I am designing some vertical aluminum pieces to be used to hold shelves level in a rack. The idea is to make 6 of these vertical pieces and use them together to build a rack that holds shelves super level and parallel(+/- 0.005" over 68"). Three of these uprights will go on one side of the rack and three the other.

The plan is to take six 4" x 2.5" x 72" pieces of aluminum and cut about 60 0.125" wide x 1" deep grooves spaced 1" apart on the 4" face. The key is that these 6 uprights be able to stand vertical and that the grooves are all spaced the same to each other. In other words, the 60th groove on all six uprights need to be 60" from the bottom groove (+/- 0.003 or some tolerance like that) and so on.

Two concerns:
1) After cutting 60 grooves 1" deep in a 2.5" deep piece of aluminum will the aluminum end up bowing because of stresses in the aluminum?

2) What are realistic tolerances to expect for the spacing of the grooves from part to part?

Are there any other things to consider?

I have attached a JPG that illustrates the concept but remember that the attached JPG is just a concept, not the final dimensions, etc.

Thanks in advance for your opinions and advice.

....Two concerns:
1) After cutting 60 grooves 1" deep in a 2.5" deep piece of aluminum will the aluminum end up bowing because of stresses in the aluminum?...

They will form a very nice bow. Over 60" with 60 slots it would not be surprising if it bows almost 1".

....2) What are realistic tolerances to expect for the spacing of the grooves from part to part?

+/- 0.002" is easily possible with the correct machine, maybe better.

....Are there any other things to consider?...

Cutting slots 1/8" wide and 1" deep will be impractical using an end mill; these will have to be done using a slitting cutter which means you will need a right angle head on the machine.

And a question; where are you getting 4" x 2.5" aluminum bar? This is an uncommon size in my experience; uncommon to the point of not being available.

I agree, 4" * 2.5" is odd. I'd cut it from cast aluminum tooling plate. Should bow less but will still bow.

I was thinking of using this stress releived material from Ryerson (http://www.ryerson.com/stocklist/StocklistServlet?COM=GetTable&ID=2095).


I guess that it would be 4" x 3".

If you start with 3" material, and you need to face the side with the grooves, I'd only take minimum skim cut off of this side, and take almost the whole half inch off the other side. It may come back this way. You have to try and equalize the amount of material being removed from both sides.

What if I changed it and took quite a bit more material off the face and left 1/8" x 1/8" nubs? I have attached a jpg. Would this get rid of the curl?

As long as you took a significant amount of material on the face opposite the Nubs, you'd be alright IMHO.

What if I changed it and took quite a bit more material off the face and left 1/8" x 1/8" nubs? I have attached a jpg. Would this get rid of the curl?

It is not likely you will ever get rid of some curling the stress relieved stuff will give the best results but that will likely be expensive. Machining both sides as Big Mak suggest will help but it is not predictable from one length of bar to the next how much curl you will get.

One approach you might consider is to cut grooves 7/8" deep in a length of 4" x 1" then bolt this to a length of 4" x 1-1/2". These are both standard sizes. Because you are cutting the 1" thick material almost all the way through it would not curl as much and an curl that did occure would be removed when it was secured to the larger piece. If this approach was used it would be essential to make sure the 1" piece was clamped along its whole length during machining because it would become very flexible with most of the cross section gone and could tend to lift or vibrate under the cutter. One approach would be to do all the connecting bolt holes first and then use these to secure it for slotting.

Geof:
Very good and interesting suggestion. Especially if I used both bolts and epoxy to bond the two together in assembly.

I am thinking at this point to drastically reduce the depth of the groove to something like 0.060" and try some test cuts on my mill using an end mill. If that goes well I may just send some drawings out for quote.

Thanks for all your help and advice for the noobie!