chatter issues milling a pocket

Ukraine Train · May 23, 2015

I'm milling these pockets in annealed 8620 with an Iscar Heli2000 with APKT inserts. 500SFM, .005IPT, ramping down at 2° to .150" deep per pass. I get a loud screech as it goes around and it's leaving chatter marks. Interestingly, I started this job with worn inserts and it went ok, but when I flipped to the fresh side I started having the issue. I tried adjusting speed and feed with no effect. Any suggestions?

Also, what's a good way to deburr the corners of this on both ends? Hand held flap wheel? Wire wheel? Thanks for any tips.

Erick O · May 23, 2015

I think the cutting parameters are o.k.
Due to the geometry of the finished part, when the cutter is in the corners there is no rigid lateral support to absorb the pressure of the cutting action. I'm guessing the part is chattering, or the part and tool are resonating together. Would a round pocket cut in a set of soft jaws would give more contact and support? Can you flip the part over and use a larger diameter tool and/or a shorter extension?

DMF_TomB · May 23, 2015

chatter

Ukraine Train said:
I'm milling these pockets in annealed 8620 with an Iscar Heli2000 with APKT inserts. 500SFM, .005IPT, ramping down at 2° to .150" deep per pass. I get a loud screech as it goes around and it's leaving chatter marks. Interestingly, I started this job with worn inserts and it went ok, but when I flipped to the fresh side I started having the issue. I tried adjusting speed and feed with no effect. Any suggestions?

Also, what's a good way to deburr the corners of this on both ends? Hand held flap wheel? Wire wheel? Thanks for any tips.
View attachment 140228

.
part vibration usually means lowering depth and or width of cut, lowering sfpm, lowering feed. sometimes a smaller diameter cutter is used.
.
leaving .010 to .020 for a finish cut usually reduces any burr left. often the chatter marks from a roughing cutters are removed by the finish cut so minor chatter marks does not matter much

CarbideBob · May 23, 2015

Ukraine Train said:
.....Interestingly, I started this job with worn inserts and it went ok, but when I flipped to the fresh side I started having the issue.

Maybe a hint here?
Bob

NodecoMachine · May 23, 2015

I would use a smaller diameter solid carbide endmill. Less cutting forces and such.

706jim · May 23, 2015

CarbideBob said:
Maybe a hint here?
Bob

I had a chatter problem milling an aluminum wheel some years back. Long extension on a brand new 1/2" HSS 2 flute.
After the cutter was "broken in" which took about 15 minutes, the chatter disappeared. Maybe something similar is happening here with the fresh inserts.

CarbideBob · May 23, 2015

Yup,
and what is weird is that every carbide company in the world used to give out "hone stones" with their name on it for free like candy.
Every machinist had a Kennametal, Carboloy, Valenite, or Newcomer stone. We bought them by the thousands. Much better than ink pens or hats.
The purpose, get rid of chatter by intentionally dulling the edge and actually increasing the cutting load....... Strange, eh. more load, less chatter, and longer tool life.
You would just hit the edge of each tool with the stone and life would be so much better for you.
Now coatings mean you need the right edge prep before it is coated and these stones are hard to come by.
At one time you could order any carbide up-sharp, A,B or C honed. Today a very different world of catalog/internet standards and no longer true.
Sadly only the volume users get their choice of edge prep now inside a grade so most just have to live with dropping off feeds and speeds.
The price for progress and lower cost inserts.
Bob

Milland · May 23, 2015

CarbideBob said:
Yup,
and what is weird is that every carbide company in the world used to give out "hone stones" with their name on it for free like candy.
We bought them by the thousands.
The purpose, get rid of chatter by intentionally dulling the edge and actually increasing the cutting load....... Weird, eh. More load, less chatter.
Now coatings mean you need the right edge prep before it is coated.
Bob

Hi Bob,
Is it fair to say those were also the days of much larger carbide grains, and the reason to "dull" the edges was to reduce the risk of larger grains digging in to the workpiece and being pulled out? The traverse rupture strengths would have been lower too, so lowering the chance of sharp edges grabbing the work and overloading the tool could be a factor.

What do you think?

lowCountryCamo · May 23, 2015

I always thought to reduce chatter you wanted a sharper cutter to reduce cutting force. Although after reading what CarbideBob wrote that does make sense to me.

Krovvax · May 23, 2015

Grab a good carbide endmill and youll get rid of the chatter. The apkt facemill just bang around on every insert biting the stock a endmill is sharp will reduce the cutting force and cut instead of banging. Im pretty sure its going to fix your problem and might be even faster.

Ukraine Train · May 23, 2015

Thanks guys. Maybe I'll try a 1/2" endmill. Should I just follow the pocket contour or would it be better to sort of work my way from the inside-out to reduce the step over? I wanted to use the inserted-endmill because I have 300 of these to do and figured it would be cheaper to replace a few inserts rather than a few $60 endmills.

I'll also do a finish pass to try to knock the burrs down.

Milland · May 23, 2015

If your fixturing is stable enough, I'd run as large a drill as you can fit into the slot (either middle, one end, or both ends), then set up a narrow stepover, full depth high speed/feed path for a 1/2" or so vari-flute style four flute endmill. Rough to .020, change to a dedicated finish mill for a final pass. This could be a five or six flute finisher, let it wail...

Krovvax · May 23, 2015

Drop a 1/2 inch drill in the middle of the pocket and hsm the pocket with a 1/2 endmill and you should use around 3 endmill should be faster and time is money so worth the extra bit of $ in tools. Tools are consumable time should always be priority on a 300 pcs run. If the job take 3 hours less your endmill are going to be paid for.

Atomkinder · May 23, 2015

Drop the biggest drill you can in then rest machine with an HSM path. No point starting with a small drill and a larger one will give the chips somewhere to go. Get an air blast in there too.

shamanj · May 24, 2015

Deburr: just use a chamfer tool or a spot drill and just kiss the edges with a .2mm DOC on all edges so you don't slice yourself open on it. Being a handwheel sharp edges may bite.

Larry Dickman · May 24, 2015

You don't say what cam system you're using, but switch to an HSM like Optirough or Volumill. Use an 1/2" 5fl em, as a starting point, 5k rpm, 120 ipm, 12% stepover and .75 doc. No coolant. (air blast if possible) Your burr problem will go away as well.

jdj · May 24, 2015

YES! a drill is a "primative" tool, but still very efficient in the right area. After that, a variable helix type solid carbide end mill is very hard to beat!

Ukraine Train · May 26, 2015

Thanks for the suggestions. I use NX for CAM software, but still learning. I'll play around with it to get a HSM path. Where do you like to get your variable helix end mills? I think I've checked with my local shop supply place before and they didn't have these.

Rstewart · May 26, 2015

Carbide End Mills, Thread Mills, Thread Gages, Drills, Solid Carbide Thread Mills

https://www.maritool.com/

MotoX · May 26, 2015

I think you'll be fine with what you're using as far as tooling, I'll bet the problem lies in the workholding.Your pockets are right on top of where the parts are unsupported.

I used to run parts like this all the time, and like you i started with a 3 jaw chuck on its back and had loads of chatter.

If your parts are consistent O.D., then interpolate a circle into some thick softjaws in a vise like I did, and the problem should go away.

If you're careful, while its running, put your hand on the part and you can verify to a certain degree that it is the parts that's vibrating.

I do have to agree with everyone else though a salid carb em with a hsm toolpath would be superb, but i'm always used to making do with what i have.

my .02

chatter issues milling a pocket

Cast Iron

Plastic

Diamond

Diamond

Cast Iron

Titanium

Diamond

Diamond

Stainless

Hot Rolled

Cast Iron

Diamond

Hot Rolled

Titanium

Hot Rolled

Titanium

Diamond

Cast Iron

Stainless

Cast Iron

Similar threads