Feed Speeds and RPMs for Cuts in Thick Hardwood
Adjusting bit speed and travel may help reduce a screaming sound that happens when machining solid wood on a CNC router. November 26, 2007
Question
We are cutting 2” thick birch hardwood. The tool we are using is a 4" tool 1/2" diameter with a 2 1/4" cutting length. We are cutting into the wood 1/2" at a time and running the bit at 18,000 RPM at 200 inches per minute.
We are getting a very loud screaming noise from the bit. We were told to put a blank bit above the 4" bit to “fill in” the rest of the collate. We did this and it seemed to help a little, but we are still getting the loud scream. Do you have any suggestions on ways we might eliminate this noise? Or is this just expected when cutting thicker hardwood?
Forum Responses
(CNC Forum)
From contributor M:
Birch and other hardwoods can be fairly loud to cut. Slowing down the rpm's will help. Bigger diameter cutters will also help. When cutting, if there is material on both sides of the tool, or if the cut is wider than the radius of the tool, the noise will be the loudest. You can take multiple roughing passes to quiet the operation down, but this will also increase the cycle time. Keep in mind that the noise can also be related to excessive heat and vibration, which will shorten bit life tremendously.
From the original questioner:
Thanks. We are already doing the multiple roughing passes, if you mean instead of cutting the full 2" at one pass, doing it in 3 passes. Would even more passes be better yet? There is material on both sides of the bit. I will try slowing down the rpm's. What would be good to try? 15,000?
From contributor D:
Chip load is what you need to know, to find the correct speeds. Feed/rpm/number of flutes. I usually aim for about .026 to get best cut and life from the tool. You never mentioned how many flutes were on the tool in question. Either way, you are cutting too slow.
From contributor R:
I think that some of the noise is the resonance in the hollow space between the walls of the cut, if you have wood on both sides of the cut. If you can avoid this by roughing out the shape on the bandsaw so that you are trimming less than the 1/2" bit diameter, it would help. If I am doing a lot of identical pieces, I like to make a dedicated, gasketed fixture and use a template to rough-cut parts first. If this is not possible, try using 1/4" cut levels (4), leaving .06" for a final cleanup pass at full depth. The final pass can run faster - about 300 ipm. The first passes usually leave small step marks, so the final pass is just if you want to remove these. Of course, this extra cutting takes more time, but these are being cut faster and more accurately than you could do otherwise, so it is relative. A lot of people get over-concerned with cycle speed, when accuracy and dependability are just as important.
From contributor M:
With the roughing, I wasn't talking about depth. I was referring to leaving some stock per pass so that you don't have wood on both sides of the tool. For a 2 inch piece of birch, I'd make my last cut full depth, removing only about 0.03" for a cleanup pass. That way you don't see 2 lines where you made three passes in depth.
From contributor O:
We cut a lot of 1 3\4" thick hardwood - maple, ash, walnut, mahogany. We run at about 200ipm at 12,000rpm, 3 passes with the 3 flute rougher, final .015 with the 3 flute finisher. Slot cutting will always scream some. Having a sharp rougher is key to having it run quieter.
From contributor T:
Many of our clients have similar applications, and without the extreme noise. It sounds like you are running the tool a little too fast and at too high an RPM. Try slowing both down (it wouldn't hurt to ask your tooling supplier for their input), and this should reduce the noise.
From the original questioner:
Thanks for all the input so far - it is very helpful. I spoke with our tool manufacturer. They recommended a 4" long 2 flute upcut rougher with a 2 1/8" cutting edge, running at 16,000 RPM and 660 inches per minute, leaving a .060 around the outside and then coming in with a finisher bit to get the remaining .060. We have never used upcut bits because I never want to chip the top surface. Would that .060, in your opinion, give me plenty of leeway so as not to chip into the finished product?
From contributor O:
They've also told me to run at 400-600ipm. Tried it and didn't like the results. Maybe it's me and my machine.
From contributor T:
I believe that most of our clients are only running 95-100 IPM in this heavy of a material, and removing the same amount. They were cutting at the higher feeds at one time, but they were getting lots of noise and cupping on the material. If you want to stay at the higher speeds and feeds, try reducing the depth of cut to .25 inches and see if that helps.
From the original questioner:
By cupping, do you mean that the edge of the material wasn't a straight 90 degree cut?
From contributor T:
It created a scalloped (cupping) edge along the length of the cut.
