Speed and Feed to reduce chatter marks in a 2.75 inch depth?

gmoushon · Aug 8, 2020

Having trouble eliminating chatter marks in a deep pocket.

Material is 6061. Final depth is 2.75 inches.
Using a 1/2" 6-flute HSS end mill with 3 inch flute length.
Pocket geometry is 0.6 x 1.075.
Machine is a Kitamura MyCenter0. BT30 spindle.

I first hog the material out by drilling and then rough it with the end mill leaving 0.010 for a finish pass.

I've tried multiple combinations of speed/feed and still end up with chatter marks.

I also have a 11.5mm carbide 4-flute end mill that I could use if that would be better. Also wondered if conventional cutting on the finish pass would help?

Any help would be much appreciated.

gm

michiganbuck · Aug 8, 2020

could be how the part is held..

fmari --MariTool- · Aug 8, 2020

Way too many flutes in the cut. A 3 fluter would be best.

gmoushon · Aug 8, 2020

fmari --MariTool- said:
Way too many flutes in the cut. A 3 fluter would be best.

Don't have a 3-flute on hand and I'm trying to finish the job this weekend. I do have a 1/2" 2-flute high helix HSS but I thought it would be less rigid and thus lead to more chatter. Is my thinking wrong?

gmoushon · Aug 8, 2020

michiganbuck said:
could be how the part is held..

I think its being held ok... using 4" high 1" thick aluminum vise jaws.

EmGo · Aug 8, 2020

gmoushon said:
Don't have a 3-flute on hand and I'm trying to finish the job this weekend.

Then slow it down as much as you can and increase the feed as much as you can .... and too bad they don't make the good tap magic anymore, it was sometimes helpful in this situation.

Bobw · Aug 8, 2020

I was going to say get one of Franks necked back 1/2" endmills, you can stick
those suckers out a mile and never have a problem. BUT.. I understand Monday
deliveries, and you got what you got right now, and its got to work..

3" of flute on a 1/2" endmill is always a bitch, always. HSS just makes it worse.

One trick I like. Give the bottom of the endmill something to do. Its like
a little kid, if it doesn't haven't much to do, it'll bounce around and scream
at you.

Leave a little step at the bottom, maybe .060 to .080 wide and .100 or .150 high and
take it out on your finish pass. Gives the endmill something to do besides
scream at you. Alternatively, shallower and wider, maybe .050 deep, .200 wide.

gmoushon · Aug 8, 2020

Bobw said:
Leave a little step at the bottom, maybe .060 to .080 wide and .100 or .150 high and
take it out on your finish pass. Gives the endmill something to do besides
scream at you. Alternatively, shallower and wider, maybe .050 deep, .200 wide.

Thanks. That makes sense. I'll give it a try!
gm

SpeedsandFeeds · Aug 8, 2020

Are those oblong holes on the side already machined prior to cutting the operation? If so that certainly is not helping. Relieving the endmill to about .600 flute length and spiraling from the top down may help to.

BT Fabrication · Aug 12, 2020

ya id say, even my 4 flute likes to clog on aluminum.
i use a 2 flute all the time. if worried about the finish. leave a bit of meat, rough it out with any carbide mill, leave like 20 thou, switch end mills to a long one and do a finish pass.

HSS works on aluminum, but is super abrasive, I like bare carbide for that reason. it stays sharp longer.

Wsurfer · Aug 13, 2020

Fwiw,
I just did something similar on my brother , standard bt30. 4x4 x 3.1" deep pocket
In 6061.
Step 1 .5" 3 flute yg1 2" loc goung down 1.9" below model top"
Step 2 .625 necked 3 flute yg1 hanging 3.25" from face of collet nut in er32 (maritool) in .5" step downs. Left .01" on the wall.
Step 3. .5" necked 3 flute Maritool hanging 3.2 from face of collet nut er20 (Maritool). Ramped down .4" steps on wall with a finish pass @ 140 ipm taking .01 woc.

Sounded good and came out nice. You can barely feel any lines/steps and no chatter marks.

Edit. All cuts at 10k rpm

Bobw · Aug 13, 2020

Step 3. .5" necked 3 flute Maritool

Those necked back endmills are the bees knees.

ChipSplitter · Aug 13, 2020

Bobw said:
Those necked back endmills are the bees knees.

You sure that's not just a bunch of malarkey..???

Bobw · Aug 13, 2020

ChipSplitter said:
You sure that's not just a bunch of malarkey..???

Now you’re on the trolley!

Hardplates · Aug 13, 2020

Surprised no one has said ditch the HSS and go with carbide, its stiffer and better for long stickout. Anyway ditch the HSS. Yes lots of flutes can pack with chips in aluminum but I don't do much aluminum so when I do I often use tools made for SS, tool steel and Nickle alloys. They work just fine provided I keep the radial enjoyment low.

litlerob1 · Aug 13, 2020

Bobw said:
Now you’re on the trolley!

Don't compliment him Bob. I'm still tryna run him offt.

R

BSCustoms · Aug 14, 2020

if you get stuck again and don't have access to properly relieve your tool just buzz back the cutting edges on a pedestal grinder to make it like the relieved neck cutters. spiral down in.

also in a super pinch with a two flute, take a full flute off. one flute has a hard time chattering.

dandrummerman21 · Aug 14, 2020

I am surprised nobody asked: what rpm and feedrate are you trying to use?

The suggestions are mostly sound, but if we find out that you're running some high rpm, we'd mostly suggest to start there.

Nothing wrong with going 500rpm (or even less!) if it gets the job done.

Speed and Feed to reduce chatter marks in a 2.75 inch depth?

Cast Iron

Attachments

Diamond

Titanium

Cast Iron

Cast Iron

Diamond

Diamond

Cast Iron

Aluminum

Titanium

Cast Iron

Diamond

Titanium

Diamond

Stainless

Diamond

Cast Iron

Stainless

Similar threads