I've moved up from running prototype 420 stainless in a Haas VF2 to running production 6061 in a bunch of Makino a51's. I'm countersinking larger holes (3/4-1-1/2) and QC has asked me to look into chatter marks. It seems they've been running 6 flute countersinks, which from what I believe we should be running 3 flute or less? Hoping the less cutting edges it has the less the chatter will be. Any input is always appreciated.
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Countersink chatter
- Thread starter Plouch16
- Start date
- Replies 38
- Views 9,608
Joe Miranda
Titanium
- Joined
- Oct 19, 2004
- Location
- Elyria Ohio
If you are plunging (which it sounds like you are) you cannot run a countersink slow enough. Even in aluminum I would be between 40-50 sf. If you have the option of interpolating that is hands down the best way to go.
Yes I am plunging. The problem is on some of the pallets there are 64 holes that might get countersunk on a face. Interpolating will increase cycle time exponentially. I'm still new to their cam software, but it seems they run their 3/4 at 2340 rpm @ 49 z feedrate. I know it is entirely too fast, but the change in chatter vs added time may not be worth it to them.
mjk
Titanium
- Joined
- Oct 20, 2005
- Location
- Wilmington DE USA
Agree with above about to fast
I'd try adjusting speed down manually to see if you get an improvement.
That won't change your cycle time, but I wouldn't be surprise if a 6 flute loaded up with 6061 material
I'd try adjusting speed down manually to see if you get an improvement.
That won't change your cycle time, but I wouldn't be surprise if a 6 flute loaded up with 6061 material
I'd drop the "0" off of your 2340 rpm and run 234. Decreasing the rpm won't slow down a ipm machine at all.
What he ^^^ said. Surprised it's not kicking up a big Ole nasty honking burr too.
Brent
Scottl
Diamond
- Joined
- Nov 3, 2013
- Location
- Eastern Massachusetts, USA
My experience, strictly on manual equipment, is that 6-flute countersinks tend to be very prone to chatter on some materials.
Always used a single flute on the bridgeport at the old shop, and even on the Haas machines. Figured that's the way I am headed.
Eeeeuw. Get rid of the damned six-fluters. Those never work for shit. ONE flute is plenty. Agree with others on speed as well.
G
Guest
Guest
The go to first fix for chatter as others said is to drop the RPM, no matter what the operation.
Bobw
Diamond
- Joined
- Feb 8, 2005
- Location
- Hatch, NM Chile capital of the WORLD
Big countersinks are never fun..
I've had some success with the 6 fluters by grinding off 1 or 2 flutes, say #1 and
#3, turn it into a variable flute tool. Sometimes that will dampen out the
chatter.
A makino huh? I bet she can interpolate pretty darn well at a high feed rate..
If I were you, I'd get my hands on some chamfer tools (Maritool has some nice
double enders), and let it rip. Depending on the size of your chamfer, you
can feed the hell out of them and still get a nice chamfer. I'd guess you
could get close to the cycle time you are running now, and get a better product.
I've had some success with the 6 fluters by grinding off 1 or 2 flutes, say #1 and
#3, turn it into a variable flute tool. Sometimes that will dampen out the
chatter.
A makino huh? I bet she can interpolate pretty darn well at a high feed rate..
If I were you, I'd get my hands on some chamfer tools (Maritool has some nice
double enders), and let it rip. Depending on the size of your chamfer, you
can feed the hell out of them and still get a nice chamfer. I'd guess you
could get close to the cycle time you are running now, and get a better product.
The man who held my position before me had no machinist experience, so he ordered what he thought would work best. Currently this is what they are running, but that will be changing next month as I am taking over tooling. Small changes such as a different countersink are easy enough to go along with from the upper management.
They are extremely fast, especially coming from those VF2's and VF4's. This is something I want to look into further down the line, as I've only been here for over a month, and would not like to make any large changes until I'm settled in.
Finegrain
Diamond
- Joined
- Sep 6, 2007
- Location
- Seattle, Washington
Agree with running it as a chamfer op, maybe take depth cuts.
Or, plunge with the horrible 6-flute to within .005", then just take a quick swipe with a chamfer tool to final Z.
Regards.
Mike
Or, plunge with the horrible 6-flute to within .005", then just take a quick swipe with a chamfer tool to final Z.
Regards.
Mike
toolmaker96
Hot Rolled
- Joined
- Jul 9, 2003
- Location
- Carson City, Nv. USA
Change to a chamfer mill & interpolate
mhajicek
Diamond
- Joined
- May 11, 2017
- Location
- Maple Grove, MN, USA
These chamfer mills work great for me in 17-4 and Ti:
Helical Solutions - Chamfer Mills - Helical Flute, 3 & 5 Flute - High Performance
Helical Solutions - Chamfer Mills - Helical Flute, 3 & 5 Flute - High Performance
Captdave
Titanium
- Joined
- Sep 24, 2006
- Location
- Atlanta, GA
That is still way too fast, maybe 300-400 RPM 500 tops.
mjk
Titanium
- Joined
- Oct 20, 2005
- Location
- Wilmington DE USA
Makino a51's + "The man who held my position before me had no machinist experience"
That could have been nasty
That could have been nasty
G00 Proto
Hot Rolled
- Joined
- Feb 18, 2013
- Location
- Dirkdirkistan, ID
I make countersinks one of three ways... if I have the right size, I prefer an 82 degree center drill (I never spent anytime thinking about it, but I think the leading drill stabilizes the cut and they have two deep gullet flutes); I will interpolate or helical plunge with an 82 degree chamfer mill; or if I absolutely need the right size the first time, I surface the countersink with a ball or bull endmill.
I bought a set of 82 degree 6 flute MA Ford countersink tools...broke one, threw away the rest.
I bought a set of 82 degree 6 flute MA Ford countersink tools...broke one, threw away the rest.
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
What spindle rpm you have? I would run a 3-4 flute chamfer endmill as fast as your rpm allows and go at it.
