Poor cut quality on solid birch wood

[mmak2916]

I'm cutting some pieces on solid 3/4" birch wood. I've done numerous tests with the feeds/speeds and a climb/conventional cutting, however the cut quality is just not that great. There's chips and coarseness/fibrous shavings left on the side. When the bit reaches the corners, there's a screaming/screeching noise which is very high pitch and irritating.

Here are my cut settings:
Onsrud 57-910 1/4" downcut bit
10,000RPM
4IPS
7 passes at around 0.117 depth per pass
Climb cutting

Attached are the photos of the piece. The overall size of the piece is around 1.4"x3.5".

I'm still a newbie to the CNC world, would appreciate the help. Thanks!

[Kyle Stapleton]

You are cutting way too fast for a part that size.
Try 1ips. or slower

[David Iannone]

yeah, cutting too fast.
Take a small sample piece of the wood. Cover the smoothest side with transfer tape. I like "Conform" brand. Squeegee it down.
Then take some double sided adhesive tape (like banner hem tape) cover a piece of coroplast with it then squeegee it down.
Then apply wood with application tape to the sticky side of the tape you applied to the coro. Use roller or laminator to smash the two together.

When you cut on the machine, cut through the wood by about .1

The transfer tape will hold to the sticky tape and the small letters should not move and cause chatter. the transfer tape will come right off the wood and make it easy to pull out. Also you can walk away from the machine and let it cut letters without worrying about them jumping around after the cut.

Harbor Sales sells all these products.

Dave

[mmak2916]

Hi Kyle, I just made a cut with 1IPS. The cut quality of the sides came out better but there were more chipouts than before in the same area as pointed in the photos. Any other thoughts?

[David Iannone]

try .7 inch per sec and increase stepdown to .25" or maybe even .376"

After your cut out is made, you could go back with a profile pass just barely taking off any material. But you got to have them held down securely.

Dave

[gc3]

bump up the spindle to 12-13k try a spiral ramp

welcome to the world of solid wood machining...

[scottp55]

Try 1.6,.5,10.5K with .125" passes/spiral ramp/last pass .001/ conventional cut.
IF possible, change design from a sharp angle where tearing out to even the very smallest of radius. Also if possible, flip wood 90 degrees so the tearout section isn't unsupported endgrain.
Never cut Birch, so I may be talking through my hat:)
Bit squeals at corners because the machine slows down for corners just like you do in a car, VR(Virtual Ramping NOT ramping like in a profile toolpath setting) and it's "Hungry".
Doubt if it was ever getting near 4IPS on a small part like that anyways because of VR.
If my settings are still "Noisy" reduce RPM slowly while listening to bit. Some woods are "Picky" and even 500 RPM can make a huge difference. Got one wood that likes 9K for RPM. Go figure:)
Hope this helps.
scott

[Brady Watson]

Some woods, regardless of what you do, will cut like crapola. Birch and maple come to mind - and it has to do with the way the grain runs through the piece more than anything.

You can sometimes get good results by using allowance (say .02") and a climb cut stepping down say .125" per pass with a ramped plunge. Leave a .05" onion skin on the bottom. Then come back, FULL DEPTH in one pass, @ zero allowance using a Conventional strategy. You can try Climbing it with no allowance @ .125" pass depth, but you will most likely get climb marks.

Climb - does just that...It climbs on the material and pushes the wood fibers IN rather than yanking them out.

-B

[mmak2916]

Thanks for all the great suggestions/advice! After more tests per your suggestions, I think I came upon a happy medium in terms of noise and cut quality. A lot cleaner edges and fewer/smaller chips.

Feed: 1 IPS
Plunge: 0.5 IPS
7200RPM
.125" passes/spiral ramp/last pass is .001
Climb cut

Thanks for all the help, much appreciated!

[Brady Watson]

Keep in mind you are out of the torque range for your spindle @ 7200 RPM. You can get the same results by doubling both the spindle speed and XY move speed. So...Run 14,500 RPM at 2" per second XY. You'll cut the same exact size chip (chipload).

-B

[mmak2916]

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.

[gc3]

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.

shop/machine environment...it is what it is...invite you to visit our shop during routine production day...noise...the sound of money being made

cnc makes noise...a lot of noise especially with solid woods...try cutting Cumaru, Tzalam stock...

13K seems to be sweet spot for these kind of materials

[scottp55]

Start at Brady's settings, and do the same exact thing you just did at 1 IPS but reach around to VFD without looking at the readout and gradually lower RPM until she quiets down and cuts nice. THEN look at the readout and enter that RPM into the toolpath under edit bit. 1/4 Downs are still my noisiest bits and have to be tweaked the most.

[Burkhardt]

Looks like most of the trouble is when the cutting edge of the bit "brushes against the grain" in the areas where the cut direction is at an acute angle to the grain direction. As mentioned earlier, this is difficult to avoid.

It can be done, if you don't make the cut in one loop but segment the outline and switch between climb and conventional as appropriate for the attack angle.

But that is admittedly a bit complicated and will at least double your machine time. Some segments would be quite short.

[dlcw]

I've had pretty good luck cutting birch. Make sure the bit is RAZOR sharp. Factory new, not resharpened. With the feeds and speeds being recommended, you should be able to get pretty good results.

[bobmoore]

Kar; I would try getting rid of the down cut bit and try a straight bit or a low helix upcut bit. Run the rough cut at the settings you listed but maybe slow the feed down to 3 ips with a .010" offset allowance and leave about a .025 onion skin. Finish with a conventional cut at 0 offset 1 pass full depth.
Bob

[garyb]

Kar as Bob suggested change your tooling
the 57-910 is not the tool for that job. Its the extreme heavy duty standard tool which has a very aggressive grind and not suited for finish cuts in hardwoods like birch, maple etc.
I would suggest you change to a chipbreaker/finisher 60-300 series bdp015 if you need 1/4" or the 60-200 series 3 flute low helix finsher.
Those tools will give you a far better results than what your achieving.
Gary

[mmak2916]

Brady, what does it mean by "out of the torque range for your spindle @ 7200 RPM"? What are the consequences and outcome if I continue to use this setting? Thanks!

[mmak2916]

Update

I tried 14000RPM at 2IPS using the same settings I used to make the clean cut. However, I'm back to round 1, the chips appears to be more and the sides are not cutting as clean. It worked the best at 7200RPM but it was said to be "out of torque range for the spindle"

[Brady Watson]

You go with the settings that YOU want to run on YOUR tool. I just mentioned that the RPM you are running is below the spindle's constant torque power band. It does best (has full horsepower on tap) at 12,000-18,000 RPM. It is a wood router and not a milling machine...the spindle was wound for high RPM power, not low RPM torque.

It is possible that the spindle can hit a hard spot (like a knot) and bog down when it is running at such a low RPM, causing the steppers to either work harder or even stall - and you lose position - scrapping your part. You should at the very least be aware of this possibility. Otherwise you may be lead to believe that there is something wrong with your machine.

Also, several well seasoned machinists have chimed in on your problem and recommended different tooling. I would consider that part of your solution to hairy/chipped parts. The right tooling geometry makes all the difference in the world - and cheap tooling should be avoided. Good tooling goes the distance and cuts better.

-B

[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!