There must be a better way

[Captdave]

Hi Guys,

I’m machining the ends of some 7/8” 12L14 for ½-20 studs and only getting about 300 pieces before the tool is worn out. This stuff cuts like butter and would have expected better tool life. How I have it setup now is to start a Z0 and helix down at .200 per turn to -1”. Quality 4-flute carbide end mill at 500SFM and .003 chip load. Would it be better to start at Z-1” and use the side to cut the diameter in a couple of turn that way? I tried to program a circle move starting at X .440” and moving inward but it would not take less then the full cut at once. Was I using the wrong milling process or maybe use 3 mill circles each with a smaller radius? Winmax control.

I also tried a 3/4" indexable end mill using the mentioned process but still had to go back and finish with an end mill due to the insert relief angle left high spots on the diameter which added too much time. I have little experience with thread mills but it seemed too much to try to thread mill that way.

I run 2,000 of these 24 at a time so trying to balance tool life with cycle time is important.

Thanks

[fasto]

What part of your EM is wearing out? The very tips and corners?
If so, for this kind of application I'd try a "bullnose" em, with a corner chamfer. Or, an endmill with the corner rounded off intentionally.
The goal is to spread the cutting load out over more of the em, not just cut with the very corner, which it sounds like you might be doing.

I don't think that your material would stand for a full 1" engagement of the EM, even with a small doc. I bet you'd get a severe taper on your part from flex, much larger diameter at the top.

If the EM's are burning up, might try reducing SFM a bit, and using a 5 or 6 flute EM to keep the cutting speed up.

What type inserted EM were you using? I have some Seco's that take XOMX inserts, once you get over the $$$ insert costs they are really fine. I'm not sure they'd work for you, I've been using them in cast iron.

[BobWarfield]

500 SFM looks high, based on G-Wizard's figures. I would try more like 250-280 CFM with a quality endmill. The chipload is a tad high too, maybe more in the range of 0.0025.

Best,

BW

[Captdave]

Started out using a straight corner end mill but switched mid way thru the first 1,000 to a .030" radius EM. Helped out a bunch but still not where I thought it should be for 12L14 material.

I have several Ultra-Dex End mils
http://www.ultradexusa.com/saber-mill.html
which I use in 6061 with excellent results and the inserts last forever. Tried the UD5 grade with mixed results in steel but the relief angle on the insert doesn't work well for the way I'm machining these.

I have the Gwizard and usually higher SFM then advertised on 12L14, maybe too high in this case. I have another job I have to start on Monday but I'll try the slower SFM when I get back on them.

Thanks Dave

[timf]

http://volumill.com/
i bought this software for roughing to save cycle time. which it did fine but what i also noticed was tool life increased dramatically also, i assume because conditions the tool was under were more consistent.
i dont sell this nor am i part of them but for roughing it flat out kicked butt for me, reduced a 64 minute pocket cycle to 24 minutes for roughing.
it sounds a little crazy but when you get into it everything makes sense and i cant understand why no one figured it out before.
maybe it could help you

[glovebox20]

Hello

Are you using a Dura Mill Wisper Cut, GARR VRX, Hantia Varimill, or other Variable hex, Variable flute EM with ALTAIN coating? That would be my first choice me Steel/Steel alloys materials. I would use a 1/2 EM with 1.00 to 1.25 Flute length. 450 SFM and .0035 chip, & no coolant to start with (Check manufacture guidelines). I would take the cut at full Z depth, but, I would probably mill 3 different circles plus one finish pass at .005-.008 stock per side. That should give about a .06" Radial depth of cut (Side of EM). You might find out you can get away with Two Rough passes + one Finish, or even one Rough Pass + Finish. The key is to take the full depth on Z so you use the full length of the EM for cutting instead of wearing out the bottom first.

You can use Mill Outside circle and increase your blend Arc to .375 to .750 to get a smother entry/exit. Or if your like me, I would program it using line and arcs and arc in/out at a .75 R. and adjust your start/end point so you only mill like 25* of the lead in/out arc (Store your X,Y Arc center, then clear out the X Start And type a value for Y and it should Auto cal. the rest). And if you want to get really crazy. You can set your Z retract at 1.1" or something and have your Z start/bottom at Z-1.0 to rapid all the way down on the Z axis, then start feeding on the X,Y. And if your foolish like me, you would even add a couple of more Change parameter blocks and Change your Z retract to 0" to keep the EM from lifting up after the second circle. Best to Try this above your parts first Until you know you have enough clearance in the X,Y before rapiding to your next start point. If you PM me, I could send send you a more detailed program like this.

I love the Volumill theory, just wish I had the software to try it out with.

There's My 2 cents

glovebox20

[Captdave]

Tried several different combination's of end mills and patterns but the best results are coming from a .75 index able end mill helixing down at .2" per turn. Oh well, 8 mins for 4 parts really stinks.

[Rich Carlstedt]

Make yourself a tool.
It should look like a rotobroach with inserts and straddle the studs.
In fact, you may want to use a Rotobroach on the inside only
That would dramatically reduce time
Rich

See
http://www.hougen.com/cutters/rotabroach_advantage.html