Wasting time and money - milling advice needed

empee · Jan 4, 2011

Hi ,
I have 14 solid stainless bars (316) bars of approximately 1 inch square that need machining down to approx 7/8 inch square.
They are approximately 6 feet long.

I have a bridgeport type mill and have purchased a 6 tooth face mill (4 inch dia) to machine 4 pieces simultaneously - i have made clamping nests to cater for this.
Picture / details of cutter -
https://www.machineryhouse.com.au/Products?stockCode=M518
Problem is I am finding that I am struggling to cut even .040 deep without having the tips wear too quickly. I am running coolant and 140 rpm approx and with slow auto feed.
Can anyone give me better advise on rpm and feed rates ? Or any other tips ?This is proving to be a very tedious job. Any feedback would be appreciated.

Cheers Mark in Oz

kpotter · Jan 4, 2011

I have the same cutter but in 3 inch I run it on a 7.5hp K&T I run 400rpm 3inches a minute no coolant through mild steel at about 3/16 of an inch full depth and the inserts last forever I do this for hours a day and run pallets of parts. I think you need a bigger mill or a smaller cutter and you need to increase feed, to stay under the hardened surface but I dont think you have the HP . stainless is nasty 303 is nice but 316 will work harden and that is why you are tearing through inserts. Try cutting one at a time in one pass and keep the feed up dont back off.

John Welden · Jan 4, 2011

Oh boy....that's a really harsh job for a Bridgeport. It's like towing a heavy trailer with a small car. That cutter is made for a modern machine with ridgity and horse power and you don't have either. You'd probably be better off doing one at a time with a smaller tool. The designers of the BP didn't have this sort of job in mind. It's a fairly light duty machine.

HuFlungDung · Jan 4, 2011

Perhaps if you mill only 3 or 2 bars at a time, you will get longer tool life. When you mill a 4" width with a 4" diameter tool, you've got a very thin chip at the entry and the exit, and this tends to roll over (instead of cut) which produces extra rubbing and heat. The hot stainless has a greater inclination to weld to the insert, which can lead to premature coating failure. A fairly aggressive feed (like maybe .005" per insert) would also help get the edge of the insert under the chip which helps preserve the very edge.

Bruce Nelson · Jan 8, 2011

If you have the 4 inch cutter centered on the bar, your cutter will hammer on your Bridgeport because only one cutting tooth is in contact at a time. If you move the cutter off the center of the work you can get two or more cutting teeth in contact with the work at one time, which should eliminate the hammering. If you center the cutter as far off the edge of the work as possible, your chip entry will be thin, and you should be able to run at a much higher feed rate.

mrainey · Jan 8, 2011

If your machine will take it, maybe double the RPM with feedrate in the 7-10 inch per minute range. I'd also try turning the coolant off.

PixMan · Jan 8, 2011

mrainey said:
If your machine will take it, maybe double the RPM with feedrate in the 7-10 inch per minute range. I'd also try turning the coolant off.

+1

That's what I'd try. You're probably shortening the insert life through thermal cracking if not flank wear from too slow of a feed rate. Perhaps both failure modes at work there.

InnovativeMach · Jan 8, 2011

I'd definetely try upping the RPM. The new tooling is pretty amazing and most often people run them too slow. It's going to beat the bridgeport pretty badly though.

PixMan · Jan 8, 2011

InnovativeMach said:
... It's going to beat the bridgeport pretty badly though.

Sorry, but I totally disagree. Those cutters (I have something similar) cut like butter when you run them right.

oldbrock · Jan 8, 2011

ditto Arainey

Boris · Jan 8, 2011

Chucking a few numbers into my trusty number cruncher yields a RPM of about 400-500 rpm and try a feed of about .1mm /tip

Keep the b/port in low gear , dont try and use the high gear
Use no coolant, but if you can rig up an air blast it will help( I used to empty the mist coolant system of coolant and use that)

If it starts to struggle, reduce the number of bars you are cutting and use the soft entry method of cutting

Mind which way the chips will be coming out as they will be hotter than an aussie cricketer being roasted by the media

Boris

Mike C. · Jan 8, 2011

It's a Bport copy. Undoubtedly, it has a servo type table feed. He has no way of calculating and setting chip load. If he does calculate table feed by stopwatch or similar, it will change if the feed rate is set without the cutter working, as the motors are so small that they load up and slow down under a load, especially one heavy enough to give .005" per tooth. 4" is a mighty big cutter to be dogging a BP copy in 316. I think I'd definitely drop back to two bars instead of trying to go the whole four in one bite, will lower HP requirement severely. I don't have my hp required calculator here at home, but I think you would find 4", full depth in 316 to be over 3hp, with is likely all the mill has, if that much.

adama · Jan 8, 2011

Generally i would be running something like that only 3 up on a 4" cutter. On the Bridgeport i would go as slow as it goes in high speed. Cutter would ideally overhang about 3/4" on clockwise side and clear by about 1/4" on far side of cut to avoid any rubbing issues (its a really important point on any alloy - work hardening material). You don't idealy want edge of the insert entering the work first, it will rapidly break the edge down. Same when leaving, if it does a full swing the chip gets thinner and thinner, eventually turning into near a rub, very fatal for inserts on stainless. Depth of cuts what ever comes first - finished size or rigidity issues. Feed make sure your taking a cut on every insert, forget the insert makers spec as i doubt your going to get near that on a Bridgeport, but make sure every tooth is taking over 1 thou, ideally more. If possible only cut the 2 sides you have too, don't try and remove the other 2 - keeping every side even unless its the requirements of the job. Stainless always has a bit of a work hardened skin to it.

S_W_Bausch · Jan 8, 2011

I am afraid to say this, but...

The assumption is the head is exactly perpendicular, right?

If the head hasn't been trammed, and the cutters are entering at an angle, would that be troublesome?

Or am I missing something?

(and this would be better done in a horizontal mill, correct?)

jdj · Jan 8, 2011

S_W_Bausch said:
I am afraid to say this, but...

The assumption is the head is exactly perpendicular, right?

If the head hasn't been trammed, and the cutters are entering at an angle, would that be troublesome?

Or am I missing something?
)

You aren't missing anything! That is definitely something worth checking.

Jeff

jdj · Jan 8, 2011

Carbide grade is a very important factor. The best two types that I have seen (for 316 SS) are Mitsubishi US735 and F620. Hopefully someone has some other grade recommends?

Jeff

register · Jan 8, 2011

Mike C. said:
It's a Bport copy. Undoubtedly, it has a servo type table feed. He has no way of calculating and setting chip load. If he does calculate table feed by stopwatch or similar, it will change if the feed rate is set without the cutter working, as the motors are so small that they load up and slow down under a load, especially one heavy enough to give .005" per tooth. 4" is a mighty big cutter to be dogging a BP copy in 316. I think I'd definitely drop back to two bars instead of trying to go the whole four in one bite, will lower HP requirement severely. I don't have my hp required calculator here at home, but I think you would find 4", full depth in 316 to be over 3hp, with is likely all the mill has, if that much.

Agreed on the need to reduce HP requirement. Try two or three bars.

As for the feedrate, I'd be interested in a rough estimate of what feedrate you have been running. Modern inserts don't always feel "right" in the same way that HSS tools do. If at a 0.001-0.002 i.p.t. feedrate you are likely rubbing your inserts to death. Letting the tool take a proper "bite" can do a good deal in terms of stabilizing the cutter while in the cut and reducing chatter.

Henry

stephen thomas · Jan 8, 2011

Every time I read a post like this I say a little prayer of thankfulness for that "obsolete" planer holding down an oily patch of concrete in my shop.

And it will run darn near unattended! :smoking:

smt

Steve Seebold · Jan 8, 2011

Find someone with a BIG Blanchard grinder or a double disc grinder and just have them ground. It will save you a lot of aggrivation.

77ironhead · Jan 9, 2011

empee said:
/snip/
I have a bridgeport type mill and have purchased a 6 tooth face mill (4 inch dia) to machine 4 pieces simultaneously - i have made clamping nests to cater for this.
/snip
Cheers Mark in Oz

care to elaborate on 'clamping nests'?
are you running 4 bars separated by a gap between each, or are you running 4 bars all clamped together into one big slab (effectively turning them into 1 bar)? If you're running with a gap in between each bar, that will be part of your problem- inserted tools aren't real happy with an interrupted cut.

Wasting time and money - milling advice needed

Plastic

Diamond

Diamond

Diamond

Stainless

Stainless

Diamond

Plastic

Diamond

Hot Rolled

Titanium

Diamond

Diamond

Diamond

Diamond

Diamond

Hot Rolled

Diamond

Banned

Titanium

Similar threads