profiling deep finishing pass, chatter, please help

[TPR]

i only have a few parts i've done this deep and i cant seem to get the hang of it.

on my finish pass i'm running a 1/2" 3 flute carbide tool, 2.75" stick out, DOC is 1.875", 40 IPM, 3500 rpm and i'm only taking off 0.005" oh and this is in 6061 aluminum and a 2" cut length on the tool. the part is very rigid.

sometimes it works and others times it doesn't and of course as soon as it gets some chatter the damn tool pulls out and wrecks my bottom plane.

any suggestions would be awesome

i working with a pcnc1100 series 3.

thanks guys

Carlos

Similar Threads:

• Finishing Pass is above model
• Outside Finishing Pass Fixturing
• Cutting 3" deep pockets - no finishing pass?
• Newbie- Vcarve pro finishing pass?
• the finishing pass

[popspipes]

Chatter, once it starts its hard to get rid of, I would try reducing RPM. With that much stickout its going to be a problem, chatter is a resonance of the tool or work piece or both, There may be cutters specifically ground to reduce it I am not sure, I know it works on lathe boring bars by reducing the back relief of the cutting tool and varying the doc and rpm.
I try to use the shortest "fattest" tools I can.
long tools and high RPM = Chatter, just my rule of thumb.......

I really havent found a good cure for it, what works in one situation may not work in another.

[TPR]

thats my issue, i cant find the pattern of what does what

[TPR]

thanks for the reply :-)

- - - Updated - - -

oh, and if i go off GWizard, it wasnts me to run 5000 rpm and 90 ipm, full depths of cut..... makes no sense

[joshetect]

I run a similar cut. I use a destiny tool viper 3 flute (variable) You need to go through a reseller to get them, but lakeshore carbide also has a variable 3 flute.

You can also email lakeshore and see what they recommend.

Our unique geometry includes a .005-.007 corner radius extending tool life, a highly polished flute gullet improving chip evacuation, variable helix multi index flutes eliminating vibration and harmonics and Zirconium Nitride coating for hardness and lubricity. This design allows a heavy chip load per tooth for maximum material removal in aluminum and unmatched performance. Can be used to rough or finish, slot or profile in aluminum and plastics.

[DRWPrecision]

Afternoon TPR,

First change to a 4 Flute Endmill it'll have more backbone, second get away from the squeeze collet and go to a short solid holder with a set screw. Just hand grind a flat on the endmill for the set screw to lock. This will solve your issue with tool movement.

Good luck and Let me me know your results
DRW

[TPR]

I run a similar cut. I use a destiny tool viper 3 flute (variable) You need to go through a reseller to get them, but lakeshore carbide also has a variable 3 flute.

You can also email lakeshore and see what they recommend.

What feeds and speed do you run with that tool?

[TPR]

Afternoon TPR,

First change to a 4 Flute Endmill it'll have more backbone, second get away from the squeeze collet and go to a short solid holder with a set screw. Just hand grind a flat on the endmill for the set screw to lock. This will solve your issue with tool movement.

Good luck and Let me me know your results
DRW

I'm running a set screw tool holder, the tool doesn't come out of the holder, it's the holder that comes out of the spindle when it chatters

I may try that 4 flute. I'll order one, got nothing to loose at this point

Thanks

[DRWPrecision]

Ok, with that said you just shedded new lite to your issue... hold off on spending money on a new endmill and let's focus on the bigger problem of dropped holder. I'm not familiar with the machine you mentioned but I did noticed it uses an R8 holder. I'm willing to bet that majority of you chatter is stemming from a bigger problem overlooked as your over focusing on the cutting edge i.e. tool. Let's work backwards and focus on the first weakest link, the tool holding system. Assuming you have an auto air ratchet for the R8 holder the problem is possible air pressure issue or a sheared socket pin causing insufficient makeup power. First check for a cracked plastic airline between the air valve and ratchet motor and follow with checking the roll pin in the ratchet socket... I'm putting my money on the roll pin!

If you find the roll pin to be the issue Replace it with a hardened and ground pin of the same diameter and length and problem solved.

In regards to speeds and feeds for a four flute leave RPMs the same just add feed for the additional flute. Considering your depth of cut no need to use a 3 flute or high helix endmill.

Keep me posted...

[AUSTINMACHINING]

If your getting pullout at only
.005 of engagement, you have a drawbar problem probably causing the chatter.

[Steve Seebold]

40 IPM, 3500 RPM is way too fast.

When you approach the cut are you circling in or are you going straight in to the cut?

Can you describe the pocket you are cutting? Are there any corner radii or is it a round hole?

[DRWPrecision]

TRP, My apologizes if I wasn't clear. The ratchet socket I mentioned drives the hex on top of the Drawbar....

[joshetect]

Definitely double check your PDB. I have mine set at 120 psi, and the tool 'just' barely comes out.

Also see Tormachs writeup on tool pull out and where to lube and where to keep clean.
https://www.tormach.com/uploads/163/...1010A-pdf.html

[DRWPrecision]

I wouldn't be to concerned with the RPM, 3500 is only 460 SF. We constantly run Carbide on aluminum between 1000-1250 SF although you might drop the chip load in half. At 40 IPM on a 3 Flute your at .004, bring it down to .002 after you address your Drawbar issue.

[CadRhino]

I bet it’s runout in the spindle. Have you checked it?
It is a challenge to get the r8 tts to run true without some honing/tweaking.



QUOTE=DRWPrecision;2111728]Ok, with that said you just shedded new lite to your issue... hold off on spending money on a new endmill and let's focus on the bigger problem of dropped holder. I'm not familiar with the machine you mentioned but I did noticed it uses an R8 holder. I'm willing to bet that majority of you chatter is stemming from a bigger problem overlooked as your over focusing on the cutting edge i.e. tool. Let's work backwards and focus on the first weakest link, the tool holding system. Assuming you have an auto air ratchet for the R8 holder the problem is possible air pressure issue or a sheared socket pin causing insufficient makeup power. First check for a cracked plastic airline between the air valve and ratchet motor and follow with checking the roll pin in the ratchet socket... I'm putting my money on the roll pin!

If you find the roll pin to be the issue Replace it with a hardened and ground pin of the same diameter and length and problem solved.

In regards to speeds and feeds for a four flute leave RPMs the same just add feed for the additional flute. Considering your depth of cut no need to use a 3 flute or high helix endmill.

Keep me posted...[/QUOTE]

[IMT]

+1 on checking runout.
Also in my experience using an R8 spindle with any tool that sticks out of the spindle more than 3 inches or so (including the holder) you must reduce the spindle speed to avoid chatter. Basically the tool deflects due to lack of spindle rigidity as well as tool flex. Reducing the spindle speed helps somewhat.

[Steve Seebold]

I wouldn't be to concerned with the RPM, 3500 is only 460 SF. We constantly run Carbide on aluminum between 1000-1250 SF although you might drop the chip load in half. At 40 IPM on a 3 Flute your at .004, bring it down to .002 after you address your Drawbar issue.

Yeah, but you’re definitely not doing that on s Tormach.

[shred]

If you have a PDB, pull the Bellville stack and look for cracked washers. That's a surefire recipe for chatter and TTS pullout.

[C*H*U*D]

Pull and check the wear on your Tormach TTS R8 collet. I was having issues some time ago, and when I pulled mine out to check, the wear on the collet showed it was gripping only along the slots of the collet at the very bottom. I replaced it, and a lot of my issues with chatter went away. Maybe you got a lemon.

[philbur]

With that size cutter and DOC you are pretty much on the limit of the ER20 TTS holder, even with all the tweaks and tricks. Every tooling system has its' limit and you found the TTSs'

What you should try is a ER40 collet holder with a an R8 shank. Also forget the PDB, use a manual and do it up tight. It works for me when profiling with a very big DOC.



Phil