

From the original questioner:
I guess I should have asked: Assuming a clockwise rotation with my finished piece on the left, should the bit travel up or down?

From contributor G:
Now that's a different question. Moving up would be a conventional cut and moving down would be a climb cut. I only use conventional cutting in our business (mostly plastics). For some wood projects, the climb cut will prevent a big chunk of wood from "blowing out" of your part. Sometimes conventional cutting will catch the wood grain in just the wrong way and a blow out will occur. The way I teach our new guys is to tell them that they are standing on top of the cutter. The finished work piece is on your left.

From Brian Personett, forum technical advisor:
A couple of things:
1. If your bit is directly underneath you and you're looking down on it, if it's turning clockwise, it's a RH rotation. If it's turning counterclockwise, it's a LH rotation.

2. If you imagine yourself behind your bit pushing it through the material, if the bit is to the left of the line, it's a LH offset; if it's to the right of the line, it's a RH offset.

3. If at the cutting edge or the front edge of the bit, it's pulling away from the work piece, it's called power cutting. If the cutting edge or the front edge of the bit is pushing into the material, it's called climb cutting. Both have their applications, depending on various factors, material, finish quality, tooling, etc.

4. Where saws are concerned, see item #3. I cut melamine 99.9% of the time, and I always climb cut or in your analogy, opposite of a table saw.

From the original questioner:
Thanks for the responses! I will be cutting mostly ¾” melamine and ¾” plywood, some laminated, some not. I’m looking for feed speeds, bit types/diameters, cut direction, and I’m sure more when I get into it.

From Brian Personett, forum technical advisor:
What we've covered in this thread should be covered in either your machine training or software training.

From my experience with melamine, most domestic board doesn't really care whether you climb cut or power cut. I prefer Canadian board with hardwood chips that really fuzzes if you climb cut. As a rule, I power cut. The fuzz can be an issue with .018 PVC.
With VC plywood, you're on your own. I've had really mixed results, depends a lot on the core - fir, poplar, import, etc.

As far as feed speeds and all that jazz, most of the players in the tooling business have guidelines listed on their websites. Or just ask them, they should be able to tell you. I machine a lot of 3/4 melamine and 3/4 plam on a PB core. I use a 3/8 compression bit, 16K RPM's at 12 MPM. I'd go faster, but that's as fast as my machine will go. I know guys who are cutting the same thing with smaller diameter bits as well. Talk to your tooling guy.

From contributor J:
What Brian calls "power cutting" I call conventional or chip cutting. I use whichever works better for whatever material I'm cutting. If you have a tool changer, here's a trick. To change from a power cut to climb cut (or visa-versa) just change the tool from a RH tool to a LH tool that spins opposite to the RH tool. In effect, that changes the direction of cut without actually changing the direction. But, something else to consider is if you perform mirror image processing on your machine (process parts at both ends), then one end is climb cutting and one end is chip cutting. This advice is subject to correction.

From contributor M:
Contributor J - great tip! That trick is deployed often by people who want to maintain the type (climb vs. conventional) of cut running in mirrored origins on machines that are capable of such. One word of caution - always run a left handed cutter in a left handed holder. The collet nut threads are manufactured in the hand of normal operation for the cutter. Loading a left handed cutter in a right handed holder is a highly unsafe practice that could result in the nut unthreading during operation!

From contributor A:
See picture for details.

Go to the Onsrud web site and read every bit of information contained under the "Onsrud cutter technology." This is the best place to read up on everything you will need to know about tooling.

From contributor J:
Contributor M, I almost always write parametric programs. In order to avoid the mirror image change in cut direction, my NC1000 programs have a statement similar to this one (Might be wrong, I wrote it from memory):

JP(61,5):4 ; TRUE MEANS AREA DX1 OR DX2 (BUTTON 4 PRESSED), JUMP TO :4
; IF FALSE THEN IT MEANS AREA SX1 OR SX2 (BUTTON 1 PRESSED), EXECUTE NEXT LINE

and then the program inserts the parameters for G41 or G42 tool comp. cuts.

P.S. That code avoids a tool change that adds ~7-10 seconds to each program.