Poor cuts, what's going on?

[cn00728]

Hello,

I have had a new HAAS mini mill for a number of months now. I am starting to do batch runs of parts and have been generating scrap the past few days. I am getting vibration on each hole I plunge into on the part pictured in the attachment. It is 3/16" 6061-T6, and cut with a 3/16" 4-FL HSS at P1.5 F3.0 5K RPM The P and F was double on the last run and the cuts were twice as bad. So I'm now at the P and F listed, and the photo shows the result. All along the cut, it looks like the bit vibrates a bit maybe, and you get what look like little vertical indentations. How slow do you have to go to get a perfect cut? Is the bit really bending at a F3.0 into this stock?? The step visible on the side is where the bit even apparently wandered as the cut was being completed. Where the bit plunged, it even wandered into the part. I have a dozen of these parts now, each with the same problem. Now, I am a beginner, so I would appreciate the help.

I should point out that on this try, I put a new double ended cutter in, and had a single ended cutter before, and no vibration during plunge before at a P3.0. Could the double ended cutter be generating harmonics during the cut, it's only a 3/4" length cutter?? I would play around with the plunge rate, and I get vibration even at 1.0. I see demo's and videos of parts being cut out way faster than I am going, so what am I doing wrong??

Thank you,
Alex

[laka]

Are you holding this part securely? It may be the aluminum is deflecting, not the tool.

[HuFlungDung]

Are you plunging right through full depth and cutting it in one pass, or do you have a finish allowance?

A 3/16 endmill does not have a lot of flute space, so it can clog. For full width cut from the solid, I would estimate you can bump your rpm up (if available), reduce the depth of cut to .046" per pass, bump feedrate up to 20 ipm (for starters), and leave a finish allowance of about .005 for the final profile.

It would be best to ramp down to cutting depth with a center cutting endmill, although plunging .046" at a time is not too awful, any vertical plunge cuts should be done a small distance away from the finish profile, because the tool will wobble around. An endmill is not as stable as a drill, because it has no conical point.

A 4 flute endmill might not be center cutting (you did check that before you used it, right? ), but chances are that it is incapable of clearing chips during the plunge. A ramp or helical entry into the part greatly improves the tool life.

[dertsap]

if your plunging the em are you predrilling the hole first ,
if you predrill and leave .01-.02 for finishing you should be ok , 5k is too fast especially with a hss endmill for plunging , treat it as you would a reamer , slower rpm and higher feed rate , also if you undercut the flutes so you only have .1 or so of the tool in contact with the part then you will avoid needless rubbing on the walls which can cause chatter
use g81

[cn00728]

Thank you for the responses.

Yes, the workpiece is secure, and I am using center cutting end mills. I agree that the chips may be clogging the cutter. 5K too fast!?!? I thought speed was your friend, or does the cutter just have a higher chance to chatter? So maybe I'll try 4K?

Probably should put a finishing pass in, but will have to redo the code. That is not real easy because I'm doing a portion of the code by hand. Don't have the money for Mastercam... What, did you think my business is making money? ha ha.

Alex

[fpworks]

Alex,
As these guys said earlier, you really need a finish pass. Also, that 4 flute endmill is NOT your friend for cutting aluminum. Switch to a three flute solid carbide endmill. 6000 rpm and 35 ipm. Your wall finish will be beautiful.

Four flute endmills do not work well in a plunge. Three flutes are a little better in a plunge, you can really drive a two flute endmill in a plunge.

[cn00728]

Yes, always learning. I had this all wrong, and am shocked at the suggested feeds, but this should do wonders for production numbers and make this machine move some! I also purchases ME Consultant Pro to help out with the numbers. This program seems to get a lot of good word on this forum.

Alex

[DareBee]

Originally Posted by fpworks Alex, . Switch to a three flute solid carbide endmill. 6000 rpm and 35 ipm. .

Absolutely

CARBIDE CARBIDE CARBIDE
especially with small diameter cutters (HSS has huge deflection)

[JROM]

Just pre-drill the hole to remove most of the stock, then you can use any endmill you want. The big boys are all using 3 flute carbide endmills these days. I like a 50deg helix and flood coolent. If you go that way the sky is the limit for feeds and speeds (within reason)