[WhippyBoy]

I've got the 1100 mill, only about two months old now (I'm also a newbie, btw). Using Gwizard with the Tormach 1100 defined, it estimates with a 12mm Carbide endmill, on the most conservative setting, it says I should be able to cut at DOC 10mm / 10% Cutwidth / 5,100RPM / 1,800mm Feedrate on 6061 Aluminum. When I go to test this, I get major squeal and chatter marks.. I've even set it back to 5mm DOC and slowed down the feed to 1,300 and get a loud squeal not the sweet hum when the feeds and speeds are spot on with a very shallow and slow cut. The endmill I'm using is a nice 12mm Iscar coated carbide. I'm cutting dry with a mist of WD-40 on the aluminum block prior to start.

Is there something I'm doing wrong here? Is Gwizard way off or am I using it incorrectly? Appreciate any constructive suggestions from Tormach vets! Thanks in advance!

[Steve Seebold]

Not familiar with the end mill you're using. I know their insert cutters work really well. I think the feed rates you're getting from Gwizard are a bunch of crap. I don't know where this gou comes up with the feeds and speeds he does. Your feed rate us way too high. When I do a ruff cut, I will run the cutter 5,000 RPM, 40 IPM, .200 depth of cut and about 20% of the cutter diameter width of cut, while leaving .015 for a finish cut, then I'll slow down to 3,500 RPM and about 25 IPM for the finish pass for which I will always take at least one spring pass.

I have never been able to get a satisfactory finish while running the spindle 5,100 RPM.

[SCzEngrgGroup]

You really don't give us much to go on. How many flutes?? WHAT coating? What are the flute length and stickout? What kind of toolholder are you using?

There are a great many factors that can cause the problems you're seeing, but you have to start with the above really critical factors. Chatter is a resonance effect, which is greatly affected by machine rigidity. It will be much worse if there is significant runout, or a machine resonant frequency near the vibration frequency created by the cutter at that spindle RPM. In many cases, what seems the "obvious" right thing to do is exactly wrong. With chatter, increasing feedrate is, if anything, more likely to reduce the chatter than reducing the feedrate. Changing RPM, either up or down, can also help. Changing the number of flutes can make a big difference, as it changes the vibration frequency. Using a shorter, stiffer, tool will often help a lot as well. Always use the shortest, stiffest toolholder you can. If you're using an ER20 chuck, try using a setscrew holder instead - they are much stiffer. Make sure your spindle bearings are properly pre-loaded, and there is no axial or radial play, or excessive runout. You might try going deeper as well - the machine should be able to handle quite a bit more.

On relatively lightweight "hobby-grade" machines, like the Tormach, I find I get a better result by going slower and deeper. I see little value to carbide, as the machines are generally not rigid enough to really get much advantage out of them. I prefer HSS, which is MUCH cheaper, and gives me the same MRR. As an example, try taking a full-width slotting cut at 2900 RPM, 1/4" DOC with a 1/2" 2-flute endmill. The Tormach *should* be able to do that, and at the lower RPM you're less likely to encounter chatter, as the machine frame can more effectively damp out the lower frequency vibrations.

Regards,
Ray L.

[WhippyBoy]

Thanks for the replies and advice. My cutter is a 4-flute, 12mm Carbide Iscar with Tialn coating. I have about a 50mm (2") stickout using a TTS setscrew holder for it. I think I'll try out some of your suggestions on the Feeds & Speeds and see what happens. Thanks!

[SCzEngrgGroup]

Thanks for the replies and advice. My cutter is a 4-flute, 12mm Carbide Iscar with Tialn coating. I have about a 50mm (2") stickout using a TTS setscrew holder for it. I think I'll try out some of your suggestions on the Feeds & Speeds and see what happens. Thanks!

I meant to suggest: 2900 RPM, full width, 1/4" DOC at 20 IPM. I do this with HSS. What GWizard suggested is pretty reasonable. You're running nearly twice the RPM, with a 4-flute tool, which should give you roughly 4X the feedrate, and that's roughly what GWizard is giving you. I'd guess the machine is simply not rigid enough to handle it.

Also, a 4-flute is not the best choice for aluminum - two or three flutes is better, especially without coolant. If you're really determined to use carbide, you might want to try a variable helix tool, as they are designed to avoid the harmonics that induce chatter. But, really, I think you'd be much better off using HSS. And, you'll save a LOT of money to boot. I do most of my work with 1/2" 2-flutes that cost me about $12. I'm guessing your Isacr tool probably cost at least 4-5X as much? And without coolant, you'll probably be chipping the heck out of the cutting edges in short order. I can use the same $12 tool for weeks at a time.

Regards,
Ray L.

[WhippyBoy]

Thanks for the extra details! Makes sense. I'll have to find some 2 fluter's and give them a try. I actually won the carbides on Ebay and picked them up for about $10ea, so they were kind of a steal; especially for the Iscars! I'm guessing you're right about the Tormach not being rigid enough. Man.. seeing some of those high-end VMC's tear through aluminum with 1" cutters at full depth on Youtube makes me salivate! But I'll make do with the Tormach for now. I bought it to learn on before investing in a Haas VF2 later on. Thanks again! Good to know what others are using on the Tormach so I at least have a good reference!

I meant to suggest: 2900 RPM, full width, 1/4" DOC at 20 IPM. I do this with HSS. What GWizard suggested is pretty reasonable. You're running nearly twice the RPM, with a 4-flute tool, which should give you roughly 4X the feedrate, and that's roughly what GWizard is giving you. I'd guess the machine is simply not rigid enough to handle it.

Also, a 4-flute is not the best choice for aluminum - two or three flutes is better, especially without coolant. If you're really determined to use carbide, you might want to try a variable helix tool, as they are designed to avoid the harmonics that induce chatter. But, really, I think you'd be much better off using HSS. And, you'll save a LOT of money to boot. I do most of my work with 1/2" 2-flutes that cost me about $12. I'm guessing your Isacr tool probably cost at least 4-5X as much? And without coolant, you'll probably be chipping the heck out of the cutting edges in short order. I can use the same $12 tool for weeks at a time.

Regards,
Ray L.

[SCzEngrgGroup]

Thanks for the extra details! Makes sense. I'll have to find some 2 fluter's and give them a try. I actually won the carbides on Ebay and picked them up for about $10ea, so they were kind of a steal; especially for the Iscars! I'm guessing you're right about the Tormach not being rigid enough. Man.. seeing some of those high-end VMC's tear through aluminum with 1" cutters at full depth on Youtube makes me salivate! But I'll make do with the Tormach for now. I bought it to learn on before investing in a Haas VF2 later on. Thanks again! Good to know what others are using on the Tormach so I at least have a good reference!

I'm working on a Novakon Torus Pro, not a Tormach. But I still think the Tormach should be able to do that cut, or at least close to it. If it's unhappy, just back off on either depth or feedrate until it sounds happy.

NO "benchtop" machine is going to cut like a real VMC. There is a world of difference in spindle RPM, power, and machine rigidity. There's a good reason those expensive machines are so expensive. Even a "little" Haas will run circles around these small, lightweight machines, both in terms of MRR and real-world accuracy and precision. But, they can still do an awful lot of good work. You can see the kind of stuff I do with mine here:

http://www.cnczone.com/forums/novako...n_machine.html

My machine is larger than the Tormach, but otherwise not all that different in terms of capability. They're very similar in terms of spindle power, overall rigidity, and accuracy.

Regards,
Ray L.

[mike sr1]

Is your fixture nice and solid?
endmill sharp?

[WhippyBoy]

I'm using a 6" Glacern Premium Vice, milling a 1" x 2" x 12" block of aluminum with about 6mm of the base clamped in the jaws (trying to profile as much of one side as possible). The endmill I'm using is brand new, so it's sharp.

Update: So I'm able to hit F1,800mm's at 5,140RPMs (maxed out) @ 10% width and 3mm DOC... I'm going to experiment more with what's suggested below because I'm just not happy with the DOC... the cycle takes forever! Below is my CAD model of what I'm working on; it's my prototype for a Mosin Nagant picatiny rail / mount.

Attachment 202222

Is your fixture nice and solid?
endmill sharp?

[keithmcelhinney]

I run a smaller machine than the Tormach and started out not knowing a thing. I now know a tiny amount (enough to get in trouble), but one thing thing that really changed what I could do with my mill is keeping the stickout as little as possible. I don't run 1/2" bits but I run some 3/8" 3 flute variable helix endmills and they cut really nice on my machine and are super quiet.

-Keith

[Philbobb]

I was having the same issue with what seemed like panzy cuts making the machine chatter. Started using a torque wrench at 30 in/lbs on the drawbar and it stopped. Obviously make sure the collet and drawbar are lubed appropriately as well.

[zero_divide]

Attachment 202308

This machine should be able to pull out the cut you describe easily.
First of all dont use TiAlN coating on aluminum.

Aliminum sticks to it and it may be contributing to your chatter.
I dont care that BW says its ok. Its a wron coating for aluminum.

Second of all you should not use 4 flute endmills on aluminum.
It should be ok for such a shallow cut however.

Check your tool clamping and stickout too.
Too much stickout will lead to chatter.
Also make sure you check for endmill runout.

Good luck

[Steve Seebold]

Thanks for the replies and advice. My cutter is a 4-flute, 12mm Carbide Iscar with Tialn coating. I have about a 50mm (2") stickout using a TTS setscrew holder for it. I think I'll try out some of your suggestions on the Feeds & Speeds and see what happens. Thanks!

It looks to me like you're trying to run your machine as if it were a Haas or some other type of real machining center. YOU CAN'T DO THAT. You don't have the horsepower or the rigidity to do that.

If you feel the need to be able to run like that, you probably bought the wrong machine. If I were you, I'd sell your machine before you destroy it and buy a machine that will do what you're trying to do.

I remember when I was learning to run NC and CNC machines, the man who was teaching me would tell me a brand new HSS end mill was actually TOO sharp, and when they are TOO sharp, there is a good chance they will cause chatter. I remember, he would drag a copper penny over the cutting edge just to take a little bit of the dead sharpness away.

After seeing the feeds and speeds people are getting from a program like GWizard, I am ever more convinced that the author read a book that somebody wrote that read a book that somebody wrote that read a book that somebody wrote and so on.

Running HSS cutters at the speeds and feeds recommended in GWizard for cutting aluminum is going to give you the exact same result you would get if you run your HSS cutter too fast cutting steel. You're gonna burn it up.

I have a friend who had a shop and he REFUSED to spend the money to buy good carbide cutters, but he couldn't understand why after 3 or 4 parts his HSS cutters had turned to an amber color, and after about 20 parts they were blue. Well, he was working them so hard he got them so hot he actually took the temper out of them.

Oh yeah, I should also mention he wouldn't spend the money to buy good coolant either. ARE YOU?

[SCzEngrgGroup]

After seeing the feeds and speeds people are getting from a program like GWizard, I am ever more convinced that the author read a book that somebody wrote that read a book that somebody wrote that read a book that somebody wrote and so on.

Never mind that there are MANY of us out here running at those feeds and speeds all the time, and getting excellent results, with very long cutter life.....

Regards,
Ray L.

[tbaker2500]

You need to look at tool and part rigidity. To cut at high speeds you need a really short, stiff cutter, and a firmly held workpiece. Hanging off the edge of the vise is a great way to get chatter/squeal. I recommend this article:
CNC Milling Chatter and Stable Milling Speeds

[Spinnetti]

You need to look at tool and part rigidity. To cut at high speeds you need a really short, stiff cutter, and a firmly held workpiece. Hanging off the edge of the vise is a great way to get chatter/squeal. I recommend this article:
CNC Milling Chatter and Stable Milling Speeds

I've made that mistake too many times - single side work support is asking for chatter city... I also found that resonant frequencies happen on any setup, and to tweak speeds and or feeds to avoid that. Choke up that cutter, fully support the work, use good tools, and good coolant. I found Gwizard is fine, but start with the 2nd off slowest setting on the wizard and make sure the data is accurate in all the cells. If buying cheap noname cutters, don't expect stated performance.... Gwhiz was 10x off on HSS wodruff cutters though.. even on the minimum setting it stalled my spindle...

[WhippyBoy]

I appreciate what you're getting at but I never for a moment thought I could cut like a big VMC can with my little Tormach. I was going by what I've seen Tormach's own video cutting demonstration are doing and by what Gwizard indicates I "should" be able to cut. I'm even using the conservative turtle setting... I'm thinking my issue (like yourself and some of the others have suggested) is too much stickout and/or too many flutes for aluminum. I have a three flute uncoated carbide cutter coming in today and am going to give that a shot.

Regarding Gwizard, I've heard nothing but great reviews from people on this forum and the other ones... so that's why I put a lot of stock in what their recommendations are. Not sure if you've used it, but their calculations do take into account the cutter type and material as well as the machine you're using. This is why I was a bit shocked that I could not cut 'approximately' by what was recommended.

It looks to me like you're trying to run your machine as if it were a Haas or some other type of real machining center. YOU CAN'T DO THAT. You don't have the horsepower or the rigidity to do that.

If you feel the need to be able to run like that, you probably bought the wrong machine. If I were you, I'd sell your machine before you destroy it and buy a machine that will do what you're trying to do.

I remember when I was learning to run NC and CNC machines, the man who was teaching me would tell me a brand new HSS end mill was actually TOO sharp, and when they are TOO sharp, there is a good chance they will cause chatter. I remember, he would drag a copper penny over the cutting edge just to take a little bit of the dead sharpness away.

After seeing the feeds and speeds people are getting from a program like GWizard, I am ever more convinced that the author read a book that somebody wrote that read a book that somebody wrote that read a book that somebody wrote and so on.

Running HSS cutters at the speeds and feeds recommended in GWizard for cutting aluminum is going to give you the exact same result you would get if you run your HSS cutter too fast cutting steel. You're gonna burn it up.

I have a friend who had a shop and he REFUSED to spend the money to buy good carbide cutters, but he couldn't understand why after 3 or 4 parts his HSS cutters had turned to an amber color, and after about 20 parts they were blue. Well, he was working them so hard he got them so hot he actually took the temper out of them.

Oh yeah, I should also mention he wouldn't spend the money to buy good coolant either. ARE YOU?

[tbaker2500]

I use GWizard numbers all day long, but it's really important to watch the tool deflection. If it's orange, don't do it.

I am continually amazed at how incredibly difficult machining is. Every new project brings new challenges. (Broke an EM today because I was stupid on how I held something.)

[WhippyBoy]

UPDATE:

Well, you guys were right! My problem was that I had far too much of the end mill sticking out. I moved about half of it in leaving only about 25mm of stickout and it tore through the roughing cycle with that sweet hum and flying chips!

[tbaker2500]

SHHH!! Don't tell them, it will go to their heads!