[twocik]

Curious what's the least you've clamp in a 6" vise without the work pulling out and that doesn't hurt the finish ?

I'm pushing the cutters almost as fast as I can get them, face mill too. I ordered aluminum cutting inserts from Tormach that should be here this week, hoping this will help.

I'm clamping about 1/8" of the bar stock not exceeding 1.3" depth with no problem. However when it comes time to mill the back side that's .125" + my clearance level. I'm having to cut off for every nest and I have a lot of parts to cut. I've trimmed down the stock material as best as I could or as close to my size parts size, but the bottom facing time seems to be the issue here.

Using the Tormach facing mill 1.5" and about 4" woc at 6" in length 6061-T6 stock, I had to hand code a facing file. 6 rough passes .02" doc, 4337 RPMs at 40 IPM. Finish face .009 4337 RPMs at 40 IPM. The finish is very nice rainbow

Any suggestions (smaller size jaws, taller parallels, etc..) please feel free....

thanks

[dbrija]

Curious what's the least you've clamp in a 6" vise without the work pulling out and that doesn't hurt the finish ?

I'm pushing the cutters almost as fast as I can get them, face mill too. I ordered aluminum cutting inserts from Tormach that should be here this week, hoping this will help.

I'm clamping about 1/8" of the bar stock not exceeding 1.3" depth with no problem. However when it comes time to mill the back side that's .125" + my clearance level. I'm having to cut off for every nest and I have a lot of parts to cut. I've trimmed down the stock material as best as I could or as close to my size parts size, but the bottom facing time seems to be the issue here.

Using the Tormach facing mill 1.5" and about 4" woc at 6" in length 6061-T6 stock, I had to hand code a facing file. 6 rough passes .02" doc, 4337 RPMs at 40 IPM. Finish face .009 4337 RPMs at 40 IPM. The finish is very nice rainbow

Any suggestions (smaller size jaws, taller parallels, etc..) please feel free....

thanks

It occurred to me while I read this that my answer would be a lot different if I had some polycarb between me and the piece that might get sucked out of the vise and thrown at me. Your speeds seem reasonable to me. You might get away with making that a .04" cut x3 instead of .02" x6, especially once you have the new inserts.

I did find out yesterday that holding 1/8" in my 6" vice cutting .05" at 90IPM stayed put. G0, G1, whats the difference....

[twocik]

Yes first mod on my machine was adding 1/4" poly to the sides on my guard at 18" or 21" high (can't remember) and a new thick face shield. Very fast mod, but wow did it help.

0.04" and it didn't choke ? I've noticed my gauge peak at about 4" into the part at my giving settings. However it could be my inserts are beat and need to be replaced.. Are you using the aluminum cutting face inserts ?



Does Tormach have an upgrade motor coming out anytime soon, maybe 2 or 3 hp...

[dbrija]

Yes first mod on my machine was adding 1/4" poly to the sides on my guard at 18" or 21" high (can't remember) and a new thick face shield. Very fast mod, but wow did it help.

0.04" and it didn't choke ? I've noticed my gauge peak at about 4" into the part at my giving settings. However it could be my inserts are beat and need to be replaced.. Are you using the aluminum cutting face inserts ?



Does Tormach have an upgrade motor coming out anytime soon, maybe 2 or 3 hp...

I'd pay for that upgrade....

I am using a Glacern FM45 facemill with Korloy aluminum inserts. The load meter doesn't move much.

[twocik]

"The load meter doesn't move much."

Wow maybe I need to take your advice and give that a try.



".05" at 90IPM"


Damn that blows my mind, it's gotta be my inserts. Have any video of this ?




As for the least that I clamp it's looking like .1" would be the least, but I'd have to mod my jaws.

[MichaelHenry]

Have you checked out Mitee-Bite products? Their web site has lots of interesting gizmos for fixturing.

Mike

[dbrija]

"The load meter doesn't move much."

Wow maybe I need to take your advice and give that a try.



".05" at 90IPM"


Damn that blows my mind, it's gotta be my inserts. Have any video of this ?




As for the least that I clamp it's looking like .1" would be the least, but I'd have to mod my jaws.

".05" at 90IPM was just an accident, hence teh G0/G1 comment. No real plans to try that again. That cut did bog down a tiny bit. It was only 50% radial engagement.

Unless I entered it wrong, G-Wizard said 2200RPM, 50% radial engagement, .05" depth of cut would run at 100IPM. Don't use the tool much though so that may be baloney (namely me setting it up wrong).

If I have a chunk of spare material in the near future, I may just see how hard I can really push it.

[BlueFin]

I bite at .125" as well, but I know what you mean, cutting those vise holds off is a pain, I always try to design for putting screws through my part and bolting it to a sub plate when ever possible, but you can't always do that.

[twocik]

WOW

[nomedia="http://www.youtube.com/watch?v=ZwGu-JSdol4&feature=player_embedded"]YouTube - Star Part Demo[/nomedia]


Ok so these little guys look to be promising, holding only .06". However I need to figure out if they work with my shars 6" vise. If not I'm most likely going to buy 2 GMT premium vises once things get going. Thanks for the heads up Michael forgot about that company

[BobWarfield]

Oh good, twocik, I was just going to suggest a Talongrip.

I use hardened step jaws that have a 0.010" step that hold pretty good. I like the better than parallels, in fact. But if I had to get below 0.010" I would go for the Talongrips.

Cheers,

BW

[stucaruk]

I routinely hold some 8" x 10" x 2" thick 6061 parts in aluminum softjaws with .1" steps milled into them. It's no big deal to go 160IPM with a .150" DOC and a 1.6" stepover with little fear of chucking the part. I use Mil-Tec SS inserts which work very well in our Fadal, and seriously remove material in out horizontals.

If you're concerned about chucking the parts, mill soem 60 degree dovetails in a pair fo hard jaws, and take the time to machine a dovetail in your parts. It might add an op, but you can take a huge cut with minimal stock to leave for your second ops.

[tikka308]

I bought two of the GMT premium vises (GPV-615) for my PCNC 1100 and love 'em. Just had a fixture plate made (arrives in a few weeks) which will help even more re: taking advantage of two vises with multiple setup positions

WOW

YouTube - Star Part Demo


Ok so these little guys look to be promising, holding only .06". However I need to figure out if they work with my shars 6" vise. If not I'm most likely going to buy 2 GMT premium vises once things get going. Thanks for the heads up Michael forgot about that company

[twocik]

Yes I'm most likely going to run parts side by side on each vise and for longer parts use both of them to hold the work. Who knows maybe even three of them.