Soft aluminum

[So not a Guru]

Anyone have any experience routing soft aluminum sheet? We've got some 0.080" thick 7075-0 sheet we have to route parts out of, but we've broken 10 bits without making a good part yet. The Onsrud tech support says they'll call back sometime, but they've told us that before & never returned the call. In the mean time, we need to cut our parts.

We are using the 3/16" "O" bit recommended for soft aluminum, but we can't seem to find the right speeds & feeds combination.

[Machineguy]

That's like cutting bubble gum.

I take it the material wants to stick to the cutter?

 

If I was having that problem, I'd grab a paint brush and some STP lube from the auto store. (Slick 50 works on 6061 TO, but you cant find it anymore)

Mobile 1 syn maybe. You need to keep that cutter as slick as possible.

Yea I see its a router, but sometimes you need to change things up to make it work.

It will make a mess, but you have a job to do. Just a idea !

 

 

Paint the sheet, not the cutter.

[So not a Guru]

Actually, it turned out that the problem is the special "O" cutter. the darn thing is so delicate that simply measuring the tool chips the end. I switched to an 1/8" single flute upcut bit & ramped contour. It' cutting beautifully now.

 

Still no call back from Onsrud. In a word their tech support, $^<k$.

[Ewood42]

I've had pretty good luck using TiB2 coatings in aluminum. Reduces chip adhesion, good wear resistance, and has good lubricity.

[Bubba85]

We rout 7075-O sheet all the time anywhere from .040 to .125. We use the 63-600 series of cutters from Onsrud (single flut upcut). Run them around 15,000rpm and 50ipm. Unimist Coolube in a spray bottle sprayed on the material before the cut works pretty well for us.

[So not a Guru]

We rout 7075-O sheet all the time anywhere from .040 to .125. We use the 63-600 series of cutters from Onsrud (single flut upcut). Run them around 15,000rpm and 50ipm. Unimist Coolube in a spray bottle sprayed on the material before the cut works pretty well for us.

Do you have to ramp contour? Or do you cut full depth thru the material?

[Bubba85]

Do you have to ramp contour? Or do you cut full depth thru the material?

I ramp it to full depth on the lead in.

[Jim at Gentex]

I switched to an 1/8" single flute upcut bit & ramped contour. It' cutting beautifully now.

 

Yep...that sounds about right.

As mentioned, the stuff is so gummy that anything more than a single flute cutter is going to load up almost immediately and probably snap.

 

Glad you got it running good now! 

[So not a Guru]

I ramp it to full depth on the lead in.

Thanks

[kunfuzed]

+1000 to ramp to depth on lead in.  We've got some idiots here that will do a 1 degree ramp contour around an 8 foot long part!  

[Newbeeee™]

+1000 to ramp to depth on lead in.  We've got some idiots here that will do a 1 degree ramp contour around an 8 foot long part!  

Think of the overtime - not the productivity!!!

[Bubba85]

+1000 to ramp to depth on lead in.  We've got some idiots here that will do a 1 degree ramp contour around an 8 foot long part!  

When I was running our routers i was told by the programmer then that those machines were not able to ramp. He would plung the single flute router bit and had a 50/50 chance of snapping the tip off.

[kunfuzed]

Plunging no bueno...