Milling O1 tool steel with 1/32" endmill

Hi all,

I'm trying to machine a 2.5mm piece of O1 tool steel with a 2 flute carbide, uncoated, 1/8" shank, 1/32" square OSG endmill. The part has a gradual slope so the depth of cut ranges from 1mm to 2.5mm. I am trying to mill a bunch of narrow and long slots but the tool only makes it about an inch until it breaks. So far I have tried feeding it at 10k rpm, 2 ipm with a 0.0001 ipt, and 1 ipm with a 0.00005 ipt with no success. It is a full width of cut and full depth of cut 2D contour toolpath, but I have not made it consistently past the 1mm section. I am using a Tormach PCNC 770 with flood coolant. I am aware that spindle speed is a limiting factor and don't have a speeder or similar yet.

I was wondering if it is possible to run this at a full depth of cut or should I be using multiple depths of cut? I was also wondering if my feeds and speeds are appropriate or terrible?

Thank you in advance

Terrible machine whose limitations you'll have to work around (I put one together and saw how it's made, not hate, just fact). Questionable TIR and lack of stiffness and accuracy in the ways are the main problems you'll face.

Soooo....

Can you change from an endmill to a saw blade by fixturing the part on its side, say in a groove in a plate clamped in a vise? This is your best bet for success if you have to use this machine.

If you must use an endmill, check TIR on each tool (carefully), reseat in spindle each time you get a reading of more than .0001" on the dial. When you hit that, go start your process.

Try a 3-flute cutter, same TIR process/target. Stub for as deep as you can go, then regular length, but not over .1" flute length. Better still are solid reduced shank with stub flutes to get the depth, but suddenly you're paying ~3X more per cutter.

Slow the RPM (start around 100-200 SFM), increase feed to ~.0002"/T, see how it works. Vary RPM/Feed if you feel excess vibration from the spindle, there's resonances you'll need to work around to find the "sweet spot". Try cutting .008" deep per pass, vary if still breaking tools.

You must (MUST) use either an air blast or coolant properly aimed to flush the cut zone, chips packing in a slot are death to small carbide cutters.

If you're (for instance) only cutting in X, try sticking an indicator on the Y axis to see if there's any deviation from nominal during use. If the Y is wandering that's another risk point.

If this is the sort of work you'll be doing, start looking around for a proper linear-way VMC. Sell the Torment to someone you dislike...

Definitely do multiple depths of cut. Another thing that may help is a coolant mister to blow the chips out of the cut. Misters can be obnoxious but may be the best in this application. Recutting chips is probably what is killing your end mill.

Ed.

those tormach have a ton of free play, it all depends how tight the machine is, if it's loose on the ball screws, you are screwed as it then moves lets say 0.010 in one tooth, overloading it and breaking it off. if its the same spot, that would be my guess.

best bet is the machine or the process isn't suitable for what you are trying to cut at 0.030" or basically the width of a bandsaw blade.

the 2 flute isnt helping either. find more flutes like 4 or so

NicholasL said:

Hi all,

I'm trying to machine a 2.5mm piece of O1 tool steel with a 2 flute carbide, uncoated, 1/8" shank, 1/32" square OSG endmill.

Click to expand...

That's a major part of your problem right there.
Use the right tool for the job things will go smoother for ya.