question about face milling

rodney1 · Nov 9, 2006

I am having a problem with a 2 in. face mill. I am running a vtc200b mazak. The plate is a36.
20in wide by 24in.long running 1880 rpm with a 015 feed rate. I am having to index about every hour. Taking a 080 depthof cut and a 1.25 step over. the cutter is a 3 insert 8side positive optimill. Can anyone tell me what is wrong??
I dont get across the plate but one time and the load meter starts to climb.

car 84 · Nov 10, 2006

How deep is the total depth of cut because these numbers sound good. Things that may help are cut deeper per cut getting under the scale,adding clamps to raduce vibration and cut one direction making all cuts climb cuts.

fpworks · Nov 10, 2006

A couple questions/concerns that I have, but you may have already considered:

-are any of the edges of the workpiece flame cut?

-may I assume you are starting your cut outside of the part, where you don't have to plung/ramp through the scale? (to minimize scale cutting)

-are you using coolant? Probably not a good idea here.

rodney1 · Nov 10, 2006

Yes the edges are flame cut, yes the cut is from the outside. The depth of cut is .080 I have a 2 in. thick plate set on a angle and am taking a total off the small end of 1.188 and the big end is .187

fpworks · Nov 10, 2006

If your cut is taking your inserts through any flame cut regions/edges, that is undoubtedly a cause for killing off your inserts.

If possible, cut off the flame cut areas with a saw, then machine.

If that isn't possible, it may be worth it to reduce your speeds substantially through the flame cut regions, as your insert's cutting parameters for A36 don't apply here.

Gary E · Nov 11, 2006

Save your self a lot of time, money and agravation and have that plate Blanchard Ground.

And ohh when was anything 2 inches dia called a "Face Mill" ??

pepo · Nov 12, 2006

I learned a long time ago to get torch cut hot roll plate at least normalized. Blanchard grind to clean is usually a wise choice to get the bark off the faces. If you dont have this done it can be a lot of work and money just to get down to the steel. You know the steel is in there but its got this Kryptonite skin on it.

oops · Nov 26, 2006

You should look at feed milling that part. I'd use a 2.5 inch Iscar style feed mill. For the Vtc 200B you should be able to run a .04 DOC at 500 to 650 SFPM at .04 chip per tooth for a total feed per rev. of .160 .

Using about a 2 inch step over you'll get small ridges about .03ish high but that'll be no problem for a 4' facemill to clean off when you do a finish pass. No coolant on those feedmills. You'll get far better life from the feedmill inserts and your finish tool inserts will keep their corners for finishing at around a .015 -.02 DOC.

I think you'll clean that face off much quicker this way.

Search

Largest Manufacturing Technology Community on the Web

Search

question about face milling

rodney1

Plastic

car 84

Plastic

fpworks

Stainless

rodney1

Plastic

fpworks

Stainless

Gary E

Diamond

pepo

Hot Rolled

oops

Plastic

Similar threads