Need Help!- large size aluminium(6061) machining

[sharathchandar]

Dear all,
raw material is aluminium 6061 and size 48"x37"x.75".

operations on side view
1).dia .31" thru gun drill along 48" length @ 7 places.

operations on top side are
1).4"X.15" true round slot .11" depth @ 161 places.
2).dia 0.0394" hole .177" depth @ 161 places.

operations on bottom side are
1).1/8PT tap .315"depth @ 35 palces.

i'm wondered how to attain mentioned spec of flatenss on top side .002".

can you guide how to plan the process/toolings/clamping.

if there is any advanced technology i'm ready to invest.

advanced thanks for your valuable advice.

[Paulo E.]

A flatness call out like that you are better off if its less than say 10 parts to purchase stock with that flatness spec already done. As for a holding I would try the Mitee-Bite Clamps, they should give you all the holding force you need while having the top surface of your part free of clamps. You could also try these clamps to run either a shell mill or a fly cutter on top, but to tell you the truth even if you were to use a vacum fixture, I dont see that flatness call out getting done by convencional machining. A call out of that nature on a large part like that it's usually honed.

[Geof]

Originally Posted by sharathchandar Dear all, raw material is aluminium 6061 and size 48"x37"x.75". ....i'm wondered how to attain mentioned spec of flatenss on top side .002". ...

Probably impossible. It is very unlikely that 3/4" plate is that flat to start with and your 161 slots in one side are certain to make it move as surface stresses are relieved.

The big problem I have found in trying to get 6061 plate flat is that as soon as you take off any material it warps, then if you take some off the other side it warps differently.

Cast and ground plate, tooling plate would be preferred for flatness but it is a different alloy.

[big_mak]

If I remember correct the flatness spec for that cast and ground plate is only0.005" per foot. So that wouldn't necessarily help out, but it is much less likely to move.

Alcoa's trade name is Mic6 I believe.

[dertsap]

i agree with the use of mitee bites mostly for the fact they will not draw the part down to the table causing any unneeded stress , if you have a sharp facemill such as a hertel then that would be your best bet
i would do all the ops leaving extra material on that particular face and save the facing op for the very last , if you leave .01 extra then you can take one cut at .005 , then back off the clamps and retighten , take .004 or .003 do the same thing then do .002 or .001 with very little pressure on the clamps ,the last two depths you can pretty much judge after seeing how well the first cut goes , i pick that particular order when its been something that i wanted to play safe with , use enough pressure to hold the part in place , the weight should be near enough to prevent it from moving on such light cuts , it's painfull but do-able , the only issue i could see happening is chatter in the center area of the part , thats why i suggested the sharp cutter , a standard facemill will in no doubt chatter an unsupported length such as that , which raises the question of what is the surface finish meant to be , no matter what cutter you use you will need an optimal spindle speed because i see surface finish on that size of plate being more of an issue than flatness
it may be a good idea to let the part sit for a few days before doing the last facing op just in case the part needs to relieves itself some

if its for production runs then i would seriously suggest looking into a surface grinder

[dertsap]

after all that , it just dawned on me , what is the final thickness of the plate ?

[big_mak]

You could in fact fly cut it if you were worried about vibration. Use something similar to a Sandvik R590 cutter and take out all but one insert. Your feedrate will go down, but your surface finish should be near impecable if your head is trammed in properly.

Maybe do all the detail work and and use some double sided tape and some clamps placed around the outside to make sure the part doesn't shift around.

It's always fun trying to keep big stuff flat with out getting into too many flips of the part.

It would be best though if you couls atleast start with tooling plate!!!!! I will still more what every they say, but not as much as plain ole 6061

[scadvice]

If you have a large double disc grinding shop nearby, do the work and then have it ground. You may want to stress relieve and retemper after machining.
Otherwise...its single point fly cutting, maybe with a diamond. hold it very lightly on the edges or hard waxed to the table with edge stops. Very sharp tools will minumize distortion. -Steve

[dertsap]

one thing you will need to hope for is the customer checks the flatness using feeler gages with that face flat to a granite table or something similar .
if a three point check is done instead , then sag will probably show on the dial reading