Trying chamfer mill vs conventional coutnersink today, any tips?

Tap_or_Die · Feb 2, 2016

So we have been running stainless angle for a while now. Only in the last year we started running them on a cnc mill. The one issue we have had is the countersink just doesn't last, and I dont think its the tool, or program. The machines is just to small to run tough material (the countersink will wobble in the collet during cutting, also x and y axis show heavy loads). So I decided to decrease the pressure by trying a chamfer mill. This will be the first time using one so I'm just fishing for some tips on how to run these. My first thought is to use a helical interp and finish at the bottom.

1/8" x 2" ss angle, 5/16 through hole, need to countersink 82deg to 1/2". Tool is a accupro, 3/8, 4 flute, 82deg, TiCN coating. I know, accupro is not all that great, but ive had some good luck with them and as a test run, I wanted to try a cheaper tool before going all out.

Mtndew · Feb 2, 2016

Tap_or_Die said:
I know, accupro is not all that great, but ive had some good luck with them and as a test run, I wanted to try a cheaper tool before going all out.

Accupro isn't bad, they have some really good stuff for the price. Chamfer mills are all I use because they are so versatile and when they get dull or chip I just have my cutter guy resharpen them and recoat them. They last years unless you smash them.
Interpolating would be your best bet in the stainless, but I would try just plunging unless you get too much chatter.

Tap_or_Die · Feb 2, 2016

Really, you think plunging would work? At what rpm? If I interpolate its gonna be at 150-225 sfm and .001 per tooth...

Atomkinder · Feb 2, 2016

What's the stainless alloy? 303 isn't going to machine like 304 for instance.

I'd still interpolate. In my experience chamfer mills don't have the relief behind the cutting edge for a plunge move in more difficult materials.

I'd probably start around 250SFM (depending on alloy) and .002 chipload and go from there. Chamfer mills are pretty tough.

Mtndew · Feb 2, 2016

I would try the same sfpm for plunging, and adjust from there based on how it sounds

michiganbuck · Feb 2, 2016

Collets are noted for not holding well. Coutnersink operation is often a wide chipload. Weldon shank and a endmill holder might be better.

Tap_or_Die · Feb 2, 2016

Its 304. Ill try to interpolate for now.

Tap_or_Die · Feb 2, 2016

What about the depth per pass, z-.025 or less?

adama · Feb 2, 2016

What had you been using as a countersink? I personally switched to the MA ford single flute ones for stainless countersinking, the single flute removes a lot of the tourqe requirement and they seam to have there cutting angles + clearances just right. Some of the other single flute countersinks i have tried in the past have been crap to say the least very grabby and matching what you describe. A 3/4" od MA ford single flute countersink in 316 is easy on the Bridgeport to full dia, its hard doing the same with pretty much any other 3 flute or single flute one i have tried.

Have had mixed luck with chamfer mills, especially for countersinking. Its real easy to be takeing too big a chip on a small hole + big tool type job and they don't clear, just jam up and shatter. Not such a issue with the small chips of going along a edge, but milling what you describe and its real easy to end up with more than 180 degrees of engagement and minimal chip escape space coupled with zero flute spiral letting the swaft escape and bad things happen fast!

Tap_or_Die · Feb 3, 2016

adama said:
What had you been using as a countersink? I personally switched to the MA ford single flute ones for stainless countersinking, the single flute removes a lot of the tourqe requirement and they seam to have there cutting angles + clearances just right. Some of the other single flute countersinks i have tried in the past have been crap to say the least very grabby and matching what you describe. A 3/4" od MA ford single flute countersink in 316 is easy on the Bridgeport to full dia, its hard doing the same with pretty much any other 3 flute or single flute one i have tried.

Have had mixed luck with chamfer mills, especially for countersinking. Its real easy to be takeing too big a chip on a small hole + big tool type job and they don't clear, just jam up and shatter. Not such a issue with the small chips of going along a edge, but milling what you describe and its real easy to end up with more than 180 degrees of engagement and minimal chip escape space coupled with zero flute spiral letting the swaft escape and bad things happen fast!

I tried a few different countersinks, the latest was a 1/2 solid carbide hertel single flute, 3/8 shank. It worked for about 20 parts then started to chip on the cutting edge. I think the machine was just to weak, it started to wobble and the table showed more load every part. Then i seemed the table would move just a little which is what I think caused the tool to chip

I got a good part yesterday and ill post a pic soon...

michiganbuck · Feb 3, 2016

One trick if you have grinding ability is to circle spin the angle, then back the clearance at perhaps 10* but only go perhap .007 deep then roll the rest of the clearance round..Yes play with the depth till you shave the right amount for the job.

Rstewart · Feb 3, 2016

I interpolate almost every countersink I do, maybe not in Aluminum. In stainless it's a no brainer to me.

Maritool makes some nice coated chamfer mills.

Tap_or_Die · Feb 3, 2016

Here what she looks like, Id say the finish is fairly nice and the machine took the cut well, we will see how long it lasts...

Tap_or_Die · Feb 12, 2016

We are at 160 holes and counting.

Tap_or_Die · Feb 19, 2016

Okay, so we finished the run with 552 holes done. Thats .38 cents per part for the tool, and labor was cut from .5 hours to .15 hours per part. I believe the tool has payed for itself and more. It did develope a small chip on the tool, however I believe it was from operator error,( coolant was knocked off target), he didn't catch it in time....

jbifs · Feb 19, 2016

Personally, I have just sharpened a drill bit to 82 degrees. I have tried fancy countersinks, but at the end of the day simply using a drill bit does the job just as fine minus the finish. Reason why I use drill bits is because I often need have holes that are counterbored 1/8" + the 82 degree countersink. Instead of thru drilling, tool change to endmill to counterbore, tool change to countersink...

Search

Largest Manufacturing Technology Community on the Web

Search

Trying chamfer mill vs conventional coutnersink today, any tips?

Tap_or_Die

Cast Iron

Mtndew

Diamond

Tap_or_Die

Cast Iron

Atomkinder

Titanium

Mtndew

Diamond

michiganbuck

Diamond

Tap_or_Die

Cast Iron

Tap_or_Die

Cast Iron

adama

Diamond

Tap_or_Die

Cast Iron

michiganbuck

Diamond

Rstewart

Stainless

Tap_or_Die

Cast Iron

Tap_or_Die

Cast Iron

Tap_or_Die

Cast Iron

jbifs

Aluminum

Similar threads