LinkBack URL
About LinkBacks
This current cut is ran with an 8mm end mill, single flute
14K RPMs
.13 in per minute
The radius of the slot comes out fine for me, but I cannot get the sides to finish up well
Need to get this done with 1 pass... Any ideas?
This current cut is ran with an 8mm end mill, single flute
14K RPMs
.13 in per minute
The radius of the slot comes out fine for me, but I cannot get the sides to finish up well
Need to get this done with 1 pass... Any ideas?
Last edited by dlange; 09-23-2010 at 03:11 PM. Reason: oops
Are running climb milling or conventional? Is the cutter straight or helical?
You should be able to get a cleaner finish than that running a two or three high helix micrograin carbide cutter climb milling.
An open mind is a virtue...so long as all the common sense has not leaked out.
Helical, and both styles of milling, doing a complete oval slot
I'm chaning tools now to a 2 flute end mill
I'll repost
I did get a better finish but I went from that .13 feed rate to a .04
Thanks
another picture on the way soon
I'd agree with Geof,
A one flute bit is more intended for plastics I believe. How thick are you cutting? It looks like 1/4".
Mike
just over 1/8 .13 of an inch
sliced my finger a bit on the new 2 flute!! exciting!
Picture coming after a few cuts
This was at.. 15K going .1 inch per minute
I've brought it up to 18K and ran it slower, all the way down to .04 Still getting these cut marks..
Sorry, the bottom slot is the one in question :-)
Do you ahve the ability to change the direction of the cut? It looks like that is your prob.
Mike
I wish it were that easy.
The object here is to get a clean finish, one pass, that's it. Then I can move on with my life!! LOL
I was getting a more clean finish with single flute... what am I doing wrong here?? The calculation for the machine is [mm/100*g]
I've been told g is for RPM... I don't even use the calculation, I don't know how to get it to work!
Is it quite loud/vibratey when it's cutting? If those marks are due to vibration then it's going to get worse with a speed up/feed slower/more flutes combo.
The finish may be better in the ends of the slot because the workpiece is stronger in that direction, OR the finish may be better at the ends because the outer point of the cutter is now feeding faster than the programmed feed (actual feedrate = programmed feedrate x ((programmed radius - cutter radius) / programmed radius))). Your control may/may not compensate for this at the ends of the slot. Work out that feedrate and apply it to the straight edges of the slot. See if it helps.
Why finish in one pass? You could use a rougher up the middle of the slot then a nice finisher afterwards to clean up the sides.
If you must use a single tool then reduce the angle of engagement by using a spiral path/pocketing cycle, or a trochoidal path. Chip load will decrease and you will be able to ramp that feedrate right up - it won't take longer and the pressure on the tool/workpiece reduces, lessening vibration/deflection.
DP
GENIUS!! I'm putting in the 5mm and trying that right now!!!!
That was my main issue, too much material to take out!
One thing that's just occurred to me...If you have limited options regarding toolpath and you want to do it with one tool only - another option you could consider on this job is to rough the middle with the end of the cutter then move down in Z to the fresher/more rigid upper part of the flute to finish the sides.
DP
Posting Permissions
