Will to pay to get things made (Aluminum Machining)


#1

Hello,
I designed 3D models in Solid Edge and like to get them made and wonder if anyone is interested.
Raw material are 2 pieces if 1/4" thick 12" x 12" aluminum plates. Needs to drill 2 dowel pin holes and 12 fastener holes through both plates. Then, for each plate drill more holes then pocket mill to 3 and 4 depths. Estimate total time is 2 hours. The third piece is to drill 3 holes then cut the profile out of a 1/8" thick 11" x 18" wood based board. All 2-1/2 D operations.
Please contact [email protected] or 817-571-6670 for more information.
Thank you
Sean


Aluminum milling task needed
#2

I assume dowel pin holes will be precise press fit. What are there exact diameters? Should be 0.XXXX" measurements, unless metric.

Have to check to see if we have that size reamer for that pin and will probably need to buy matching drill for that.

What are typical positional tolerances for holes, ±0.XXX"

Will fastener holes be straight through, countersunk (screw head). Will nuts and bolts be used or will one of pieces have thread hole.


#3

Photomancer, Glad that you replied.

This is for my prototype mold. Translation: no tight tolerances required. I just need it to prove my concept.

Dowel pins are for lining up top and base plates and they don’t have to be press-fit. Tolerances can be +/- 0.002" that most NC machines can achieve. You can use 1/4" or a similar size reamers if they are readily available.

Through holes are for 1/4" bolts to tighten up the plates with washers. No countersinks.

Positional tolerance of +/- 0.005" is fine with me. They just need to be lined up between top and base plates. Clamping the plates together then drill will do it.

The depths of those pockets are of my concerns. A reasonable NC machine should be able to achieve +/- 0.001"
The profiles of pockets on top and base plates are basically symmetrical. I need them to match to +/- 0.004 with the help of dowel pins, assuming the NC machine cuts the profile accurately.

Thanks
Sean


#4

People that know me probably don’t want to ask me again because I always ask “What are the tolerances?” Woe to those that say "The normal." Tolerance stack-up on assemblies is especially critical.

Just as a bit of knowledge going forward. You tolerance your drawing features by what the PARTS NEED then find the a process capable of it. Don’t reference what a machine do unless you know the specific machine that will do it. Even then you can get bad results.

Regarding Dowel hole size: Unless you are willing to hammer a pin in, they will always -0.000" to +0.00X" the diameter of the pin. -.00X" is a force fit. Agree with drilling mating holes at same time. Good practice if can be done.

But what do you need? E.g. .125" ± .005" or ± .010", or ?? If you need ±.001 you’ll need a machine capable of ±.00025". General rule: Machine and measuring capability should be at least 1/4th of tolerance. In Measuring standard is 1/10th. So if ±.001" is what you think machine is capable of, then don’t go lower than ±.004"

General note: anything under ±.005" is considered a precision or high tolerance part in aerospace manufacturing, not sure other industries. If you work in optics, then this isn’t precision. But for most machine parts is.

Regarding the upper and lower plate mismatch. What is the maximum they can be out when paired? This will result in different approaches. Is what you are describing is the pockets edge sizes are to be within .004" of whatever the pin size centers ultimately are - not as dimensioned on the drawing. Or within .004" between the mating parts?

By that I mean: Using nominal dimensions on the drawings. , [-A-] & [-B-] are the origin and meet in the lower LH corner so all positions are positive. Nominal as designed Hole position center of of Pin is 1.000" from bottom edge (Datum [-A-]) and 1.000" from Left edge (Datum [-B-]) e.g.: 1.000" up and 1.000" to right.

Here’s where tolerance stack up gets nasty:

  • Using a ±.005" for positional tolerance of hole, it can be located .995 ~ 1.005" in each direction.
  • Hole for pin diameter is ± .002" then the center can be .993 ~ 1.007" in each direction since pin can move around (press fit eliminates this at least on one side).

Is mismatch of plates a Maximum of .004" assembled? I’m assuming it is, so you are really talking about ±.002" on the edge profiles of mating plate features. If holes drilled at end no end to worry about stack-up from those positionally being .004" If edges of mold are much straight, then profile is relatively easy, if a curvy, less so. You say it it a mold so I assume it will have tapered walls for release.

I think the part you want can be made on Haas. But folks grossly under-estimate the tolerance importance when dimensioning a drawing. Folks tend to over-torerance when they don’t need to. When there are assemblies of mating surfaces and profiles there will be a need for higher tolerances. Generally think "How much can these be off? Then split that in half for the two parts. If one one is foo the max - Plus directions and the other is in the Minus directions, you still be at the edge of your tolerance band. You may have to subtract the tolerance for positional of pins - if they can move, then every thing else moves plus or minus in relation to them.

Depths are easiest.

I am not trying to scare you always. But if you are looking at manufacturing these molds then you need to be aware of these parameters. If you have multiple molds, they will vary between each other - which will also mean parts made from them assemble differently.

Now a further bite in the rear: Tooling, which is what molds are, generally use 1/4 to maximum 1/2 of the part tolerance. So if on assembly these part will tolerate ±.010~.012 then the above the 1/2 max above.

I think this topic would be much attended classes on how to decide what tolerances should be and various way of achieving these. I think between myself and @Will1 (Manufacturing Engineer at Lockheed Martin) we can come up with a 2 or 3 class series to get people going. It is something most folks haven’t been taught, but very important. This is just how to achieve the Design goal … maybe get @frank_lima involved on this to decide what is the minimum tolerances you really need in the design … Will and I worked/work trying to actually produce the engineers’ generally over-toleranced features. :wink:


#5

Photomancer,

I can see you are very experienced in engineering. I guess I was too spoiled by my machinists and those pricy 4 and 5 axis machining centers when I wrote NC programs in my previous life for milling jet engine airfoils with tolerances between +/-0.0005" on the dovetails and +/-0.002" on the sculptured blade surfaces.

With my current pet project, it’s like a forging piece that doesn’t have datum planes. It does not matter if the edges are like saw teeth because they are not used in defining the geometries. The work piece is held in place and the datum planes are established after the first cut. The center of one pin can be set up as the program origin. The other pin orients the work piece. If the machine controller is capable of defining a working coordinate system, the only tooling needed is a vise or clamp to hold the plates down, which I assume all shops have. Under these conditions, the tolerances on the profiles are determined by the machine setup and cutter run-out, etc. The mating of the top and base plates are controlled by the pins. Therefore, the tolerance on the profiles between the plates depends on the afore mentioned factors. So, I think tolerance on individual profile of 0.006" will be good enough for me.

You mentioned Haas, which I know is of good quality. Is there a Haas at DMS ???
If so, I just need someone who can set it up. Otherwise, I need to find some alternatives.

Thanks
Sean


#6

Yes. We have a 3-axis machining center. If you write tool paths you are way ahead on this project. Get with @Chris_Wischkowsky @nicksilva or some others. They can probably get you in touch with someone you need.

Spent a lot of years as a source rep overseas. Very familiar with airfoils - retired from P&W. Had I known you are familiar with G&DT would have been easy. Of course on your projects the Engineer “should have” calculated stack ups. You job was to “make it so”

[quote=“sfeng, post:5, topic:41626”]
forging piece that doesn’t have datum planes.
[/quote] Sounds like the N-stacking angles/points out in space.

Ah yes, root tolerances and finishes critical. Then we had to deduct measurement error that brought it down to about .0004".


#7

Lived and worked next to East Hartford for 4 years before coming to DFW. No more snow to shovel…