PDA

View Full Version : sparks from a face mill?



Black Forest
09-26-2010, 08:16 AM
I was facing some cold rolled steel this morning with a 6" 10 insert carbide face mill. All was going well and then I started to get sparks. Lots of sparks.

I was feeding slowly and rpm's at 1400. What was wrong? I have done it the same way many times and no problems and great finish. I was just using compressed air for cooling and chip removal.

JoeFin
09-26-2010, 08:37 AM
Might not have had enough cooling because it sounds as if you hit a spot that was work hardened and you dulled some edges

Evan
09-26-2010, 08:55 AM
Assuming it was the equivalent of regular 1018 carbon steel even work hardening won't be enough to explain that. The most likely explanation was some sort of inclusion of much harder material which instantly took the edge off the inserts.

More important though is that you were running it much too fast. At 1400 rpm you are driving the inserts at over 2000 sfm. That is only a comfortable territory for Cermets and much too high for carbide. You should be running them no more than about 300 to 500 sfm at most which means 200 to 300 rpm.

Mcruff
09-26-2010, 10:16 AM
More important though is that you were running it much too fast. At 1400 rpm you are driving the inserts at over 2000 sfm. That is only a comfortable territory for Cermets and much too high for carbide. You should be running them no more than about 300 to 500 sfm at most which means 200 to 300 rpm.
Not to mention what size machine are using a 6" face mill on, this must be a decent sized mill to run that efficently.

J Tiers
09-26-2010, 10:45 AM
More important though is that you were running it much too fast. At 1400 rpm you are driving the inserts at over 2000 sfm. That is only a comfortable territory for Cermets and much too high for carbide. You should be running them no more than about 300 to 500 sfm at most which means 200 to 300 rpm.

+100

probably it was squeaking also.


I was feeding slowly and rpm's at 1400. What was wrong?

BOTH OF THESE are wrong.......

Evan has explained the 1400 end of things..... but the "feeding slowly"..... THAT is really bad also.

You have a 10 insert face mill.... at 1400 rpm, you had 14000 cutters passing the work per minute. Divide your feed per minute by 14000 and see what you get for a depth of cut per insert.

Carbide would want at least a thou or two per insert, maybe more....

if you were feeding at 2" per minute, 2/14000 - 1.4 TENTHS per tooth..... Carbide is not that sharp.

All you were doing was rubbing most of the time, with a cut maybe once every 10 or 15 teeth, when enough thickness of uncut built up due to feed.

Slow WAY down, and take a more aggressive feed per tooth, like 10 x more PER TOOTH, not 10x faster absolute. at 200 rpm, you have 2000 teeth per minute, so if you want to feed 0.002 per tooth, you must feed at 4" per minute.

Mcgyver
09-26-2010, 11:06 AM
RPM = (CS x4 ) /Dia. Write it on the wall.


Not to mention what size machine are using a 6" face mill on, this must be a decent sized mill to run that efficently.

+1

Then you get guys that calculate speed and feed properly, and set DOC to a removal rate the machine can handle.....100 passes .005 thou sort of thing.

To maximize tool life there has to be the right balance between feed speed DOC and machine/set up rigidity and horsepower. This is where the so called calculators fail; they can't judge rigidity and most don't have horsepower function.

Not to say you shouldn't doing what you're doing BF - great finishing cut might all you're after, it's just a general common on guys newer to it trying to figure out the cut

wierdscience
09-26-2010, 11:29 AM
At that speed and feed if you where taking a light DOC those wern't sparks,but the swarf glowing yellow.Like others have already said 1400 rpm on that face mill is way to fast by a factor of at least three.

400-600sfpm is the happy spot for most inserted carbide tooling I use.That means a 6" face mill should see 250-380 RPM.

DOC would be whatever you have the HP and rgidity for and feedrate would be 7.5-11.5 ipm at a .003" per insert chipload.

Coolant,either none(dry machining) or flood.Intermitant coolant is the second worse thing you can do to insert carbide right behind re-cutting chips.

Black Forest
09-26-2010, 11:30 AM
OH Oh OH, I guess I had that all figured wrong! Expensive lesson. I ruined 300 dollars worth of inserts. Unless you think the heat didn't ruin the other corners? Meaning somehow diminished the carbide for cutting.

I was doing this on a big horizontal mill. Plenty of power and very rigid. It weighs two metric tons. About 4500 lbs.

Liger Zero
09-26-2010, 12:16 PM
Flip them over and see if they work. Nothing ventured nothing gained. Odds are they'll be fine.

bobw53
09-26-2010, 12:21 PM
Some sparks is normal, lots of sparks isn't.

This was busting through a weld, I had already written off the inserts. Besides, it looks cool.
http://farm3.static.flickr.com/2078/3534587737_e5c6c72565_z.jpg

Black_Moons
09-26-2010, 01:29 PM
Last time I had sparks and 'dull thuding sounds' while turning a square thing round.. It was because my brazed carbide tool had developed a 1/32 or so radius on the cutting edge... The bad way. (Rake to front relief radius! ie 0 sharpness).. Yea... Dull thuding sounds.. Thud thud thud. Caused by a dull thuding tool.. who would'a thunk it?

Tool edge was of course very badly damaged, And I even managed to strip a bolt that holds my compound to my lathe due to the forces (likey was overtight and chinese swiss cheese steel to start with)

Sparks are generaly bad if you don't know why they are happening... as is using a dull tool.

whitis
09-26-2010, 01:53 PM
Kennametal has some useful calculators
http://www.kennametal.com/calculator/calculator_main.jhtml
They do consider horsepower. They don't consider rigidity but they do give the tangential cutting force.

Evan
09-26-2010, 03:18 PM
The other corners will be fine. Heat doesn't hurt carbide tooling. Otherwise brazing carbide tools would destroy them and it doesn't.

If you like sparks then try cermet or CBN inserts. :D

Machining a bearing race:

http://ixian.ca/pics6/cermetfun3.jpg

j king
09-26-2010, 03:44 PM
love the clear pic Evan.

Evan
09-26-2010, 07:11 PM
I consider that to be one of the best machining pictures I have taken. It just turned out perfectly.

recoilless
09-27-2010, 01:34 PM
Appears that OP has figured out the issue. My first thought was it could have been running in reverse. I did that with a flycutter ...twice hopefully never again. Lot less $ I spent cause of mistake.

Black_Moons
09-27-2010, 01:55 PM
Appears that OP has figured out the issue. My first thought was it could have been running in reverse. I did that with a flycutter ...twice hopefully never again. Lot less $ I spent cause of mistake.

My friend did that on my lathe... Except it was verus UHMW plastic and the tool had a giant relief so it was just like '...Huu?'

Black Forest
09-27-2010, 04:29 PM
No I haven't figured it out! I did not have any time to remount the inserts and indicate them in yet. It takes a while to set this face mill up. I hope to have time on Tuesday.

airsmith282
09-27-2010, 04:39 PM
i have had no issues with carbide cutter on my fly cutter at 400 to 460 rpms on SS or mild steels,1400 or faster is great on aluim, and nope no coolent needed even on the steels

have tried some unknow steels prettyhard stuff but even 400 to 460 was still good to run on with carbid,,if if your taking to deep of a cut that can go bad on hi speeds or speeds over 500 rpm

Mcgyver
09-27-2010, 04:49 PM
i have had no issues with carbide cutter on my fly cutter at 400 to 460 rpms on SS or mild steels,1400 or faster is great on aluim, and nope no coolent needed even on the steels

That doesn't tell someone much; it might be too fast, might be too slow. Its surface speed that matters, its such and such a diam at so many rpms that determines surface speed.

what's the surface speed?

Evan that is a neat pic, makes me want to get a chunk of your floor and go turn some bearing races :D

Black_Moons
09-27-2010, 05:01 PM
Mcgyver: Previous experiance with him tells me airsmith does not believe in SFPM, Only RPM :(

Its a lot like trying to tell how fast your car is going by looking at the engine RPM.. And in this case, trying to tell someone else the speed limit by telling them thier engine should run at '400 to 460 rpms'.

Really does not work without knowing the exact ratios of the transmission and what gear you are in. Its KPH/MPH (SFPM) that matters allways, Not the RPM, RPM alone is incomplete and hence worthless information.

Evan
09-27-2010, 05:56 PM
makes me want to get a chunk of your floor and go turn some bearing races

I actually took a chunk of the Corundum aggregate and ground it to a tool shape with my large diamond wheel. It worked on mild steel not too bad but was very fragile on the edge. Not enough cobalt binder I guess... :D