[Crashmaster]

Hi All,

I am slot milling the face of a round part made out of 1215 steel on a lathe. the slot is .375" wide and 1.1" deep. I am using a .375" solid carbide 4fl end mill. Currently my DOC is .05", SFM is 200 and Feed is .0042. I am looking to see if I can optimize this, specifically on my depth of cut #, it seems low to me. Prior to raising the DOC and possibly shattering a carbide end mill, thought I would get the zones thoughts...

[underthetire]

It really depends on what lathe you have. No magic number for all machines on this one. A big Mori SL603 will take quite a large cut, but a small 6" machine won't.

[Crashmaster]

So even on a slot milling operation the limit is really HP on the spindle and rigidity?

[fpworks]

no, the limitation is the rigidity of the live tool spindle, even on larger turning machines.

[wildwestpat]

Hi Crashmaster

This is one of the reasons why milling machines were introduced. The problem is that the lathe spindle is being subject to forces from the mill in more than one direction. The slot mill is both climb and conventional cutting as well as biting into the work at anglesbetween the two - compare with a conventional turning tool that imposes a uni directional cutting force. This puts forces on the cross slide and saddle arrangements of the lathe in directions that are not normal to turning operations. The larger the lathe the better able it will be to resist forces that are acting in other directions than those experienced in normal turning operations.

That said you can maximise the feed rate by making sure all the gibs are as tight as possible locking them if practical. The spindle should be OK if it is in good condition as the forces generated in conventional turning on a large diameter will be greater than a a 3/8" end mill will take but if the bearings are worn or out of adjustment chatter will cause problems.

IMO - lock the saddle/carriage - tighten the cross slide - tighten any other slides if you are using a milling adaptor on the saddle AND listen to the noise the cutter is making as you increase the rate of material removal.

I assume you are aware that a single pass with an end mill will not deliver an accurate to size slot as it will tend to cut over size. If tolerances are important use a smaller diameter end mill and machine the second side in stages to achieve the correct dimensions.

Regards - Pat

[Crashmaster]

Thanks for the input everyone. An update; I am currently about 275 parts through a 600 part job. I was able to ramp my SFM to 262, my feed is the same, .0042. I was able to increase my DOC to .175 per pass. I feel I could probably get it up to .2 but am not very comfortable with that DOC. I should tell you I am running these on a new (less than 3 months old) Mazak Quick Turn Nexus. I was able to get around 125 parts before my carbide end mill started to noticeably wear. I can live with that. These parts use to take us 13 minutes to run on our old wasino and I have them running at about 2:15 now. The boss is happy so I'm happy.