Need Help!- 15"X18"X.050" 2024 Aluminum!!

[tminnig]

We were just awarded a job for a very thin aluminum part. It will start at 3/4" thick and need to be milled down to have a 1/2"X1/8" wall around its entire periphery and a .050" thick floor. I have done a lot of parts like this, but not on this scale. Never anything larger than about a 6" square. Any suggestions on how to hold this beast in place to machine it and keep the floor finishes looking great would be much appreciated. Also, any suggestions on best cutting tools, sizes, and practices are appreciated.

I haven't posted here a lot, so most of you regulars probably don't know me from anyone, but I do have about 15 years machining experience, 10 of which has been heavily involved in process development, tooling and fixture design, and programming in a [primarily] aerospace and defense job shop. I only note this in case you feel like my knowledge/experience will affect your response to my question.

I am allowed .040" flatness variation at the corners, but the appearance must be impeccable. Chatter will not be acceptable, and of course, time is of the essence (both in development and machine cycle).

Thanks in advance for any and all ideas/thoughts.

Travis

[PinMan]

Hmm, that sounds like a thinker lol.

Why are you starting with 3/4" stock? That just seems like a lot of wasted material and time bringing that whole piece down 1/4". I would suggest starting with 9/16" thick.

As far as holding, I leave a 1/2" oversize on the sides, making that part 16"X19" and use toe clamps to hold it. You will most likely still see a bowing in the middle area tho. The best holding would probably be a vacuum table.

I would hog out the interior meat with a large indexable cutter with aluminum grade inserts then finish pass the walls with something much smaller depending on what your inside corner radius is allowed to be.

[tminnig]

Pinman,

Thanks for the prompt reply. I am starting with 3/4 stock because it's 1/2 high, not 1/4. Sorry I didn't explain that clearly in my first post. I went with the excess stock so I could hold it with low profile edge clamps and face one side and mill the outer contour, then flip the part, take off the excess and mill out the pocket to the thin floor. Therein lies the problem, however. Even if I use the toe clamps, isn't a large diameter insert cutter going to cause a lot of lift and forces that will generate inconsistency in my thickness and also increase the possibility of chatter? Finishing the walls with something small will definitely be a possibility. I pose the question on the insert cutter sincerely, not in defense of myself, so feel free to respond with any pertinent information on how I can make good use of a large insert cutter if that is in fact a good method.

Also, the toe clamps leave a lot to be desired for stability across that span and thickness, don't they? The vacuum is actually the idea I like the most, but it's something I've never done before and we don't currently have the equipment for. The job may justify setting up for it, but obviously we would like to work with what we have if there is any possibility of success with more conventional methods. BTW, this will run on a horizontal machining center, if that makes any difference.

My initial thoughts were to use a combination of toe clamps, tooling tabs, and double sided tape in conbination with some very sharp, solid carbide endmills that have wiper flats and a high positive radial rake. Any thoughts on this? Should I run the endmills full depth and try to remove all the material at once right to finish in order to keep as much strength in the material as possible? Or should I plan on leaving a very small finish cut on the floor?

Thanks for your thoughts and willingness to help.

Travis

[budP]

How many of these do you have to make?

If it were my job I would go to my local foundry and have them cast, that would only need finish cutting.
budP

[tminnig]

Well, it's potentially a long term deal, however that's not currently the case, this is a relatively small initial order of 50 parts. Casting is interesting, however we are almost always at the mercy of our customer's requirements, which the spec will deem as billet material, complete with grain direction requirements. I doubt casting will be an option.

I am interested as to how this makes it better though, you still have to cut a .050" plate that is 270 sq in. It will still have to be held, located, and cut and I don't understand why casting it first will solve any of the problems I think I'm going to run into? Can you elaborate some on this? At the very least, I may be able to use the information in the future...

Thanks again,
Travis

[LaserImage]

Travis,
I'm not a machinist, so please excuse my simple-minded question. Why not use a .050 plate and machine the 1/2" border from a separate piece then attach? I'm sure it's because that's not what the customer wants, but I had to ask anyway.

Gary

[tminnig]

Why not use a .050 plate and machine the 1/2" border from a separate piece then attach?

Gary, it's a great idea... now to get it to the right guys desk at the customers facility... I like how you think, unfortunately you are right, I can't make these types of decisions, and I seldom know enough about its use or function to be able to determine if it will fulfill the customer's needs or not. So my suggestion would only come across as begging for mercy, and I'm sure that wouldn't help the company's owner get any kind of profit from them again.

Travis

[LaserImage]

Originally Posted by tminnig So my suggestion would only come across as begging for mercy, and I'm sure that wouldn't help the company's owner get any kind of profit from them again.

But what if your innovative idea to change how you make their part saved them lots of money? Wouldn't you be the hero then?

Not being an engineer or machinist, I can't imagine how that part would be functionally different if it were machined from one solid piece or assembled from two, but I can imagine how much cheaper it would be to make.

Gary

[KLUCAS4]

I worked for a Comp. before that machined about 95% Alum. primarily and we made Airplane Bezels that had a really thin bottom thickness and this is what we did. We first machine the outour contour and the inner countour (pocket) then made a plate that would just slip in the inner countour on the 2nd opp we just put the plate in then were able to grab it without distorting or scratching the part and just face milled of the excess and deburred the edges. We just made some extended length alum vise jaws for both first and 2nd opps. And of course we used ground alum inserts for the face mill.

[tminnig]

Gary, the idea that a part can be cheaper and just as functional is one that I'm really not in a position to argue. I'm sure there are many cases where you are correct, but there are also many cases where supply chain, assembly requirements, strength and fatigue requirements, and many other factors could be such that a two piece assembly would not be a good idea to perform certain functions; and could also make it much more expensive and problematic in a complete product than it might at first appear. In my case, I almost never know what my parts are being used for or what they do. I may still make the suggestion, and I'm sure it's very valid in certain scenarios to be sure. I'm just not typically provided enough information to allow myself to think like that. The company I work for is strictly a machine shop. We only do simple assembly and hardware installations and almost never build mating components; we are very focused on strictly machining. We simply quote individual parts and machine them. I think that makes us a very good supplier to our customers, actually, because we can focus on what we do best, and let someone else focus on what they do best.

Klucas, those are some good suggestions. Thanks for your input. I have used similar techniques on smaller parts with success. My only concern would be that the inside of the pocket would have to maintain much more critical tolerances than the print requires in order to keep the second operation workholding from causing a lot of distortion across the middle of the pocket. With a part this large (relatively speaking), the chance of fitting a 'plug' into the pocket so good that I didn't have an out of tolerance thickness variation across the bottom of the floor is very great, wouldn't you say? Have you done this with parts that had similar size requirements? Did they have ribs or some other type of support structure inside the pocket? I agree that the idea has merit and I will look into it further as a potential candidate as I start my pre-engineering next week, thanks for your input.

Thanks again,
Travis

[Geof]

You are doing 50, bite the bullet and press for a vacuum setup.

Machine the 1/2" deep recess, finish the inside surface of the walls and take the absolute minimum off the top of the walls; this means the bottom at this stage is almost .25" and with luck will be stable during the final cut on the bottom so you don't get chatter. During this machining the part is held down by toe clamps around the perimeter, if you have enough material you can finish the top of the walls without moving clamps

Then you make a custom shaped vacuum puck that this tray will fit over with an O-ring seal around the sides so you can pull a very good vacuum. Now machine the outer surface of the walls and face the excess off the bottom to get your final .05" thickness. Full vacuum should be plenty to hold the part down, the total force over that area is more than 3500lbs.

Actually if you made a shallow vacuum tray to put the material in for the first operation you may be able to avoid using clamps.

[KLUCAS4]

The bezels were about 12 x 8 so not quite as big as the part you are producing. But I think if I had to do this job I would approach it the same way. The Insert doesnt have to be the same in length just in width the width that your are chucking on. So another words it dooesnt have to fit exactly. If its about .004 smaller on the width this should not distort the flatness no more than .005. What I was thinking was 2 vises side by side with 2 sets of alum soft jaws about 9 inches long that would give you your 18 inches. Machine a step to support the insert and the part so it doesnt fall out so when you put the insert in it has no where to go. It should be .450 thick to fill the void, length like I said is not that important withing a .500 or so from each end. 20 Yrs experience no problems so far work for myself.