A36 steel Machining

[Mr. Wizzard]

yeah, so we have some A36 steel pieces, pretty small. Only using drill, 3/8 carbide endmills, and 1 small (.078) endmill. It seems to cut worse and wear tools faster than 1018. Is there a trick or any tips you guys have?

 

TIA!!

[Goldorak]

get better tooling or check the feed and speed

 

we cut a lot of this stuff , basically it's the same thing as a 44W plate or 1020 steel

 

we never got a single issue with tool wear

[Josh T™]

A36 should cut like butter. Don't let your SFM get to high and keep the chipload up. For the 3/8 Drill (depending on the MFG) I'd run it around 300 SFM @ 0.007 IPR. That should drill 1000+ holes in A36 with no problems.

 

HTH

Josh

[K2csq7]

Do you have a specific problem, or is it just generally bad....

 

Are you going through some scale or something? This stuff should be easy.

[Mr. Wizzard]

Current specs:

 

.531 drill: 120 SFM, 870rpm, 5.0ipm

.375 4-flute Onsrud EM, 400SFM, 4080rpm, 51.0ipm, .003fpt

.375 6-flute Onsrud EM, 400SFM, 4080rpm, 76.0ipm, .003fpt

[Mr. Wizzard]

Maybe not too bad. I've run 60 or so parts, but not much material removed. I'm thinking they should last longer, maybe it's fine.

Don't like the finish particularly.

Going thru the outside crappy scale.

The "Purchasing" people had the choice of 1018 or A36. I would have preferred 1018, never had a problem with it. This stuff just seems not as friendly in terms of tool life or finish.

[K2csq7]

Crappy material = bad finish

Crappy Scale = chipping your end mills

 

Don't think your going to get good finishes or better tool life unless this is a really high qty. job that you can spend a bunch of time tweaking.

[toy4x4]

Is your material sawed out or torched from a larger piece. What we get here is all torched out of a larger piece of plate. All of the torching hardens those sides. We set up and cut our material to size first which removes the scale and hardness from the faces. Then from there it cuts like butter.

[Mr. Wizzard]

Saw cut from round bar, no flame cut. 2-op part in the mill, not much to it.

It just doesn't seem to be cutting as nice as i'd like it to.

[K2csq7]

It just doesn't seem to be cutting as nice as i'd like it to.

 

That's weird...

I have that same problem with every job I've ever touched!!!

 

Got some screen shots? Maybe a fresh set of eyes will see a different approach...

[toy4x4]

You may try using a smaller endmill to rough out and then finish with the 3/8. Depending on your depth of cut, you may need to lower your rpm a little. I ususally get the best results with a .005 per flute chip load.

[Mr. Wizzard]

Sorry, no screen shots, prolly get in trouble. I may try messing with the rpm's and play with it a little.

Thanks guys. I'll let you know if i find the sweet spot.

[Goldorak]

with a 3/8 end mill you should get the sweet spot around 5000RPM and .002 to .003 IPM depending of the geometry , in dynamic the feed will be in the .008 to .010 range

[Reko]

Remember, A36 has a higher carbon content and is closer to 1030 steel.

 

I think the surface feet should be closer to 325 giving you an RPM around 3300 for a 3/8" EM.

 

JM2C

[Mr. Wizzard]

I'm running the same chipload (.003), but around the 325SFM range, 3310rpm's and 40IPM for the 4-flute, 60IPM for the 6-flute.

It does sound way better in this range, i think it'll work.

Thanks so much guys!