What's new
What's new

4140 Feed and speed suggestion

HSM_CHIEF

Aluminum
Joined
Aug 2, 2017
I’m just looking for a good starting point for running a 1.75in LOC by .5 dia 4 flute end mill in 4140. I’m running high speed toolpaths I have no problem going .750/1in doc with a .1 step over and around 400sfm and .0025fpt but when I increase my loc I get chatter... what should I change? Thanks everyone
 
Those aren't very HSM-ish parameters :scratchchin:.

How about 6-10% stepover instead of 20%, and much higher fpt (make sure to use chip-thinning calcs)?

Regards.

Mike
 
Those aren't very HSM-ish parameters :scratchchin:.

How about 6-10% stepover instead of 20%, and much higher fpt (make sure to use chip-thinning calcs)?

Regards.

Mike
Finegrain thanks for the quick response but you’d run a 6-10% stepover even with a 4 flute? If I was running a 5-6-7 flute I’d lower my stepover but I’m trying to remove a lot of material I’m not an expert by any means yet...
 
Annealed I'm assuming, the shit is like mild steel.. Maybe back it down 10%...

You know how people tell you to go max revs and feed as hard as you can on aluminum.
That's kind of what happens with an annealed 4140 or 4340.. My magic # in the soft stuff
has been .070 step over with a 1/2"... 700-900 sfm and feed the heck out of it.. .007+
a tooth.. Depending on your machine, run the #'s backwards and make sure you aren't
going to run out of HP.

What is going to kick your ass is the 1.75 loc.. I wouldn't want to try and take that in
one cut.. You are getting to that point where your hang out is getting up there, and an
endmill that is fluted back more than 3X D is where you are start running into issues..
I would go with a standard length 1.25loc. and get as deep as you can and then come in
with a second tool hanging further out.. If you stay a few thou off the wall you won't
even need to buy a necked back tool. Then come in and finish.
 
Agree with Finegrain - I typically run something around 8-10% stepover, maybe 700 SFM and like .002 ipt before chip thinning calc. The light stepover you use for “HSM” results in less chips to evacuate per rev so you can get by with less relief behind each flute which means you can use a higher flute count em (like 5 or 7) and since the FPT remains the same you get to go more inches per rev plus a larger core in your em which makes it more rigid and less likely to chatter. That being said, I’ve not gone much more than 2X in 4140 so maybe you’ll still have chatter problems with the 3.5X you’re looking at. Also, use a side lock end mill holder and make sure your part is rigidly held or it’ll bark back at you. Good luck!
 
Agree with Finegrain - I typically run something around 8-10% stepover, maybe 700 SFM and like .002 ipt before chip thinning calc. The light stepover you use for “HSM” results in less chips to evacuate per rev so you can get by with less relief behind each flute which means you can use a higher flute count em (like 5 or 7) and since the FPT remains the same you get to go more inches per rev plus a larger core in your em which makes it more rigid and less likely to chatter. That being said, I’ve not gone much more than 2X in 4140 so maybe you’ll still have chatter problems with the 3.5X you’re looking at. Also, use a side lock end mill holder and make sure your part is rigidly held or it’ll bark back at you. Good luck!

Thanks Nerd! I am currently using a side lock tool holder... I’ve never tried running that high of SFM in 4140 but that’s because I’ve always used 4flute maybe I would have better luck running a 5-7 flute that would make for a much stronger core!
 
BobW is spot-on the money.

My go-to for some 1/2" x 2" LOC variable-flute endmills was always 6100RPM, 100"/min, and .050" WOC. (I never bothered to calculate the speed/feed, because these lazy-man's numbers worked well-enough for my onesie-twosie jobs, with my machine & holder combo --- Nikken milling-chucks for-the-win BTW...) On something that long though, I'd do exactly what BobW suggested, and break it into (2) depth passes, and just like he suggested, I'd leave an extra .005"-ish stock on the second/deeper pass, so that I didn't rub the shank on the walls. It always worked like a charm.

Even with a 4-flute tool, yes, I'd still take that small a width-of-cut. Even though people assume that 4-flutes = wider cuts, the problem - like BobW already mentioned - is the length-diameter ratio. The flute-space removes a lot of stability from the endmill, and thus, you have to reduce the width/radial-load to keep the cutter from deflecting away from the cut.

The better solution, is to either use a shorter cut-length endmill with a long neck, or use an endmill with a smaller gullets (flute-space) which is stiffer, and still take a small width of cut.
 
BobW is spot-on the money.

My go-to for some 1/2" x 2" LOC variable-flute endmills was always 6100RPM, 100"/min, and .050" WOC. (I never bothered to calculate the speed/feed, because these lazy-man's numbers worked well-enough for my onesie-twosie jobs, with my machine & holder combo --- Nikken milling-chucks for-the-win BTW...) On something that long though, I'd do exactly what BobW suggested, and break it into (2) depth passes, and just like he suggested, I'd leave an extra .005"-ish stock on the second/deeper pass, so that I didn't rub the shank on the walls. It always worked like a charm.

Even with a 4-flute tool, yes, I'd still take that small a width-of-cut. Even though people assume that 4-flutes = wider cuts, the problem - like BobW already mentioned - is the length-diameter ratio. The flute-space removes a lot of stability from the endmill, and thus, you have to reduce the width/radial-load to keep the cutter from deflecting away from the cut.

The better solution, is to either use a shorter cut-length endmill with a long neck, or use an endmill with a smaller gullets (flute-space) which is stiffer, and still take a small width of cut.

Thank you! I guess I can do it in 2 depths of cut I was just wondering if it was possible and reliable to do it In 1 depth of cut... I’m pretty sure this 4140 is heat treaded and drawn back to around 28-32rc or is this the “annealed” state?
 
Thank you! I guess I can do it in 2 depths of cut I was just wondering if it was possible and reliable to do it In 1 depth of cut... I’m pretty sure this 4140 is heat treaded and drawn back to around 28-32rc or is this the “annealed” state?

30ish Rc is not annealed.

I would try to do it in one depth of cut at 600sfm at 5% radial and 0.006 ipt for start.
 
30ish Rc is not annealed.

I would try to do it in one depth of cut at 600sfm at 5% radial and 0.006 ipt for start.
Thanks Zero I’ll give it a shot I really just needed a starting point and I’ll adjust from there... I always end up turning my SFM down when I increase my LOC and it ends up just chipping my end mill... so I’m thinking the increased SFM will be the ticket. it is an internal pocket so I’m worried about chip evacuation I did put a .875 pre drill to help clear the chips. I also plan on running air blast
 








 
Back
Top