machining 1018 steel

[busted bit]

most of my experience has been with machining aluminum which obviously has a very big window for acceptible feeds and speeds. i just got a job to machine some steel plate, .25 and .5 thick. i will be doing this on my haas vf-2 vmc. i have an additional coolant pump which flows like a garden hose too. i will have to machine out some 2-3" dia circles and do some profiling. my question is what would be a good end mill to use out of the msc catalog, i usually use 3/8 or 1/2 diameter. i have used carbide in the past but as soon as it cuts a chip it chips the tool so i was thinking of using cobalt (coated?)even if i have to go through a few. the important thing is that i make it through this job and im not concerned about macining fast just accurate with a decent finish.
with the selected tool what would be a good axial depth of cut, ipm feed ,rpm and plunge feed.should i ruff and finish or just use 1 tool to do it? i really need the experienced help here guys, im a metal fabricator with a cnc and have done pretty well but the steel has gave me fits in the past

[DSL PWR]

Well start with a decent carbide endmill. I'd go for a Hanita vari flute. I run my 1/2" at 600sfm (4500 rpm) and about 37ipm (.002/tooth). I slot at .1 deep, and side mill at .2 deep (50% engagement) The tool will do a clean up pass at 1.0 deep and not sing. This is all done on a TM-1, so you should be able to go with a deeper cut and higher chip load on a vf-2. I've never had any issues chipping the mill if I recut a chip.

Good Luck.

[Geof]

Forget the coolant. Go with a TiAlN coated mill and use an airblast for cooling and chip removal. You can run the sfm DSL PWR suggests but if you use a 5/8" 5 flute cutter you can up the feed and take your full 0.5" thickness in one cut.

You mention circles, do you mean holes? How are you programming this CAM or hand?

[Caprirs]

Originally Posted by Geof Forget the coolant. Go with a TiAlN coated mill and use an airblast for cooling and chip removal. You can run the sfm DSL PWR suggests but if you use a 5/8" 5 flute cutter you can up the feed and take your full 0.5" thickness in one cut. You mention circles, do you mean holes? How are you programming this CAM or hand?

Someone is itchin' to show off his newly acquired knowledge.

[Geof]

Originally Posted by Caprirs Someone is itchin' to show off his newly acquired knowledge.

Is this a dig because you know I have mastercam in the company now?

Actually I was going to suggest the Haas G13 circular pocket routine.

[davereagan]

If I ran a 5/8" 5 flute slotting in 1/2" material it would sing and probably break unless it was a V carb. A variable helix TiALN coated endmil is definitely the tool for the job. I get great tool life at 400 SFM (3000 rpm for 1/2" endmill). DRY DRY DRY. Turn the coolant on, cut your tool life in half. No CAM system needed. Just a starter hole and then G3 two passes. With the starter hole already done, you can cut a 3" hole in 1/2" thick 1018 in 30 seconds. 3000 rpm, .0025" feed per tooth for the rough pass, then 4000 rpm, .002" fpt for the finish pass. This requires a stub length holder. I would not run a holder with a projection length any longer than 1.75 I prefer the new ones with 1.375" length. A lot of guys on here don't get the difference and try to get the same results with 2.5" or even 4" length holders.

[Caprirs]

Originally Posted by Geof Is this a dig because you know I have mastercam in the company now? Actually I was going to suggest the Haas G13 circular pocket routine.

Not the Mastercam. The GeofCAM. You are one of the converted now per your thread .

I just wish my mills were rigid enough to do that sort of cutting.

[davereagan]

What machine are you running? An alternative would be a 3/8" varimill taking 1/4" depth, 2 passes and 1 finish pass and you're still under a minute.

[Geof]

Originally Posted by Caprirs .. The GeofCAM. ....

I had forgotten that.

[busted blade]

sorry guys, i wasnt ignoring you. for some reason i couldnt post after initially starting this thread. i tried to get through to the administrator several times with no luck and finally just reregistered under a different name. busted bit is now busted blade. anyway thanks for the feed back.
i am set up for coolant so i guess ill try that. my problem has been that i have not been machining aggresively enough and thats why i have junked cutters in the past when trying to machine steel.im self tought and sometimes that hurts me. i think the hanita varimill? might work for me. i am using bobcad.
so i definetly need a starter hole? no plunging?

[davereagan]

You can plunge, but with a 3/8" or 1/2" four flute endmill, I get chatter if I go above 800 rpm and .00025" per tooth, so that's a brisk 0.8 inches per minute. Center cutting does not make it a drill. Even a basic 1/2" HSS drill can go 450 rpm and .01" feed per tooth for a feedrate of 4.5 inches per minute. Then you just fast feed or even rapid into the hole with the varimill. Air blast when it first starts milling after you've plunged into the hole is much more important than after it has gone even an inch or two across. There is no where for the chips to be thrown, so they need to be blown out. Chip recutting is hard on any endmill. Deadly with other materials. You'll know it when you hear it. Dry though!

[busted blade]

thanks Dave. the starter hole's a no brainer