What's new
What's new

Questions on machining aluminum plates flat for mating mold surfaces

jcardi2890

Plastic
Joined
Apr 10, 2014
Location
Pasadena, CA
Hi All, I'm having a problem where I'm not getting flat surfaces when machining plates of 6061 that are 2" x 7" and 0.5" thick. I don't have enough experience to gauge right off the bat whether this is thin enough to warrant residual stress / warping an issue. Here is some information that may be useful:

1) First I square and finish the stock surfaces using a fly cutter, the subsequent milling operations are light slots, the heaviest cut being 0.045" DOC, 0.05" WOC with an 1/8" EM.
2) When I mate the surfaces of the two parts by just laying them on top of each other, they make zero gap contact along the middle ~4" of the 7" long plate, while the ends are visibly not making contact. I measured a 0.006" max gap at the ends with a feeler gauge.
0528_overmoldGapWarp.jpg
3) I'm using a glacern 4" vise with hard jaws to clamp the plate. The area of contact with the stock per jaw is 4" x 0.25".
I'm thinking that the problem is that the plate bows when clamped in the vise, (this is not visible by eyesight by the way), and I clamp with full force and then lead hammer down onto parallels. The bowed ends get surfaced to the same level as the middle of the plate, at which point I probe with an indicator to verify the surface is flat along its 7" length to <0.001". When the machining operation is finished and I unclamp the part, the plate must bow back to its original state, hence the visible gap (0.006") when attempting to mate the top surfaces of the two plates.

I don't have this problem when I machine 9" long blocks that are 1" thick, so that's why I'm thinking the limiting factor in this problem is the thickness of the plate.
To solve the problem I am considering setting up two vises next to each other (as long as the jaws are aligned well there's no problem with doing this correct?), and in the long term considering getting a nice iron fixture plate and using mitee-bite clamps or something similar. Or perhaps I should switch from 6061 to a harder alloy
Do you guys have experience with this problem? Am I in the right track? Any other suggestions for solutions?
Thanks!
 
without seeing it, i'd say you're right about the bowing when clamping in a vice.

no possibility of putting a clamp in the middle? or using T clamps to hold it on the table?
 
In my experience I don't like smashing a part like this down with anything. If your vice is flat and you don't have chips or burrs under it you should be able to seat it flat with minimal clamping pressure. Using a fly cutter you shouldn't need to clamp down terribly hard. This is problem I have repeatedly happen with every green guy in our shop.
-Kurt
 
Hi,
If I understand, you're flycutting the two faces of the .5 thickness, one plate at a time clamped in the vise under "full force", with the 2" width of the plate contacting the vise jaws such that ~1.5" is overhanging free on each side. If that's correct, a couple thoughts:

1) Don't use a lot of pressure on the vise handle, it shouldn't take much force to safely secure the part in the vise. If you have access to a good 6" wide vise, consider using it instead of two 4" vises, although that will be better than one 4" vise to support the plate. For evidence of vise pressure affecting part flatness, leave a test indicator tip on the material and watch as you clamp it. You might see the needle move as the part bends due to the stress, or because a jaw is deflecting, moving the material with it. I'd also be careful during the lead hammering, you can easily introduce a bend that's captured by the jaw forces, only to have it spring when the vise is opened.

Make sure the jaw and parallel surfaces are clean and that no burrs are on the plate, set the part in the vise with firm hand pressure pressing it down, then light to moderate tightening force on the handle. Try moving the parallels under the plate, if it feels like they both have roughly the same drag on them, the part is likely well seated.

2) Almost all Al plate will have stress in it from the manufacturing process, if you have the time and enough extra thickness, consider taking two facing cuts, one for "roughing" which will start the stress relieving process from having the material skin removed. Set that part aside and do the remaining parts, perhaps letting them sit overnight. Then, do a light finishing cut on each side to bring the part to final thickness and remove whatever warping may have occurred overnight.


These are common problems when working with relatively thin materials, your 1" thick part is (if my math is correct) eight times stiffer (2 (doubled thickness) cubed) than the .5". A fixture may help, but it's more likely that going to a material that's seen extra processing for stress relief prior to machining will help more. Changing alloy will not necessarily help, it's more what the vendor does to the stock during manufacture that matters.

If material properties aren't critical, using a cast plate like Mic6 might make your job easier. I don't like the material as it machines worse than wrought alloys, but it has its place...
 
1/2 Aluminum and Smash it down with a hammer, sorry not gonna be flat .
Clamp it down to the table, sorry not gonna be flat.
Lightly clamp in the vise, Now your getting somewhere.
 
First Never Smash down and expect it to be flat unrestrained. Clamp part lightly in the vise and mill your part. Loosen your part with an indicator on the surface and check to see if it has moved. If it did light lightly clamp and re cut. If you still can't get it just take some 100 grit wet dry and flat sand it in on a plate.
 
1. 6061 is not a good mold material. Aluminum molds were always made from 7075.
2. 1/2 inch thick is very thin for aluminum mold plates. Somebody can correct me, but IIRC, A & B plates on a MUD set (about that size) are 2" thick
3. Never use a flycutter for mating surfaces. Any errors in head tram or bearing slop are magnified. We used to do with a 3/4" endmill and lap flat
4. A 4" vice and 7" long plate?

Just sayin' that 100 years ago, we'd have never done any of that.
JR
 
4 inch vise and 7 inch long part? forget it. Plus you're probably on a small machine if you've only got a 4inch vise. knee mill? Bench top?

Search the forum for threads on how to cut the part with double stick tape. That is your best best. Vises suck for making stuff flat and parallel.

I would have used at least 1" thick material.
 
3. Never use a flycutter for mating surfaces. Any errors in head tram or bearing slop are magnified. We used to do with a 3/4" endmill and lap flat

JR

Dude a zillion parts are cut flat with fly cutters. You can check the tram and inspect the cut surface to see what's going on. It's not a big deal. I've cut tons of mating surfaces with fly cutters and the parts will stick together like gauge blocks.
 
Get a bigger vise, or make longer jaws. ease up on the hammering and jaw pressure. Mill the sides first, then the faces. flip, flip,flip. maybe even one more flip.
 
I think if I had to do that operation I would find a way to restrain the part from moving (jack screws in a simple fixture) and glue it down with loctite black max onto THREE say 1" dia locators underneath, then you are holding it nearly stress free...then you will see how much it moves due to stress relief from the machining cuts.
 
As the others have said I think you are bending the plate in the vise, ease up on it. How much? Your indicator will tell you. You only tap the part down in the vise when you have a flat surface, not before, in this situation. How level is the bed of the vise? Indicate it to find out. I am for using a vise, not tape or glue or clamps. 7" softjaws with clamps on the ends would work if you need more support, but a good 6" vise would be better.

What are you molding? How flat do you need?

PS- 1/2" aluminum plate for A/B injection mold plates? What makes you think that is the application?
 
I don't know how much material you're taking of the top, but I've had jobs where I had to remove an equal amount of material off the bottom due to stresses in the material.

J. Clear
 
Hi All,
I tried out all the suggestions and got the flatness and mating surfaces to well beyond spec now. I dialed in before and after clamping and was definitely clamping too hard and bending it. Got some longer jaws, clamped lightly and got beautiful results.

PS- The molds are just for silicone and PU castings not injection molding. Was using renshape 5169 before but the molds warped enough over time while speeding up curing in the oven at 110F. 6061 works just fine for this job.
 








 
Back
Top