How fast are you guys spinning and feeding tool steel bits?

[61SedanMan]

I have a toolroom mill (open model, 4000 rpm) and am running a program that is doing a lot of pocketing and profiling in 6061 aluminum with a 1/2 inch, 3 flute, crest cut (roughing and finishing) tool steel end mill. MasterCam is telling me to run it at about 3000 rpm and 24 inches per minute. I am running it at 3500 and 35 inches per minute and the spindle load is peaking at 105% in some parts of the program. Is it possible to keep increasing speed and feed as long as the spindle load doesn't get out of hand? Of course I could experiment, but I am one of those 'stand on the shoulders of giants' types. Thanks.

[bob1112]

Run the Spindle at WFO and feed at 40-50ipm or until you run out of power with your mill. Not sure of your DOC but around .003 chipload in Al is usually safe. If you can see that chips are not clearing, you will have problems. Make sure to run a hi helix mill and should be fine.

[cam1]

Yes, provided that you are satisfied with the surface finish and dimensional accuracy of the finished part. Remember that MasterCam is only chugging out values based on some ballpark input variables. If you use 600 SFM for HSS on 6061 and .002 FPT, then a dia. 1/2 3 flute will cut at n=4800RPM @ 28.8 IPM, so 4000/4800 X 30 = 24 IPM. You can keep on pushing......if the process is happy. Up the speed and feed until you get the feedback that sais I've hit the limit.
A trick I learned was to program at 200% feedrate, and to dial the Feedrate override on the contol at 50% or 25% at startup. That gives you lot's of room to up the feed (double it), when you feel like experimenting. There are no set rules of engagement in this game.....

regards




regards

regards

[little bubba]

Now comes the fun part, you need to change your techniques to keep the spindle load up near 100% for the entire program, not just part of it. Play with the high speed machining filter in Mastercam, its a pain in the a@@, but it will work if you play with it enough, it will slow you down in the corners, which is where you are probably seeing the spindle load spikes. Change your axial and radial engagements (deeper and narrower), take advantage of chip thinning.

I'd say you are in the ballpark, and don't trust mastercam for feeds and speeds, manufacturers websites, and their tech lines will help you out a lot more. I used to think calling a tech-line was cheating, until I realized that for every tool I bought, part of the money was going to the tech guys/tech department, you already paid for it, use it.