[sperman]

This is a .0625 DOC, .160 WOC. It is a 1/2" 4 flute end mill running at 3000 RPM and 15 IPM. GWizard recommended slower RPM and faster feed, but it was even worse at those settings.

I've got several hours left before I'm done with this fixture. I'm afraid the end mill will be shot long before the job is done.

The endmill has about 1.4" of stickout. I know a shorter endmill would be better, but it is the shortest endmill I have.

[ame=http://www.youtube.com/watch?v=sqm_On3mERM&feature=youtube_gdata]Tormach Cutting Steel Fixture - YouTube[/ame]

While waiting for the movie to upload, I went to 3500 RPM and 20 IPM and it is better.

[GJeff]

No matter what I try on my manual mill it always makes that screeching sound on mild steel, but at least I don't seem to hear any chatter in your video. I'd also like to know what some actual experts have to say. Perhaps the screech on steel is unavoidable or perhaps it's rubbing from going too slow.

[Peter Neill]

That noise is the cutter rubbing because the chipload is too low. you're cutting barely over 0.001"/tooth with that feed & speed at best. You could happily halve the speed and keep that feed, or keep that speed and double the feed. Either one will quieten that cut down considerably.

[sperman]

I started at 2250 RPM and 20 IPM and the squeal was even worse. I guess I went the wrong direction with my adjustments.

The cutter lasted about 45 minutes before it became dull and started to pull out of the draw bar.

[GJeff]

I hate pullout. Make sure you've read this www.tormach.com/uploads/163/TD31090_ToolHolding-pdf.html

Let us know when you get it dialed in more

[mike sr1]

I didnt see coolant running in the video, use coolant especially on steel. The rpm sounds too high for steel as well, I would try about 1000 rpm to start and adjust from there, about 10 to 15 ipm, flood coolant.
The sound I am hearing is one thats made by a dull tool, its not cutting its rubbing.

That long endmill isnt helping either noise wise.

This is just my opinion, and just a few things I would try.

[LeeWay]

What? Hunh?

[Steve Seebold]

This is a .0625 DOC, .160 WOC. It is a 1/2" 4 flute end mill running at 3000 RPM and 15 IPM. GWizard recommended slower RPM and faster feed, but it was even worse at those settings.

I've got several hours left before I'm done with this fixture. I'm afraid the end mill will be shot long before the job is done.

The endmill has about 1.4" of stickout. I know a shorter endmill would be better, but it is the shortest endmill I have.

Tormach Cutting Steel Fixture - YouTube

While waiting for the movie to upload, I went to 3500 RPM and 20 IPM and it is better.

What kind of cutter is it? HSS or carbide? If it's HSS your spindle speed is way to fast. If it's carbide, your feed may not be high enough.

You need to be using coolant. In your video it looks like you are trying to run your cutter dry.

At that speed if you're running a cutter with sharp corners the first thing you're going to do is going to be knock the sharp corners off. Now you have flat corners and you are no longer cutting the material, you are just pushing it out of the way, and the longer you abuse that cutter, the louder it's going to get.

It's going to be hard to get your cutter stick out less than 1 1/4 inch because if you try, the run out on the flutes will be inside your tool holder.

You might have better luck if you use a stub end mill.

A good cutter for what you are trying to do there would be a Duramill WhisperKut. It's a 3 flute wnd mill with a .020 to .030 corner radius, and I speak from experience when I say you can really haul ass with them. I used to cut 4340 steel at 2600 RPM, .375 DOC, .188 wide at 30 IPM with a 1/2 inch end mill. But I was using a FADAL that weighed 9,000 pounds, and had a 22 horsepower spindle.

I would say that with the cut you discribe in your video, that cutter will do well for you. Only problem is, they are a little on the pricey side at around $60.00 each.

You need to remember though, "GOOD TOOLS MAKE CHEAP PARTS".

[sperman]

I am filming through my shower curtain enclosure, so it must not be visible, but I am running flood coolant.

This was a brand new carbide end mill, before I started cutting.

I'll try lower RPM tonight and let you know what I find. In the past, when I've tried cutting steel with a heavier cut the machine wants to shake itself apart.

Thanks for all the ideas. I'll let you know what I find.

[SCzEngrgGroup]

If lower RPM/increased feedrate "shakes" the machine, then your only option is to reduce depth/width of cut. You MUST maintain adequate chipload, or the tool cannot cut properly.

Regards,
Ray L.

[Runner4404spd]

switch to a 3/8 end mill. those are usually shorter and keep the same speeds and feeds. your parameters don't sound too bad other than sometimes its better to take a wider pass at a slower feed rate to increase the chip load on the tool. you need to push past the noise and get the tool into the cut once the tool is loaded it will be quiter. also make sure you have enough HP for your cut. it looks like your running a tormach, make sure your not at the low torque point of the spindle power curve.

[SCzEngrgGroup]

switch to a 3/8 end mill. those are usually shorter and keep the same speeds and feeds. your parameters don't sound too bad other than sometimes its better to take a wider pass at a slower feed rate to increase the chip load on the tool. you need to push past the noise and get the tool into the cut once the tool is loaded it will be quiter. also make sure you have enough HP for your cut. it looks like your running a tormach, make sure your not at the low torque point of the spindle power curve.

Even with his current 1/2" endmill, if he takes a wider cut, it will do virtually nothing to increase chipload (he's already at 32% WOC, so chip-thinning is virtually non-existant), and decreasing feedrate can only reduce chipload, it cannot increase it. Reducing RPM will increase chipload, if the feedrate is maintained. His current cut is under 0.2HP, so he's nowhere near power limited.

Regards,
Ray L.

[sperman]

Thanks for all of your help guys.

I started at 1000 RPM, 15 IPM and all was good.
Next as 1500 RPM, 22 IPM, still good
When I went to 2000 RPM, 30 IPM the noise was back. (Still now where close to running out of HP.)

I guess the length of the tool is too much for that speed. At least I can get back to making chips and finish my fixture.

Ray,
I don't know what may have happened in other threads, but I find your advice to be valuable.

[sperman]

I just checked with GWizard, and it said at 1500 RPM I should only be going 14 IPM.

[SCzEngrgGroup]

Ray,
I don't know what may have happened in other threads, but I find your advice to be valuable.

Scott,

Thanks.

What I hear in the video sounds like classic chatter, which is a harmonic effect - the RPM and number of flutes get the tool and/or workpiece vibrating at close to their natural frequency, or a harmonic of it. Usually, the solution is to do something to stiffen things up (larger diameter, stiffer, or shorter tool, stiffer toolholder, less stickout, etc.), or significantly increasing or reducing RPM, to change the frequency. A shorter tool will generally be the most effective solution.

I do probably 90% of my work with 2-flute 1/2" HSS endmills, with a 1-1/4" length of cut. That gives the best compromise of the many parameters, and lets me run the maximum MRR my machine is capable of, as well as cost (they're only about $13 each, and last a loooooong time). I use smaller tools only where necessary to get into tighter places.

Though not an ideal solution, you can try clamping your workpiece directly to the table, putting blocks under it, so you can be cutting higher up on the tool, to make it behave more like a shorter tool. Just make sure the workpiece remains very well supported and solidly mounted, so it doesn't vibrate as well.

Regards,
Ray L.

[dbrija]

Scott,

Thanks.

What I hear in the video sounds like classic chatter, which is a harmonic effect - the RPM and number of flutes get the tool and/or workpiece vibrating at close to their natural frequency, or a harmonic of it. Usually, the solution is to do something to stiffen things up (larger diameter, stiffer, or shorter tool, stiffer toolholder, less stickout, etc.), or significantly increasing or reducing RPM, to change the frequency. A shorter tool will generally be the most effective solution.

I do probably 90% of my work with 2-flute 1/2" HSS endmills, with a 1-1/4" length of cut. That gives the best compromise of the many parameters, and lets me run the maximum MRR my machine is capable of, as well as cost (they're only about $13 each, and last a loooooong time). I use smaller tools only where necessary to get into tighter places.

Though not an ideal solution, you can try clamping your workpiece directly to the table, putting blocks under it, so you can be cutting higher up on the tool, to make it behave more like a shorter tool. Just make sure the workpiece remains very well supported and solidly mounted, so it doesn't vibrate as well.

Regards,
Ray L.

My experience with 1/2" 3 flutes has been poor on my 1100 for some reason, but 3/8" and under work great. I've tried several things without luck, just get a lot of squeal and chatter in 6061.

[SCzEngrgGroup]

Try 2 flutes instead of 3, assuming chatter was your problem. Changing the number of flutes changes the frequency of vobration, and a 2-flute will generally be stiffer than a 3-flute, all else being equal. I assume the 3-flutes you tried were carbide, not HSS, since 3-flute HSS endmills are not very common. This could be part of the problem. You'd need to push them pretty hard to get them to perform well, and operating in their "sweet spot" requires more than 1.5HP, and running them lightly loaded does not give a good result, and wears the tool quickly. Variable-helix endmills are also good at battling chatter, that's mostly what they are made for, but they tend to be rather pricey.

Regards,
Ray L.

[AiR_GuNNeR]

I started at 2250 RPM and 20 IPM and the squeal was even worse. I guess I went the wrong direction with my adjustments.

The cutter lasted about 45 minutes before it became dull and started to pull out of the draw bar.

The high frequencies seem to effect the ability to hold the TTS holders in place. Almost like using ultrasonics to break something loose. This happened to me cutting some 6061 using a 3/8" endmill. I had the spindle speed about three times higher than I thought and got that same squeel, and soon noticed that my cut was getting deeper...

[waltpermenter]

You are running too high rpm for cutting steel with that cutter. Get it under 1000, recommended sfm for mild steel is 80-100, much lower than what some folks with only aluminum cutting experience are used to. for the 4fl .500 endmill a good ipt of .003, 100 sfm gives 764 rpm at 9 ipm.

[sperman]

Here's where I am, and it seems to be running well.

I realized there were places that the cutter was going to have to run a full width pass, so I am now running .5 WOC. I switched to a radius nosed cutter as Steve suggested (still 4 flutes.) Running at 14 IPM, 1000 RPM and it seems to be doing OK.

Thanks again for everyone's input.

Scott