Milling aluminum flat

[Joels]

If you guys had to mill a piece of 6061 aluminum flat to .001 how would you do it? I guess i would use a fly cutter as i have tried end mills and it doesnt give me a flat surface. any ideas?

 

 

Joel

[Fig sign]

this is not a correct question .

How looks Ur part ,it`s size ,how do you mount it onthe table (musking tape,vacuum ,clamps ).

How rigid is your part .

This are the main factors

[Joels]

Thank you for the reply. I am milling a piece of aluminum that is .188 thick. It is clamped to a piece of aluminum that i flycut flat. I am trying to make a pocket -.075 deep in the aluminum. I can seem to get the pocket flat. I get .02 difference from side to side. I am using a indexable 5/8 single insert end mill know. I thought if i followed with a carbide 1/4 endmill it would make it falt but it didnt. The only thing i can think of is flycutting the aluminum.

[crazy^millman]

Well I would put it down on a piece of Aluminum or Model board using super glue. I would then take small depth of cuts with small step overs to keep the amount of heat build and this also help in stress reliveing that can occur. If that doesnt work you can take the easy route and double stick tape it down to anouther thicker piece. I might look at starting with a .25 thick mill out the pocket and then grab the inside pocket with a soft jaws made to hold it on the inside.

 

I can also throw out a crazy idea you can use bondo as a support for the aluminum. Just think outside the box and try different thing and I think you will get it.

[Fig sign]

Joel !

 

When you finish allum . the most important thing is your bases .

If your base surface is unflat 0.05 mm and you clamp it with clamps or vacuum or any other stress produsing way mounting it on the table no matter what your tool will or milling process will be you will not get less then 0,05 ,you can get only more !!!

So check your base surface for flatness and if it is unflat think of nonstressing way of clamping .

Also as you know the plain defined by three points ,it means that if you clamp three points and you need to clamp fourth point ,put some bronze ribbon thickness 0.02 or the cigarette box plastic cover or some othe thin stuff or more under the needed point .the same goal -not to stress part .

The masking tape is good (without water ,naturally, the glue as MIllman sais 2 ,but anyway no matter what ,not to stress part !!!

The tool the less the better ,sharp,new ,good end mill or flycutter ,not big speed and a small take -off .

But first of all not to stress part .

Alluminium is blanket blankety material ,sometimes to get what you need you must do roughing ,half-roughing ,semifinish and finish ,every time less stress ,better flatness and a waiting period for stress-relief ,sometimes a thermal stress-relief .

The good thing is also the equal rough take-off from the both sides of your part .

 

The empasize is this -check your basic surface flatness before you start to mill your part and think before you

[Kevangel]

you may consider working double disc grinding in the process, it grinds off both sides at the same time which reduces distortion and warpage. I know TCI Aluminum in california does this.In milling flat I would use a flycutter with HS bit "lots of sharp knife edge rake" going across the part short wise i.e.if part is 4" by 20" I would not go all the way across making 20" passes rather cut across 4" way . may have to keep flipping part. I learned in grinding, heat is what causes part to warp. i.e. if I had to take .010, all of of ONE side for enginenering change, I can do this only with small .0005 passes with coolant.

[Code_Breaker]

Watermaker,

[Code_Breaker]

Waterman,

 

Don't know what happened, in middle of typing you a reply. I got posted.

 

Here what I was typing: 6061 Al is too soft and unreliable for flatness. I suggest trying qc-7 Al. It is more stable and machinable.

 

HTH

[Harryman]

The indexable cutter could be wiping stress into the part.

 

Sometimes there is already lots of stress in the material and each cut you take relives some and the part moves.

 

If alternate materials can be used, I'd say try MIC 6 tool plate. It's cast and is way more stable than 6061.

[JG]

#1 make sure you take the skin off first (rolled flat stock, both sides)

 

#2 semi-finsh then finish (both sides)

 

#3 very keen cutting edges, no hone (usually means no coatings)

[Philcott]

Watermaker,

 

The forum members have already given you some things to look at to try to get a flatter part. I like to start with thicker material and clean up one side to take the skin off the material. There are a lot of penned up stresses, in the skin, just waiting to distort the part when machining takes place. Then turn the part over and machine the other side. As has been stated earlier, 6061 can be a pain.

 

Good luck,

 

Phil

[JG]

do you know what temper condition of the material is?

 

t-0, t-2, t-6 ?

[MACHINEMASTERG]

+1 philcott

the skin holds alot of stress and we all no stress kills

[Oppiz]

Another thing to consider, Try to hold the part in the machine the way it’s going to be used. For example if the part is going to be bolted down when used, try to hold part the same way. If the part is going to be free standing then try to hold it a way that your not distorting it tape, glue etc.