Aluminum into a potato chip

[Mic6]

Well, as the subject says.... I have a 6 x 7 x .250thk plate held on my vacmagic chuck. I skimmed side 1 .005, flipped, skimmed side 2 .005. Flipped back to side 1, skimmed off .01, and roughed the .06 deep 4.5 x 5 pocket .025 deep. Flipped back to side 2 .01 yadda yadda. Take the part off, it's curled like a muther. Now that I think more about it, could my tool have beaten stress into it? Maybe a good ol single tooth flycutter? Or maybe I was being too gentle with it. Any ideas woul dbe awesome..

 

 

Edit: it's 6061-T6

[Guest CNC Apps Guy 1]

That tool does not look too free cutting. Looks more like a neutral rake which WILL put stress into certain types of parts and materials.

[Colin Gilchrist]

What is your flatness requirement? I usually ditch the face mills on thin parts and mill it with a smaller tool. It puts less stress on the part.

 

Are you cutting rolled plate? See if you can get ground tooling plate in the same material. Much less internal stress in the material itself...

 

Also, maybe consider starting with a thicker material to begin with. .250 plate will have a significant amount of skin stress...

[Mic6]

Only the pocket calls out a .005 flatness. The pocket floor to the face of the part is .005 parallel. All my stock is tagged and bought off flight matl. .250 plate. Can't tell how it was made, but it's all I have. I'm setting up with some junk oxidized material I found in the drop pile, I wonder if that coul dbe the problem Anyway, I'll try facing with a .75 endmill, and less flipping. I'll shall report back.

[Goldorak]

can you get a higher grade aluminum , like 7075

 

and + 1 to all that Collin said , .25 plate is a pita to work with

[Guest CNC Apps Guy 1]

Good call with the endmill.

 

6061 is generally pretty stable. Gummy, but stable.

[Rob @ Target Machine]

I have to make 6061 and 4047 Alum "laser-weld" covers all the time.

 

If you can get stock to size you don't have to open that "can of worms".

 

If you have to take a skim cut with a face mill, pick something with a scooped insert geometry and keep your surface speed low and your chipload high. That will minimize the stress.

 

HTH

[MIL-TFP-41]

quote:

---

That tool does not look too free cutting.

---

A balanced version of that tool hold my personal record for MMR. 2 1/2 dia @ 20,000 rpm, 640 IPM, .15 DOC. The spindle was pegged at 125%....I tried the same cut with a Mitsubishi ASX (whatever their fast alum cutter is) and was only able to get to 350~400IPM before the spindle maxed out.

[Mike Whitten CAD/CAM Contractors]

I agree with all comments above but would like to add something along the lines of what Colin was mentioning. I believe most of what you are seeing is residual stress in the material. If you can't get different material and nothing else works, you may have to do a good stress relieve / cold stabilize. You can go a little hotter on temps to reduce tensile strength slightly if job allows. Going from T6 to say T4 or T5 will make a big difference. Your heat treat person will know what to do.

 

Thanks

[taperlength]

+1 Mike

[kunfuzed]

Is there any way you can machine one side of it in an un-restrained state? Seems like if the stock is warped, the vac-chuck will suck it flat, machine it flat, but when released will go back to where it was. I've used double stick tape for flattening out stuff like this before.

[Colin Gilchrist]

Good point Kunfuzed.

 

Sometimes with material like this, a vacuum chuck will hurt more than it helps.

 

I've had good luck before with shimming a part in it's un-restrained state, then using strap clamps with light pressure to hold the part. You make a fly cut (avoiding the clamps), then add new clamps in the machined areas and remove the clamps from the un-cut areas and clean them up.

 

This should help remove any inherent curl in the work piece.

 

Mic,

 

Try making your first fly cut on the material with the vacuum chuck. Then take the workpiece off the machine and put the newly cut "flat" side down on a surface plate. Use shim stock to check the part for flatness.

 

I've also had good luck with wax when trying to hold a part in an unrestrained state. Just some more food for thought...

 

I think Kunfused is on to something here...

[j.nguyen]

Use stecher plate it will lay flat as a pancake every time. I cut steps in a .125 thick plate when machining was an option to chem-milling. The material when released from the vacuum curled 360 degrees. I had our buyer pick up a piece of stetcher plate and it sat on the vacuum plate after machining.....Good luck

[j.nguyen]

Strecher plate........7055

[Kevangel]

I would flycut it with a single point tool razor sharp with a 45 degree cutting edge (not a point). If you have many of these at some point I would look at adding double disc grinding into the mix.

[billet programmer]

From my experience there definitely is inherent stress in the 'skin' on this material regardless of the thickness. I have used a polished high positive insert in face mills & shell mills with good success. You must get through the 'skin' on boths sides in order to get it flat. Milling 3-4 sides (depending on your flatness requirement) is usually necessary.

Regarding shimming, it is better to shim the part in the beginning of the process rather than later imo.

Good luck!

[Mic6]

:UPDATE:

 

Since I have .067 extra stock thickness, I faced side one to +.02 using a .75 2 flute, and a dynamic facing path. Then I came back and faced the same side to +.01 using the cutter shown above. I flipped the part over, faced off the last .01 to 0 using the same cutter. Then I milled the .06 deep pocket in 3 passes using dynamic milling Then finished the pocket and walls with a conventional constant overlap spiral. Drilled, tapped, and reamed my holes. Took that sucker to the surface plate and if there werent any holes it would have wrung itself to the plate! I leveled it on my 3 jacks, checked the .005 flatness requirement on the floor of the pocket and the result.....0003 TIR. I had to re-set it a couple times to make sure, but that's what it read. The top face is parallel with in .001 and it's tolerance is .005.

Thanks for all the suggestions and such. The first article is off to inspection. After all this, I only have 12 to make.

[Gordon Dawson]

Looks like the wrong insert.

[kunfuzed]

quote:

---

I think Kunfused is on to something here...

---

You take that back!!!

 

[Salt4cad]

I use a 9.0 dia, flycutter 2000 rpm,s f5.

w a tp 41 diamond tipped insert kennametal

if using a vise be sure your sides are square to the top also mittee bittes work well, nest it in

have fun

[Bob W.]

When I do parts on the vacuum chuck and the flatness is critical I will measure the initial flatness on a surface plate and then shim on the vacuum chuck with feeler gauges at various points. I also make sure to use new tools or inserts and thicker stock to begin with. Once the initial cleanup pass is done I remove the shims.