I’ve started downcut endmills for the first time because I was getting a lot of tearout with uncut endmills.
Strangely, the first time it was really “squealing” as far as I could tell. I’ve read mixed info on it being too little vs too much feedrate or too deep.
I went to make a video and miraculously the bit sounded good! It confused me but I was happy. See video here
About a month later, I made another cut with the exact same bit and got the squealing again… video here.
Any idea what may be going on here? I feel like I’m going crazy
So the material is actually the exact same. It actually may be the same piece, funny enough. I got distracted and didn’t end up cutting the second side for like 3 weeks.
In both cases I had the piece glued down painters tape and super glue. I can certainly try clamping down a piece but I’d need to set up a new program for that.
In both cases the surface finish was great. But when it squeals so loud it worries me!
I would assume it was the resonance of the bit thru the wood, ASSUME, ASS of You and Me. I do notice the difference between painters tape and clamps.
You can increase the feed or decrease the feed to see if it makes a difference.
Bits that have lost their edge will sound strange.
Chase all sources of vibrations (that you can do something about): workholding matters a lot, but so does reducing stickout, making sure the tool is not dull, using feeds and speeds such that the tool does not rub,…
And specifically for downcut endmills: make sure you have excellent chip évacuation and limit depth per pass to lower values than for upcut endmills: downcut tend to push chips downward, with no place to go: they can get packed and recut, and that’s a source of vibration. When in doubt, cut shallower.
The material and the grain in the wood has a lot to do with the cut too. I heard a change in sound when the bit passed from the sap wood to the harder wood grain. This and all the other suggestions above can cause the problems. You also have the grain in different directions (cup up in one and cup down in the other.) This causes changes in sound, cut and vibrations. The bit can also try to follow the grain when going with the grain direction and depending on how the bit is set in the collet it will flex and make the sounds you hear.
And slower feed speeds. You can always set the cut up slow and bump it up in CM and see what the changes make. Router speed can also be changed.
You didn’t say what the bit brand and number the bit can have a lot to do with this also.
I have a 60 degree down cut vee bit. That bit makes a lot of noise especially when it turns a corner while cutting. I think part of the reason for down cut to make more noise is the tool engagement. The bit is pushing the chips down and pulling into the work. The up cut bits try to pull the work up and poorly secured projects can become dislodged. The down cut bits tend to push the work down. You still need to secure your projects but the down cut would be less likely to just pull a thin piece up and out of cam type clamps. I also use the #251 more than I used to. Partly because of the chip out on the top side is less with the #251 down cut but overall finish is better at the bottom over a #201.
Adjust my depth and feeds and speeds to be much more conservative as a new tool in Fusion
Use the new F&S for my first side but forget to apply it for the second side
When I looked at my second side in Fusion it was still set to the upcut bit. Whoops…
For future posterity, a decent F&S for slotting seemed to be something like 18000RPM, 107 in/min with 0.25in WOC and 0.048in DOC. Apparently these settings should only be 50% of the max machine force (18lbf) and 55% of the max power available (800W spindle). Of course, the calculation doesn’t consider downcut vs upcut bit.
I did another cut today and used my more conservative depth. I found that when going against the grain it was a good feedrate but when going with the grain or in circles (i.e. adaptive or slotting a circle) I could go to 160% feedrate. Pretty cool!
What’s a bit confusing to me here is that I am using a very small percent of the capacity of the machine with these low depths. Supposedly the feeds & speeds calculators imply that I should be able to cut deeper without issue, but they ultimately don’t take into account chatter.
I know Millalyzer supposedly has a dynamics package, although it’s unclear to me if it actually works or not…
Is there any other reference when considering downcut vs upcut vs compression when calculating feeds and speeds? It would seem like that is a pretty big missing piece of the current feeds & speeds calculator spreadsheets that have circulated around originally made by NYC CNC. Thoughts?
