Squealing noise when cutting tabs?

[hipstomp]

Hi everyone,

I'm cutting 3/4" plywood and 3/4" poplar and am getting a horrific squealing noise when cutting tabs and at corners. To be clear, the bit noise is normal until it gets to the tab, but as soon as it "bumps" up and down for the tab, or changes directions to cut a corner, the noise comes; it sounds like metal-on-metal to me, although I'm cutting wood.

I thought perhaps the collet was no good, but switched to a new collet and the problem persists.

Details of set-up:

- ShopBot Desktop
- Bit is 1/4" double-flute upcut spiral, Onsrud 52-910
- Have tried 7500 rpm @ 2 i.p.s. (chipload .008)
- Have tried 3750 rpm @ 1 i.p.s. (chipload .008)
- Have tried 5000 rpm @ 1 i.p.s. (chipload .006)
- Have tried 7000 rpm @ 1 i.p.s. (chipload .004)
- Have tried both 0.25 and 0.125 pass depth

Any advice greatly appreciated. Or if there are more details of my set-up I can provide, please let me know!

thanks,

- Nick

[bleeth]

When you are going around a corner or doing a tab the speed slows down and the sound changes.
You may want to adjust your ramp values. There is a very good article by Brady Watson on maximizing ramp values in his column on the main SB site.
Different values work better for different types of cutting. He goes into the various parameters for cutting out parts, doing 3-d, etc.

[scottp55]

Nick,
"ONSRUD 52-910 1/4" Solid Carbide Two Flute Upcut Extra Heavy Duty for Woods and Composite Woods"
Not quite sure what the "Extra Heavy Duty" implies for geometry and don't cut much Ply or any Poplar, but my 2 similar 2F .25" center cutting ups in hardwoods like higher rpm than yours. For a simple/long rectangular cut out with .5"R corners 20X5" for instance with 1/2D passes in Hard Maple one gives best finish at 1.6IPS,10K, and the other at 2.2,14K. Go figure.
Are you using 3D tabs and can you put a very small radius on corners? Helps quite a bit, as machine never has to come to a complete stop.
Agree with Dave that changing VR settings after reading Brady's article will probably help (need to start playing with that myself for small complex shapes and just getting into 3D), but still using default VR settings myself.
Don't like that"sounds like metal on metal". Can you post a vid?
Is bit dull or are there complex shapes involved? Are you getting good edge quality at those rpm's?

[garyb]

As the guys have noted above check your ramping but more so, rpm is your problem. The bit is overheating and is screaming feed me.
The 52-910 has an aggressive grind and needs to be fed, chiploads are recommended start points for a tool and need to be dialed in to suit your machine/spindle and especially the material being cut. I would expect your min to be 120ipm and 11500-12000 to be closer for you.
second point if your cutting plywood that would not be the recommend tool, the 60-100 series would be the recommendation.

I'm cutting 3/4" 9-ply birch, with a 60-123MC at 530ipm and 16500 in one pass. If I went by the recommended chipload I would be around 620ipm but due to the material density I've adjusted for the sweet spot that suits me.
Gary

[scottp55]

Gary,
What does Onsrud mean by "Heavy Duty" exactly?
Why would a person buy that for...fairly clean Hogging?
Not finding anything.
Thanks

[Ger21]

If you look in their catalog, they show a cross section of each tool. The heavy duty bits appear to be thicker in the center, with shallower flutes.

[garyb]

Gerry is correct, there is less material removed during grinding leaving a more rigid tool, hence the term heavy duty. You will also find the grind angle on that tool a little higher
Normally selected for profiling and pocketing, example; cutting a profile with an LP, in say hard hickory, the standard tool 52-200 series may have a tendency to flex and bounce off the material, while trying to maintain feedrates, (especially if your LP pass is taking less than .02), the heavy duty is designed to counter those issues and let you be more aggressive with your cutting.
Gary

[dlcw]

Like Dave and Gary said, this is pretty normal when using tabs. Your machine feed speed has to slow down to cut the tabs (and corners also), but the RPM's do not get lowered. Therefore you cutting at a much slower feedrate then the RPM's call for. This results in the screaming bit.

My machine is heavily tuned for cutting LOTs of plywood. I cut a single pass at 5ips at 12000RPM and my machine is pretty quite. When it gets to corners and tabs it screams "feed me" because the RPMs remain at 12K but the feed rate slows way down.

If the machine is not screaming on straightline cuts you are Ok on feeds and speeds. Go through the ramping document Brady did and see if you can tune your machine even more.

Each machine is different and will have a sweet spot when all the planets align. You just have to find yours.

[Davo]

Seem to experience that on 3d work, when it slows to make a lot of Z adjustments is squeals sometimes

[scottp55]

Thanks Gerry....and Gary for elucidating with the examples.
Davo, Brady also gives some examples for 3D work for VR settings.
http://www.shopbotblog.com/2008/03/a-ramping-the-vr-command-and-how-to-tune-your-tool-for-maximum-performance/

[Davo]

I think my brushes are going out - today my router became Thor's hammer and blue sparks took over the interior with popcorn noise

[hipstomp]

Thanks Bleeth, will look for the document.

- Nick

[hipstomp]

Nick,
"ONSRUD 52-910 1/4" Solid Carbide Two Flute Upcut Extra Heavy Duty for Woods and Composite Woods"
Not quite sure what the "Extra Heavy Duty" implies for geometry and don't cut much Ply or any Poplar, but my 2 similar 2F .25" center cutting ups in hardwoods like higher rpm than yours. For a simple/long rectangular cut out with .5"R corners 20X5" for instance with 1/2D passes in Hard Maple one gives best finish at 1.6IPS,10K, and the other at 2.2,14K. Go figure.
Are you using 3D tabs and can you put a very small radius on corners? Helps quite a bit, as machine never has to come to a complete stop.
Agree with Dave that changing VR settings after reading Brady's article will probably help (need to start playing with that myself for small complex shapes and just getting into 3D), but still using default VR settings myself.
Don't like that"sounds like metal on metal". Can you post a vid?
Is bit dull or are there complex shapes involved? Are you getting good edge quality at those rpm's?

Hi Scott, I am using 3D tabs. As for putting a radii on the corner, some of the cuts are simply straight lines, where the bit must stop at the end and pull upwards to remove itself. During those moments the screeching is horrific, which I can't figure, as the bit should be moving upwards through material it has already cut out.

The shapes are not too complex, but there are enough turns that I don't feel comfortable going faster than 1 to 2 i.p.s.

I don't *think* that the bit is dull, but the only way I have to check is to run my finger across the edge and compare it to a brand-new upcut ballnose I have. The sharpness feels similar on both and I do not see any burn marks.

Lastly, when I tried a few experiments upping the RPMs, I touched it after each cut and it was very hot, which I figured was a no-no.

Another problem I'm having with this bit is that the chips do not seem to evacuate. So if I'm cutting through 3/4" material in three passes of 0.25" each, by the time it gets to the third pass, the channel is quite clogged, the noise changes and the bit really sounds like it's laboring. I imagine it can't get through its own waste. During one instance of this, I hit the "stop" button too late and the part started to move.

Ought I try upping the RPMs again, even if the chipload then falls well outside of Onsrud's guidelines?

A more general question for all of you: How far outside the manufacturer's chipload guidelines are you willing to go? I wonder if I'm being too cautious, or overly concerned about how hot the bit was (hot enough that I couldn't keep my fingers on it).

thanks,

- Nick

[hipstomp]

As the guys have noted above check your ramping but more so, rpm is your problem. The bit is overheating and is screaming feed me.
The 52-910 has an aggressive grind and needs to be fed, chiploads are recommended start points for a tool and need to be dialed in to suit your machine/spindle and especially the material being cut. I would expect your min to be 120ipm and 11500-12000 to be closer for you.
second point if your cutting plywood that would not be the recommend tool, the 60-100 series would be the recommendation.

I'm cutting 3/4" 9-ply birch, with a 60-123MC at 530ipm and 16500 in one pass. If I went by the recommended chipload I would be around 620ipm but due to the material density I've adjusted for the sweet spot that suits me.
Gary


Hi Gary, thanks for this info. I should have read your post before asking the questions in the response I just left to Scott's post above. I'll look into the 60-100s, and will try further experiments with the feed rate and higher rpms.

Also, what are you using for holddown? Cutting 3/4" ply in one pass sounds like a dream to me and I'd love to be able to do so. I've been limiting myself to three passes of 0.25" each for fear of the part moving and it takes longer than I'd like.

- Nick

[bleeth]

Just noticed you are using an upcut. A compression or mortise compression is a better choice.

[garyb]

Nick
vacuum and t-track. for single pass you need to move up to at least 3/8 or 1/2" tooling,
If your cutting plywood quantity the 60-100MC (marathon) 2 flute series will give the better yield over the standard 60-100 series.

Dave the 60-100 series are compression tooling in single thru to four flute
Gary

[bleeth]

Referring to the 52 series bit Nick told us he was using.

[tomhartnett]

Checking ramp values is pretty accurate here. As well as making sure your IPS feed is high enough. Sounds like the bit is spinning against material and not cutting (by the description of the sound it makes). You might notice that the bit is warmer to the touch than usual if this is the case.

Another thing to note is a simple bit sharpness test. Lightly, lightly, run a flute of the bit along your fingernail at an angle, if it leaves a mark, it is sharp.

Best regards,

-Tom H.