How to do face cutting on aluminium plate without warp ?

Hi ,

I've a difficulties to achieve the flatness .

How to do face cutting on aluminium plate without warp ? Any tips to avoid warping while the workpiece is being clamp by precision vice.

jovansew said:

Hi ,

I've a difficulties to achieve the flatness .

How to do face cutting on aluminium plate without warp ? Any tips to avoid warping while the workpiece is being clamp by precision vice.

Click to expand...

It depends largely on the material. It may be difficult to impossible depends on the residual internal stresses left in the material from the manufacturing processes at the mill like plate rolling. The thinner the material, the more difficult it becomes. Cast material distorts less than rolled plate.

Another issue can be the size of the stock itself. If you are influencing the material when tightening the vise (bowing the material), you will never get it flat.

First off, whats the width and thickness of your finish size? Second, whats the material?

Nobody is going to say "flip it and cut half off each side" ? That was Milling 1A when I hit the Bridgeport for the first time.

SeaMoss said:

Nobody is going to say "flip it and cut half off each side" ? That was Milling 1A when I hit the Bridgeport for the first time.

Click to expand...

Figured that went without saying. However, just facing both sides does not mean it will be flat.

Depending on the size of the part, it may be prudent to tape the part down at least for the first side. Then it is sort of in a free state. Other adhesives will work as well for this purpose.

Also, how much you remove depends on how much there is to remove. A large amount of material may need to be flipped back and forth several times. Half and half can work when you're taking .030. But if you're having to take .125, well...

The material, too. Cast tooling plate would be much easier to work with as others have said.

One piece of advice - where possible, when doing larger parts, buy your material to thickness. That saves us so much time and aggravation. What's the difference in twice as much for the stock, vs. hours of aggravation trying to mill stock plate down to some random size? In the first case the customer pays for it anyway. In the second, quite possibly not so much...

If not, take a look at your part. If it is a plate with counterbored holes or similar in it, you can skim one side with the plate on tape, flip it, drill and cut the counterbores, then bolt it to the table or another plate using the same holes it will be mounted with to "wherever". That's basically the same thing as machining a lathe chuck adapter in-situ...

A final note is making clear the difference between flat and parallel. A part can be bowed practically in a circle, but the sides may still be parallel, so long as the thickness is the same along the length. Flat would be that same premise but in all three axes... so typically, if your customer calls out parallelism, you can get by without flatness, so long as it measures within tolerance along the width - with a micrometer/caliper/etc., NOT a surface plate... But if flatness is specifically called out, that's a different ball of wax...

jovansew said:

Hi ,

I've a difficulties to achieve the flatness .

How to do face cutting on aluminium plate without warp ? Any tips to avoid warping while the workpiece is being clamp by precision vice.

Click to expand...

What I do is set the plate on 3 points and clamp directly over those points. Make the supports as small as possible (I use three 1" diameter pieces of brass rod faced to equal length... around an inch long. If the plate you are machining is small, use smaller diameter supports). Then I use the largest face mill or end mill possible that will not product any chatter, and I mill the top side (obviously avoiding the locations where I have clamps). If the plate is large and thin (using a small end mill), I'll write a program to cut it so I don't have to stand at the machine. If the part is fairly strong, I'll just manually jog a face mill around the surface. Whatever works.

Then... flip the part over, and set it on 3 points again, though this time those points will be in a location that has already been machined in the first cut. Clamp directly over the support points, and once again machine as much as possible while avoiding clamp locations.

At this point, you can move the supports and clamps to a location that has been machined on both sides, and machine away the pieces that remain (the portions you were not able to machine because a clamp was in the way). Do this on both sides.

Now you should have something very close to flat, and you may be able to hold it more "conventionally" and skim both sides with a finish cut. If the material started out very warped, you may need to repeat the "3-point support" method one more time on each side.

PM

toolmaker96 said:

Figured that went without saying.

Click to expand...

You can't assume that anymore. A lot of people now started out on vmc's and think "Just put it in the machine and it does the rest !"

imo, if you don't start out manually, you never get a real feel for how metal behaves when it's cut. Or cast, or hammered, or whatever

+1 on the manual machining. I always liked the fact that I could feel ( and hear ) the cut. I am at this moment doing some consulting at a shop that is building 2 machines that I designed years ago. 2 guys are cnc only. 1 of them is a lathe guy an he is pretty good at it. The other one is a mill guy and not so good. Both are lost when it comes to manual work. I always got my feed and speed by feel and sound, not off of some chart. I actually feel sorry the people that missed out working on manual machines. Plus the fact that I could say "look what I made" instead of "look what my machine made".

jovansew said:

Hi ,

.... while the workpiece is being clamp by precision vice.

Click to expand...

Without mentioning tolerance and size, thickness of stock, or final detail its hard to tell.

An even thickness tolerance down to few thou is virtually impossible in a vice,
even with a vacuum table its hard nut to crack.

mikiemus said:

An even thickness tolerance down to few thou is virtually impossible in a vice,
even with a vacuum table its hard nut to crack.

Click to expand...

I seem to be able to do it somewhat routinely. One thing that hasn't been mentioned is the state of the material. T6 for example is heat treated and artificially aged. T651 is additionally stress relieved by stretching and will warp less.

I clamp a piece (with parallel sides) in step jaws in the vise, or in two vises for a larger piece. With the jaws loose, rock the plate to see if it is fitting flat in the steps. If not, shim it until it does not rock. This minimizes the distortion that will be caused by seating a non flat piece in the vise. If you are after really flat, flip it, do it again, then again release and reclamp unstressed, and cut only the minimum.

In practise, with good material at -T651 temper, in pieces between about 0.5 and 1.5" milled down to as little as 0.25 over large sections, I can normally get flat to within a thou or two. If you are using Chinese or Russian aluminum, well you are on your own - it will be gummy, lumpy, and twist like a noodle, doesn't seem to matter what they stamped on it.

jovansew said:

Hi ,

I've a difficulties to achieve the flatness .

How to do face cutting on aluminium plate without warp ? Any tips to avoid warping while the workpiece is being clamp by precision vice.

Click to expand...

Welcome to Practical Machinist. Isn't Google amazing?

How do I get to the store before it closes?

Uh, we would need to know the distance to the store, it's hours of operation, any possible holidays that affect the store's hours, and your mode of transportation, the condition of infrastructure, etc.

Regarding your "aluminum plate", and its "precision vise" , and the "warping" you are encountering, there is a whole page of questions to be answered.

If this is an adapter between an engine and a transmission, you can tolerate a bit of warping; unless the warping occurs while machining.



Is the thickness the last operation? Yeah, the final outline is an amoeba, or a local island, but that's hard to clamp, so let's work with a polygon of some sort, that fits in a vice. Not the best order of operations. Let's hope the material you cut off with plasma torch, or band saw, or circular saw isn't stabilizing the workpiece.

You may need to place emphasis on the quality of the plate, and its heat treatment, annealing, rolling, flattening, etc.

You need a list of priorities. For instance, if the goal was an adapter plate between engine and transmission, perfect flatness isn't needed, but thickness within tolerance is needed.

The go to material for flatness, in the U.S., would be tooling plate, which is cast, not rolled, and then heat treated. MIC-6 is one trade designation.
MIC-6 (R) Cast Sheet / Plate - Online Metal Store

Heat will be an issue, while machining, since aluminum will move around. You should consider razor sharp tooling, and flood coolant. That might be high speed steel, not carbide, not inserts.

This project is essentially a test of whether you stayed awake in science class.

You may need to drill and tap all possible holes, and mount to a subplate prior to thickness operations.

The aspect ratio of thickness to width, or length, would be nice to know.

And you may need to forget about the vise, and be willing to ensure the mill table is adequately flat, to allow the workpiece to be held down by a series of fingers, straps, etc. that get moved around as need arises.

There may be value in NOT trimming the perimeter to final size, if that perimeter is where you apply the hold-down clamps.

The secret of this situation is the choice of material, and the order of operations. And the clamps...

"Mowing the lawn" may not be the best tactic for removing the metal. You may need to make passes in a continuous, somewhat circular path, either starting at perimeter and working in, or starting in middle, and working to the perimeter.

I may have made some huge mistakes in my advice, so let's see what the experienced hands say about this, before you start work in the shop.

Well you certainly dont squeeze it, You also want your coolant temp in check.

MIC6 is rectified aluminium, even this one has 0.004" of tolerance in flatness. I use so frequent this alloy in sizes 24" 30". I think you will never get it flat or parallel on faces.

1. Get your toe claps set up where you want them. The more the better.
2. Set an indicator on the top surface right next to the clamp.
3. Tighten the clamp and find out how much flex you have.
4. Release the clamp and put a shim under of equal size that your indicator traveled.
5. Repeat for each clamp.
6. Tighten all clamps in crisscross pattern.
7. Machine with large face mill around the clamps.
8. Move the clamps and clean up the spot they were in using the same method as above.

Now you can flip the plate and should have a good starting point. You will probably have mill at least three sides to get what you want.

I use a .032" peelable aluminum shim that comes in layers ~.002" thick

Alright, so I have a plate that started out as 19" x 13" x 1" AL6061. Finished part measures 0.540" thick. I took an equal amount of 0.230 off both sides. The first side I taped and super glued to a sub plate bolted down to bed of mill. Second side it was epoxy'd down around ouside edges and removed 0.15" then added 2 toe clamps in x axis. Then took the part to finished thickness plus 0.015". Part is now warped with center convex facing up. The bottom of the part has 3 pads and the top side has a small circular center pad with an outer ring both of which are 0.04" tall. The bottom side has a bunch of pockets for weight reduction.

Any way to prevent this next time? Part flexed one way after first side and now has gone the opposite but past our thickness tolerance. Any help or pointers would be great. TIA

Sent from my SM-A500W using Tapatalk

Same as you did before, but take 2/3rd of the roughing stock (per face) off. Flip, 2/3rds. Flip again, 1/3rd, flip 1/3rd. You should now be close enough that whatever reasonable amount you left for finishing is adequate.

Better still is to rough out your pockets during the first set of cuts part way, second rough with the second set of facing cuts. Now finish the pockets while you finish face the plates. Lots of work, but when you need to have it flat you do what you have to do.

Old thread...OP never made another showing after 1st post.

valleyduramax said:

Alright, so I have a plate that started out as 19" x 13" x 1" AL6061. Finished part measures 0.540" thick. I took an equal amount of 0.230 off both sides. The first side I taped and super glued to a sub plate bolted down to bed of mill. Second side it was epoxy'd down around ouside edges and removed 0.15" then added 2 toe clamps in x axis. Then took the part to finished thickness plus 0.015". Part is now warped with center convex facing up. The bottom of the part has 3 pads and the top side has a small circular center pad with an outer ring both of which are 0.04" tall. The bottom side has a bunch of pockets for weight reduction.

Any way to prevent this next time? Part flexed one way after first side and now has gone the opposite but past our thickness tolerance. Any help or pointers would be great. TIA

Sent from my SM-A500W using Tapatalk

Click to expand...

.
many materials will warp each and every time you remove material. in general i would rough plate, rechuck at lighter clamping pressure and allow part to deform to its relaxed shape. (dont beat it flat clamped as it will distort when unclamped)
.
then semifinish cuts are taken, then its rechucked to even lighter pressure 30 in/lbs is close to finger tight. helps to use torque wrench. i made red lines on part and take .0005" cuts til gone and indicate to confirm flat
.
many materials require many rechucks to lower and lower clamping pressures with lighter and lighter cuts. quite normal for many parts to finish by taking .0005" cuts