Poor cut quality on solid birch wood

[Ajcoholic]

Brady, the trouble I was having with higher RPMs is that it makes this ear-piercing screeching/screaming noise. Wish there was a way to get rid of that noise on higher RPM settings.

There is... move faster, as Brady suggested. That squeal is due to going to slow and/or turning too fast. So slow down the RPM, or move faster.

OR - drop a flute (ie, go from a two flute to a single flute)

I typically run solid wood (all species of hardwoods, but a lot of hard maple) at 3 IPS and 10,000 with a 1/4" spiral bit as my default. For 3/4" stock I'd do two passes, perhaps three max but if you really want to get a clean edge then run a few passes in climb mode, leave about 1/32" at the bottom and then go back and do a full cut through pass in conventional cut.

Then fine tune the speeds and rpm to suit. With small pcs, you cant really go faster than a certain speed due to the ramp time, and the fact the machine is constantly accelerating and slowing down to change direction.

That works best for me, and was advice I was given here when I started.

I always do my first pass(es) in climb, leave a bit of material left and then do a full final pass in conventional cut direction.

Make sure your bit can cut the full thickness though, but most of my 1/4" bits have a 7/8" length of cut.

The reason this works in that when climb cutting, the bit wants to ride up, and away from the line of cut (the small amount of slop in the drive allows some movement) while in conventional cutting the bit is pulled into the cut. You can see the small step in the waste portion of your material after you cut this way.

[jerry_stanek]

A screaming bit is a hunger bit needs to feed faster or slow the rpms down

[mmak2916]

Just thought I'd give you guys an update. I spoke to a tech at Onsrud to get a recommendation on a bit for what I'm doing and they recommended the 60-111MW (Single Flute Compression Spiral). So I tested the bit today per the suggested RPM and IPM that was provided to me over the phone for the best chipload.

I did three tests with these settings (refer to photos below):

A) 10,000 RPM / 150 IPM @0.175” per pass, spiral ramp
B) 8,000 RPM / 120 IPM @0.175” per pass, spiral ramp
C) 10,000 RPM / 150 IPM @0.25” per pass, spiral ramp

They suggested to run this bit at 6000RPM at 90 IPM, but I swayed away from that because it was at such a low RPM speed and people here were saying that it's out of the Desktop's torque range. Is it safe to run at 6000RPM? I don't want to damage my machine.

The cut 'sounds' a little bogged down with the 8K and 10K RPM, like the feed is faster than the spindle. Is it much to worry about?

The cut quality around the flat sides are fine and the top and bottom of the piece is cleaner than the 57-910 but the culprit still lies in that particular acute angle. I feel like I'm trying to achieve the impossible here.

I may just modify my design...

Thanks for all the help so far!

[srwtlc]

Kar,

A couple of things you can try with your design/toolpath. At each of those corners, try giving it a slight radius instead of a sharp point and also, under the corners tab in the toolpath form, uncheck 'Sharp Corners'. Another thing to think about, would be to try a 0.375" compression bit. You'll get less vibration/noise and a cleaner cut than with 0.25" bit

[srwtlc]

At 0.175 per pass, depending on the specs for the bit, you may only be using the upcut portion of the bit. Forget the spiral ramp and try a smooth ramp of 0.375 - 0.5 at 0.25 - 0.375 per pass with 0.02 allowance. Follow that up with a full depth/full profile pass at slower feed and higher RPM.

[adrianm]

You may need to adjust your ramping settings. I use a very different set when I'm cutting small detailed parts compared to cabinet sides for example.

Not sure if it's such a big difference on a desktop but it does on my 8x4.

[cnc_works]

I have done a couple of things to relieve problems like this.

1. Peck drill (very conservative stepdown) a hole right at the cusp of the chipped out edge so there is less to grab and chip as it comes around the corner then run your regular toolpath.

2. Cut your regular toolpath leaving maybe .05" cleanup and clean it up with two separate toolpaths, one conventional cut for the non problematic half, then another climb cut to deal with the chip out prone side. Maybe include a little bit of overlap top and bottom for blending or it looks to be pretty easy to hit top and bottom with a touch to the sander, wouldn't take more than a couple of seconds.

Good luck!