High pitch noise - normal?

[Shane]

My Shopbot seems to be making a very annoying high pitch sound when cutting. It has nearly always make this sound since I purchased it. Just trying to find out if this is normal?

Here is a video I took where you can hear the high pitch sound. http://youtu.be/BQ68eVNVuAE

It pretty much only makes it when changing angles or directions when cutting. Sometimes the high pitch will not be apparent when cutting other times it is really loud. I've tried changing bits and brands from Onsrud to Whiteside. Doesn't seem to make a difference. But I've noticed when using 1/8th bits the noise isn't noticeable or gone all together.

I use solid carbide two flute downcut bits. I've varied the rpm's from 10500 through to 13500. Speeds from 40mm/sec to 80mm/sec.

The spindle is HSD 2.2HP 220V 1PH BUDDY 24V On Board Spindle.

Could the bearings be on the way out? I only ask as it is written on the Invoice that the bearings are not warranted.

Shane.

[adrianm]

That's the noise a spiral cutter makes when it's not cutting at it's optimum speed. The fact that it's doing it only when cutting corners or otherwise slowing down shows that you've got the feedrate about right.

There's not a lot you can do about it as it the feedrate has to slow for the corners etc so you drop out of the sweet spot.

If it was doing it on straight runs then you would need to increase the feedrate or slow the RPM.

As a wise person here once said (can't remember exactly who) a screaming bit is a hungry bit and needs feeding.

Bottom line is that's it absolutely nothing to worry about.

[jTr]

You may find it handy / revealing to adjust move speed on the fly, if you haven't tried it yet. Hit <SHIFT> and arrow key < to slow > to speed up. SB control will adjust in .10 increments for each keystroke. Since learning about that here, it's helped me to dial in proper feed rates. For any given project, the ideal RPM/Feed speed may need on the fly adjustment as you use different materials/wood species.

jeff

[shilala]

I dial in around 10K rpm and 2.5-3.0ips for 1/8 and 1/4 bits.
I cut a depth of 1/2 the diameter of the bit or a little more depending on the material. Below a wood hardness of around 900 I'll mildly cut deeper passes if I'm feeling brave. I never get any screeching at those speeds/feeds. That's fortunate, because I can't stand it even with my earplugs.

You're running at 1.5-3.0ips at 10k to 13.5krpm which would seem real close to where I am, but if you're at 13.5K rpm and 40mm/sec, that's a LONG way from where I run screech-free. That's high rpm and low feed speed to me.

I got to my sweet spot by checking the chip load calculator for my bits, then tweaking the speed down and feed up until the screech was gone. I was told my bits should not be hot when they are done cutting, which helped tremendously. I was also told a screeching bit was a hungry bit like Adrian mentioned. Those two pieces of information were gold nuggets.

[gene]

Its screaming FEED ME ! I cut with a two flute cutter 3/4" plywood single pass 12000 rpm at 5 ips. it only screams when it slows for corner turns.

[Ajcoholic]

I just cut some 1/2" Baltic Birch in one pass with a single flute compression spiral - almost no noise whatsoever! I usually use a 2 flute, at 11,000 and about 360 IPS and it works pretty well too.

If you can't move fast enough, you can try and dial down the rpm somewhat.

[gpinard]

Thanks guys, I have been watching the forum for while now. seem to be learning things faster than my questions are coming. this thread would be a perfect example of that. Have done several small projects in the few months I have had my desktop. Had observed the noise coming from the bit, but it had not been objectionable so I had not thought much about it. The chip load subject is something I have yet to learn about. Also adjustment of a cut file at the control computer is an area I have not studied yet. Lots to learn, and forum provides a steady stream of gold nuggets :)

[Shane]

Thank you for all the replies. Here is what Shopbot Support said about the issue..


This sounds fairly normal for a 1/4" bit. You could quiet some operations using a 1/2" bit where appropriate.

That said, here are a some things to double-check to optimize you tool that might help quiet it.

Make sure that the collet is snapped into the collet nut before placing it in the spindle. Also be sure to knock out any dust buildup whenever you've changing bits.

You might experiment with different chip loads. Work within the guidelines provided by the help page to see if perhaps a higher chipload might quiet it down. Currently you're toward the lower end for most materials.

Finally have a look at the ramping values on your machine. This link describes the ramping feature well.
http://www.shopbotblog.com/index.php/2008/03/a-ramping-the-vr-command-and-how-to-tune-your-tool-for-maximum-performance/

I guess the positive side of things is that at least my spindle isn't an issue. I have changed from 10500-13500 RPM. I might drop the rpm back down and see how that goes. I find that running it above 60mm/sec I don't get as smooth as finish.

I will look into changing the ramp values as it the high pitch seems mainly when coming into corners etc.

Shane.

[Brady Watson]

In VR, change your slow corner speed to 40. That should provide some cushion @ direction changes. The 'squeak' you hear in the corners/direction changes is cutter deflection.

Don't be afraid to turn the RPM up when you find your cut quality degrading around 60mm/sec. As long as you are not burning, I wouldn't worry too much about 'ideal chiploads'. If you were a production shop doing 40 sheets a day, that would be different. Quality of cut is king.

-B

[shilala]

In VR, change your slow corner speed to 40. That should provide some cushion @ direction changes. The 'squeak' you hear in the corners/direction changes is cutter deflection.

Don't be afraid to turn the RPM up when you find your cut quality degrading around 60mm/sec. As long as you are not burning, I wouldn't worry too much about 'ideal chiploads'. If you were a production shop doing 40 sheets a day, that would be different. Quality of cut is king.

-B
Brady, does composite board (like Shane is cutting) tend to create more screeching than lumber?
Reason I ask is that I don't cut composite, just mostly hardwoods, and my cuts are always best if I optimize the screech out of the picture.
It's become pretty clear to me that that screechless "sweet spot" is where I don't toss chips off any of my raised letters, even when the bit is cutting with the grain on the soft side of the grain (the edges that like to chip).
Obviously this isn't something I'd have to worry about with composite because there's no grain to worry over, and it makes sense that you go with the cleanest feed and speed, I just wondered if composite is noisier so I can remember to throw my lumber numbers out the window if I start cutting it. :)

[Brady Watson]

Some materials are worse than others, if for no other reason than harmonics. 1/4" dia tools are notoriously loud in a number of situations, but I would not say that was absolute. One way to minimize this is to up-size the diameter of the tool to say 5/16 or 3/8", or reduce step down, if the cause was too much chipload. You are correct in thinking that 'screech-less' tuning is the way to go, but on some materials you just cannot completely avoid this.

If you hear noise in the corners etc, it is telling you that the cutter is deviating from the ideal path, because it is deflecting. First thought would be to think that you are pushing the tool too hard, but in a number of cases it is because the tool is not loaded enough to keep the tip from whipping, like a broken driveshaft. With a deeper cut, the flutes of the tool are more evenly supported and this counteracts that kind of deflection. When the tool is overloaded, getting close to the point of snapping, it can also deflect because it is loaded too hard.

Sometimes the only way to get into the sweet spot is to start out conservatively, and then feather in more speed. You should be able to get pretty close in a short amount of time by pausing, adjusting speeds and resuming the file. Note that I did not say do 'on the fly' +/- speeds, because this does not purge and refill the command buffer like hitting the spacebar or 'S' key will. OTF adjustments keep the originally calculated ramp settings for the original speeds and can result in clunky corners and abrupt movement changes, which is certainly not what you want when you are trying to dial in.

-B

[shilala]

Got ya, Brady. You pointed me to an article in the past that really helped me understand what the tools were doing when they corner and dig, and where pressures are exerted. I think it was just on ramps and lead-ins, and it was excruciatingly painful, but it made sense.
I doubt if you remember what the article was, but it may help here. I'd like to read it again now that I understand a bit more, too.
I'll admit that I haven't really had need to employ the strategies in the article, but I have in a sense. I create my toolpaths and projects to work around high stresses on the tooling. The article made me aware that I needed to do so, and it's cleaned up my work dramatically. I'm guessing a refresher would take things a step forward.