[fourperf]

man it sucks. I have only really machined aluminum for years and I need to machine some steel parts. I cannot get the speeds and feed down. I dont even really know what kind of steel. I bought some cold rolled steel from my supply house and when I try to look up speed and feed they list various steel numbers. I have no idea. I have snapped 2 1/2 4 flute end mills and a third got all galled up on the end. It got red hot and actually got a little flame. I was trying to cut at 2000 rpm at 14ipm/. Thats obviously completely wrong based on the result. Any suggestions? I cant afford to keep going through end mills with the trial and error method. I was cutting .175 DOC and 25% stepover

Thanks

Mark

[JROM]

Just start out low and slow and use your overides to pick up speed.
10 % at a time till you hit the sweet spot. With a 1/2 dia four flute endmill (carbide)
start at about 1000 RPMs and 8 ipm. Make sure the coolent is on target. Also depth of cut should be 1/4 the dia of the cutter, no more and tool inguagement should be about 55% in a climb cut. Just remember that most types of steel will work harden if you let it get too hot. If the steel starts to change color your pushing it to hard. With alum. the coolent is just taking away the heat so it can be kind of thin. With steel you need more lubracation so you might want to thicken it up a little. Good luck sorry about the spelling.

[fourperf]

Thanks a lot JROM. I was machining it dry (with a little oil) but mostly dry. Perhaps that was my problem plus it was a hss end mill

Mark

[CNC_BOB]

Flood coolant is a MUST. also, even though HSS end mills are cheaper than solid carbide I recommend at least trying it. I routinely use carbide and for example, a 1/2 in 3 flute can cruise along at 2000 RPM and 20. ipm. full WOC and .15 DOC in tool steel all day long. hope this helps

[DareBee]

Yep
Speed + dry killed your tools.

I would start the HSS at 900 RPM & 8-10 IPM, heavy flood.

I you have an open machine (coolant everywhere type thing) and plain cutter you may need to drop down more, but this is fairly conservative.

If you have a HQ coated cutter and perfect conditions you can likely get the SFM close to double and the IPM close to triple, but that would be really pushing it.

Using a HQ coated (tialn) carbide will double the SFM again.

[fourperf]

thanks a lot for the advice guys.

Mark

[billystein]

for cold rolled (say 1018 no heat treat) with cobalt I run at 84 sfm. the feed i would start about 2 ipm depending on the amount of metal you remove. for hss i would slow down about 10% on the sfm. for carbide about 2000 rmp and 10-20 ipm but I prefer to rough with cobalt ruffers and finish with carbide. I know there are guys who can spin and feed a little faster but I can move metal all week with a cabalt rougher.and keep the chips hitting the floor. for finish kellering (.01 stock removal) i like to use 1/2 ball carbide I found that the tool lasts much longer at 50 ipm than 20 ipm. or even 10 ipm.

billy

[AppEng]

Coolant is NOT always a "must" with carbide tooling. Depending on the operation, if coolant is not applied directly to the cutting edge...of every cutting edge on the tool, coolant will harm tool life by creating thermal shock during the constant interrupted cut that milling creates. Do you think the guys who ball mill 65rc steel with solid carbide use flood coolant? No sir. Face milling? Nope. Sometimes it is useful to use coolant to flush chips away from the cutting zone or for ultra-fine finishes, or heat reduction. Proper tool selection, speeds, and feeds removes heat with the chips instead of putting the majority of it back into the part.

[mc-motorsports]

A lot of it depends on how ridgid your set-up and equiptment is. Feeds and speeds mentioned above are good for top quality equiptment. If your trying those feeds and speeds on hobby level equiptment, or even a bridgeport mill, you'll burn through endmills. Feed and speed charts are for reference only and don't take into concideration how ridgid the machine or fixturing is.

1018 is nothing compared to alloys, probably one of the easiest of the carbon steel grades to cut. But a Mori CNC might cut through 1018 like aluminum would cut on a Bridgeport retro. Just something to concider.

[mc-motorsports]

WHOA! I just noticed how old this thread is... Oh well...