Milling AL flat on a piece that's too large for a vice.

[machine_nut]

You haven't mentioned what tolerances you have and have you thought of using Jig Plate?
This is generally pretty flat to begin with and might save you some head aches.

[mactec54]

Hi Cartierusm

It can be quite a job to get the parts not to be bowed sometimes I found cast plate a little better to keep flat than flat bar

I have seen Aluminum parts/sheet Blancher ground

If you could not do it in your vice you will have to make some jaws for the vice as other posts have said

Holding the piece between the new jaws Take a light cut on the side that is bowed up do not beat it down into the vice just place it in the jaws with hand pressure on it take a light cut to clean it up do all your pieces this way turn them over then & do the other side you may need to do this with only 1 insert in your cutter or a flycutter if your cutter is beating on the part instead of cutting like butter you will be putting stress into your parts & they will bow for ever if this is the case

Once you have cut the back side turn it over & cut the other side again you will get straight flat pieces you must do even depths of cuts on each side as well

A photo of a piece I make in one Kurt Vice with long Jaws & is over 12" long & less than .250 thick

They are straight & flat with in .0002 to .0005 over the whole length

[Mcgyver]

So a couple of questions will regular flat bar 3/8" x 3 1/2" milled down to .345" ever be relatively flat

what's flat? a thou, a tenth, 1/16, ? knowing what you want to accomplish will drive the technique...but regardless thin pieces can be very difficult because they will move as material is removed

Originally Posted by Cartierusm I build vacuum fixtures all the time but if the piece is already a little bowed then the vacuum would straighten it out until the vacuum is released then it would bow back.

this is a problem clamping any workpiece, direct to the table, mag chuck on the surface grinder, vise, whatever...they all impose force that will distort the work. its often not an issue its because the amount of distortion on a particular job/setup/shape of peice isn't enough to notice or take things out of spec....but that distortion from camping force is still there.

getting things really flat is not trivial. ignoring the material change in shape as stress equilibriums are changed, three techniques i'm aware of to get things flat are:

1 scraping one surface (quickest and easiest imo)
2 map the surface with an indicator and shim such that the surface is the same as the map after clamping; in other words create and verify a setup where the clamping is not distorting it (this is the most common way to get thin things flat on a surface grinder)
3 cast a surface for it to sit on; ie set it in something like bondo (with a realease agent) such that its current bowed shape is supported against clamping forces

[Geof]

It will move back and forth as material is removed from each side. In my experience the best approach is mill one edge smooth taking off the minimum material then hold it in a fixture as I described many posts backs; don't hold it down just lay it in the groove and clamp with the setscrews and cold rolled bare against the un-milled edge. Take a light cut, flip end for end and take another light cut; these cuts do not even have to clean up the pre-existing distortion or any subsequent distortion, just get within the tolerance of cleaning up. With luck eventually it will be flat to within 0.001" or maybe better, or worse if luck is not smiling.

[rwexec]

If the cutting pressure is not to great, carpet tape will work.
Cheers

[Cartierusm]

WOW, thanks for all the GOOD suggestions. Right now I'm using a 2" face mill with APKT 5/8" inserts that are definately for steel. I'll have to find some for AL. I think I'll work at making longer jaws and or the set screw method.

I know about Jig Plate material, is cast aluminum the same? Also where online can I find Jig Plate Material, I've never been able to find it in an easy to order online type of place. Thanks.

[Delw]

Maybe I am missing something, but geof's way is right on the money, been doing it for years on 1/4" plates milling down to .200 thickness 3.5" wide up to 16 inch's long.

your bowing could be coming from 2 things which are most common
you tightened the vise way way to tight or your face cutter don't have good alumin inserts, more than like its the latter. I use a 3" face mill

My 40x20 has 4 kurts on it with 8" alum jaws .if you cant use alum jaws cause you don't have them then your standard hard jaws will work fine. to use multiple vises with hard jaw you need to have long piece of ground stock. I use a 4" wide x 2" thick piece
clamp the bar in the vise's then put one bolt on one side of one vise and snug it indicate it in and tighten the others now everything is aligned. remember the vise jaws will only be aligned as good as your ground bar is.

one thing I will say using the back jaw and the top of the non moving part of the vise wont work reason being is your bar stock is bowed to begin with so the pressure of the face cutter will push it down usually in the middle.

. if you need to hold a tight tol. cut one side then flip it around and cut the other. but do it with parrells or cut alum jaws. I found it best that a .750 wide cut locating face on each jaw.

if your still having problems with bowing its due to your face cutter and you may have to get a fly cutter and put a 3/8's square ccmt lathe tool in it .015 rad works best for a nice finish ( thats what fits in my fly cutter).

Again the right tools for the right job come into play ( correct inserts) on thin wide parts( the parts you are talking about are not thin but the basic principle still applies

[rwexec]

There's more than one way to sink a ship.

[Cartierusm]

I'll make some aluminum jaws 10" long then. Question buying inserts is confusing enough, I have it down pat for my lathe but for the mill I still just have the ones that came with it, they are APKT 1604. Can some one post a link to ebay which ones will be good for aluminum or a website with the correct designation? Thanks.

[rwexec]

http://www.dapra.com/cutting/squares...s.htm#xpet_alu