Shrieking / Squealing noise during some cuts

232 mill - YouTube

^ towards the end

I did some searches and found a couple results, but can never tell if people are talking about the same noise or not.

Anyways, this is my first time cutting steel. It is 1018. It is a Bridgeport Series 1 Vari Speed. Using a brand new 4-flute Carbide 3/4" end mill, taking 0.5 axial and 0.15 depth of cut. Tried 0.003 IPT at 150 SFM at first, then lowered it to 0.0025 and eventually 0.002 IPT and it still squeals like a pig. I realize it's not the best tool path, so that can be optimized. My question is, is there something wrong with the mill like bearings / bushings / belt, or is it just normal chatter from being too aggressive?

Shes only singing in the corner. Redraw the arc a little larger or program with your next smallest cutter. The closer your cutter radius is to part radius, the more it gnna squeal.

Try using a corncob rougher first. Your chatter is what I would expect from a light mill like that with the quill extended that much. A narrower width of cut with a slightly higher feed might help. A smaller end mill would help with the chatter when the tool gets buried in the corner.

OK much appreciated. I was getting worried there a bit.

When doing a spiral cut to make the circular feature in the center, it would always chatter at the same spot - at the bottom and top. Cutting around the sides was smooth as butter.

When you say higher feed, do you also mean taking a bigger cut per tooth?

Yes, a bigger cut per tooth will load the spindle more. However .003 per tooth sounds plenty high for your mill. A smaller cutter should help though. I am a wimp and would probably run at .006 per rev or .0015 per tooth though with a 1/2" cutter. You can up your RPM with a smaller cutter though.

It really depends on how many parts and what you need for a cycle time.

My input is worth exactly what it costs (free) so take it for what it's worth.

What material is that?

1018 steel.

For sure. I was just making sure my mill wasn't worn out or needed bearings changed or something. I'll take it easier on the mill.

I am going to let others chime in here because the last time I ran mild steel was 30 years ago.

humanmilkfarm said:

When doing a spiral cut to make the circular feature in the center, it would always chatter at the same spot - at the bottom and top. Cutting around the sides was smooth as butter.

Click to expand...

That might be an indication that you need to adjust the gibs (or in worse case, recondition) for the machine axis tangent to "the bottom and top". Very similar, check the drive backlash on that axis, and try conventional cutting rather than climb cutting (i.e., change the direction of the spiral rotation so the cutter edges face into the feed direction).

OK both X and Y gibs were loose. An annoyance with adjusting these on this CNC is that you I can't hand feel the tightness with a handle, but I tightened the screw down to what felt reasonable, and they still move.

It's on a ball screw, so I don't think there's any backlash adjustment. But I will try conventional cutting this weekend. Thanks!

I'd suggest staying no larger than 1/2" on your endmills when using a knee mill for steel cutting, four flute vari-mill types are best IMO. Program for more depth, less width of cut. If possible always have the cutter produce an arc when internal cuts are needed, not a right angle (don't "bury" the cutter).

Smaller cutter, more RPM, higher feed rate. I'd be tempted to try a quality 3/8" endmill, and punch up speed and feed. Make sure chips aren't allowed to pile up in any pockets or slots.

Keep the endmill as far up in the collet as possible for rigidity. For the same, keep the knee as high as you can, reduce quill stickout to minimum. If I was really limited on stiffness, I'd program roughing moves with the quill all the way up, and the knee setting my depth. Obviously program so all rapids are off the part, can't traverse through features unless you like bang/crack noises and enjoy cursing.

Your video shows the quill sticking out much further than ideal, and the wave marks on the floor of your cut areas shows the flexing of the spindle causing the tool to wallow about. Save the large endmills for light finishing cuts when you want to avoid depth blend lines, but don't rough with them.

And if those are DA style tool holders, try to get some TG versions for milling cutters. DA is acceptable for drills only in my book (and not really for them either). For roughing, you might be better off with the shortest solid tool holders you can find. When the mill doesn't have rigidity you need to maximize it at the cutter.