Machining A36 Hot Rolled Steel

[SurfRunner]

I am drilling, countersinking, and counterboring some A36 Hot Rolled Steel. This stuff is much harder than I expected.

I started out centerdrilliing with a typical HSS centerdrill and can tell that will not work.

Are there any suggestions? Should I go with cobalt or carbide tooling? Feeds and speeds?

Thanks!

[ajl6549]

A36 is an carbon steel. HSS is, at best, the last resort for machining this mat'l. I'd use indexable carbide if you can. Several companies like Iscar or Sandvik can help. If you have to use HSS use slow SFM (40 or less) and medium feed rate of .006 or so for drilling opps. .375 dia. and above. Consult your machinery hand book for more info. How many pieces do you have to make?

[SurfRunner]

Originally Posted by ajl6549 Consult your machinery hand book for more info. How many pieces do you have to make?

Thanks a lot!

It will be 5 pieces for now, but it will be something that is on-going with a small (10 piece) lot size.

[ajl6549]

I guess I was off a little. A36 is considered "carbon steel" A2 would be tool steel. Anyway it is still carbon based and there for abrasive.
How many holes per/piece? Still may warrent using carbide insert tooling???
If you do have to use HSS you'll still have to go fairly slow. If you use carbide any generall purpose grade with an edge prep. like a T or K land will keep the carbon from dulling the edge.

[Geof]

[QUOTE=SurfRunner;209500]I am drilling, countersinking, and counterboring some A36 Hot Rolled Steel. This stuff is much harder than I expected...../QUOTE]

This is just standard structural steel. It is possible that you are finding the scale from hot rolling is rough on high speed steel tooling; particularly if you are running fast and feeding slow. What size spot drill and what rpm are you using? For a 1/2" spot drill I would probably try something like 500 rpm and 5 ipm feed with plenty of coolant. I use a spot drill large enough to go out past the diameter of any counterbore because the sharp corners of a counterbore are likely to get burned off against the scale unless you go very slow. Once you are through the scale there should be no problem.

[SurfRunner]

Either/or, it's hard to machine.

The print I am working with isn't your standard print. It is very vague. The material calls out to use low carbon steel.....nothing specific.

I saw how hard the material was and saw a piece that had A36 written on it. I find it hard to locate any specific information about this material.

I am drilling six 3/8 holes. Two with .75 countersinks. Two others with counterbores (forgot the dia and don't have a print with me). It also has a 1.5
clearance hole in the center of it. The material is .75 thick.

It definately looks like I am going to need tooling other than HSS.

Thanks for your help.

[fpworks]

Is the scale burning off your drill point?

There is a huge difference between A2 and A36. A36 is like butter and you should have no problems with HSS tooling.

However, the scale is darn hard, so if you have enough material, face off the scale with a cheap carbide tool. After you get through the scale, you should be fine.

Look up 1020 or 1018 steel for cutting speeds.

[DareBee]

fpworks is dead on IMO.
A36 is very easy to machine.

definitions

"Mild Steel - No mimimum physical qualities specified. For non-critical applications. Easily welded and formed. Also called Max.33, Black plate, Boiler plate or just Hot rolled.

A.S.T.M. A-36 - Most widely used general purpose steel, 36,000 PSI minimum yield strength. Readily sheared, flame cut, formed, or welded using good shop practises."

[RICHARD ZASTROW]

In the future, I'd suggest using more machineable low carbon steel. All suppliers carry them. 1020, 1018, Freemax etc. very slightly more initial cost, significantly less time & $ in machining. If welding required, check with supplier for weldability.

[DareBee]

I agree with Richard, accept IMO Hot rolled often will exhibit less warpage during machining than cold rolled but they each have their place.

[pepo]

The official term at work is "mystery metal". Boxcars of old washing machines,bicycle frames,coat hangers,engine blocks,car bodies and bean cans gave their lives to create this stuff. It is cheap and very weldable but the skin or bark is glass hard. If you buy it torch cut get it normalized and blanchard ground to clean up,adds to the cost (doubles it) but worth it if it is for things that will be milled,drilled and tapped. I have run into hard spots deep inside this stuff that ate tools,two inches away it is fine. Probably the best approach for you is to break through the bark with a flat bottom end mill that is slightly larger than the largest feature at that location. Dont mess around doing this,feed is the key,get through it with as few turns of the tool as you can. Then do what you need to do at that place. BTW this is not carbon steel it is low carbon steel and will not heat treat unless it is carburized first.

[HuFlungDung]

For those running cnc, OSG makes a pretty nice single insert spot drill. Each insert gives 2 edges. It can spot from very small, to about 1/2" OD. They make two iterations, 90 degree (chamfering) and 118 degree which should be used for spot drilling and will serve as a top chamfer for most holes if you pay attention to the depth you are sending it to. You ought not burn the end off of it.