Trying To Surface 304 Stainless 6"x 4" x .500 thick

Gqunder · Oct 15, 2016

I'm trying to surface 6 x 4 x .500 with a face mill r8 shank with 5 carbides, It runs good for about 15 minutes the I get a galling and it seams to me the longer I work it the hotter it gets and the rougher it looks. 780-RPM Feed rate is as slow as I could go to as fast as I can go with a .010ths to .025ths depth of cut I just cant figure it out. I'm a new be so be gentle. Would a ly Cutter be a better tool ?

Finegrain · Oct 15, 2016

What kind of fluid? Gotta use something with 304 IME.

Regards.

Mike

Gqunder · Oct 15, 2016

I keep it coated with a cutting name brand ridgid is a dark brown threading and cutting oil

Milland · Oct 15, 2016

Sounds like you're using a Bridgeport-type mill, or weaker, and the lack of stiffness on both the machine and cutter body (3" face mill on R8 shank = flex) means that your carbide inserts are getting bounced off the material, rather than stably cutting. This breaks down the carbide edge quickly and results in dull surfaces rubbing rather than cutting, so heating up the part and leaving a bad finish.

Post some pictures of your setup so we can see the machine and how you're holding the part, and of the cutter and (ideally) a close-up of the damaged inserts. That should give us more info to help with.

Gqunder · Oct 15, 2016

Thank you for your post, I noticed ever thing you have mentioned special the part getting hot. I will post photos for my situation tomorrow.

Ries · Oct 15, 2016

my experience with 304 on a manual mill has been slow it way down. I have not found that carbide is worth it unless you have flood coolant- which my manual does not.
So I use HSS end mills, slow em down, and accept that my $5000 mill is never gonna give me the surface finish a $75,000 mill with flood coolant and 3 or 4 tons of mass will give me.
When 304 gets too hot, it gets hard. Then the carbide cutters degrade or chip, and HSS end mills burn.
Then you get galling and crappy surface finish.

I run 3/4 " end mills on 304 at under 200 rpm, to keep em from self destructing.

If you have a VMC with flood coolant, you can follow Machinery's Handbook feeds and speeds for carbide. If not, not.

rons · Oct 15, 2016

You are work hardening the surface.I suspect your depth of cut needs to be backed out. Depth of cut is the critical factor in what you are doing. I use a mist attachment when doing something like this. It makes a mess.

JRIowa · Oct 15, 2016

So many things wrong.

1. RPM CS for 304 is about 80 So (CS*4*4 for carbide) = 1280 RPM = 1280/Cutter dia.

2 Cutter dia Since you don't mention, I can't give RPM. With 5 inserts, I'm guessing over 3.5". Too big for a BP spindle, and should be running at about 350 RPM.

3. Inserts If you're using a .031R insert. you need to take at least a .031" DOC. What's the coating on your inserts and grade?

4. chip thickness Your feed controls your chip thickness which should be around 0.001" per tooth. Can't calculate without knowing cutter diameter and RPM

5. Flycutters are for hobbiest machinists that don't mind ruining there mills.

So, if you're running a BP or clone, you have too large a cutter running too high a speed with too light a cut at probably to slow a feed.
JR

apoc_101 · Oct 15, 2016

JRIowa said:
So many things wrong.

1. RPM CS for 304 is about 80 So (CS*4*4 for carbide) = 1280 RPM = 1280/Cutter dia.

2 Cutter dia Since you don't mention, I can't give RPM. With 5 inserts, I'm guessing over 3.5". Too big for a BP spindle, and should be running at about 350 RPM.

3. Inserts If you're using a .031R insert. you need to take at least a .031" DOC. What's the coating on your inserts and grade?

4. chip thickness Your feed controls your chip thickness which should be around 0.001" per tooth. Can't calculate without knowing cutter diameter and RPM

5. Flycutters are for hobbiest machinists that don't mind ruining there mills.

So, if you're running a BP or clone, you have too large a cutter running too high a speed with too light a cut at probably to slow a feed.
JR

Even if it were 3" tool, all bang on points. OP needs to refer to calculator such as FSWizard or to common sense for obviously overboard RPM and honestly, the wrong tool for the machine. Smaller tool and lower surface footage with help tremendously.

conant · Oct 15, 2016

This post is a duplicate of the first post where he mentions 3" cutter diameter.
Double post, different but similar.
Interesting.

specfab · Oct 15, 2016

"Trying To Surface 304 Stainless 6"x 4" x .500 thick"

Right there's yer problem.

stephen thomas · Oct 15, 2016

& yet people continue to insist "shapers are obsolete".

To the OP, if you don't have a shaper and if you do have a choice, the best choice might be to use a different stainless alloy.

smt

JRIowa · Oct 16, 2016

stephen thomas said:
& yet people continue to insist "shapers are obsolete". smt

They are!

But I'll bet you $0.10 that 90% of those on the board have never ran one. The last time I did was over 40 years ago.

As too some of the other stuff, 317 would finish nicer and it would probably be easier to run in a 4-jaw on the lathe. Even then, you need to know how to figure surface footage. BTW, with a 3" cutter should be about 430 RPM. I'd run dry.
JR

winger · Oct 16, 2016

What mill only goes down to 780 rpm?

rons · Oct 16, 2016

Gqunder said:
It runs good for about 15 minutes the I get a galling and

If you are cranking the feed by hand you won't get a good finish.

I have a Walter mill with 5 carbide inserts (8 sided) and use it on occasion. Like once every 2 years. I bought it about 14 years ago and I am still on the first side of the inserts. Last time I used it was to clean up the sides of a used Palmgren vise. I cut it dry and it came out looking new again.

On your small piece it should not be taking 15 minutes. Two passes down the length dimension is all I would do, like a two lane street. If I was new at this like you I would be taking as light a cut as possible for the first passes just to get a feel for things. And I would think less than a minute per pass with a power feed is all it would take.

Your mill head tram adjustment has to be the best you can adjust it, perpendicular to the surface of the piece to be cut down.

triumph406 · Oct 16, 2016

JRIowa said:
So many things wrong.

5. Flycutters are for hobbiest machinists that don't mind ruining there mills.

You don't know what your talking about

JRIowa · Oct 16, 2016

triumph406 said:
You don't know what your talking about

Fine, don't listen.
Just what makes you think that you do? Wait, you've been doing for 3 years and flycutting never hurt your mill.
JR

Spyderedge · Oct 16, 2016

A very small corner radius, generous geometry, and with a small diameter flycutter they can be used without damage to your mill with fine feeds and light DOC. A far as I'm concerned it's just a tool for finishing in aluminum. Also great for plastics.

Matt_Maguire · Oct 16, 2016

JR’s right you need to bury the radius, and at least shoot for 1/4Radius feedrate to have good tool life. Most millers are going to feed at least .008” per tooth with 304 & similar stainless. The little BP type mills won’t go where that 3” cutter needs to.

Some quick numbers, maybe starting a little low on speed by dropping down to 330SFPM makes for 420RPM for the 3” cutter… 5 teeth on the cutter going .008” per tooth makes for over 16IPM feedrate. Let’s call it 16…

NOW→ That makes for 80 turns of the handle per minute with a 2”(recommended) cut width (good luck with that). So you practice 20 turns every 15 seconds to get the feed feel right. NOW → you figure the .040 depth of cut you’d really like for tool life you find out the combination of speeds, depth of cut and feedrate you need 1.56HP at the spindle. Using the best SFPM of 425 makes for 540RPM and that needs 2HP. You can’t get there.

Good luck,
Matt

triumph406 · Oct 16, 2016

JRIowa said:
Fine, don't listen.
Just what makes you think that you do? Wait, you've been doing for 3 years and flycutting never hurt your mill.
JR

25 years, mill still ok, never heard any body ever say a fly cutter will hurt a mill, except you.

Trying To Surface 304 Stainless 6"x 4" x .500 thick

Plastic

Diamond

Plastic

Diamond

Plastic

Diamond

Diamond

Diamond

Hot Rolled

Stainless

Titanium

Diamond

Diamond

Stainless

Diamond

Diamond

Diamond

Titanium

Stainless

Diamond

Similar threads