Dimensioning and Inspecting Sheet Metal

[Sanguilocks]

I have been tasked with learning to dimension sheet metal using GD&T. In the past, there have been conflicting suggestions from the fabricators and the inspector on how to dimension the features, bends, and surfaces of the sheet metal part. In your opinion, what is the best way to dimension a squared U-shaped sheet with cut-outs and countersunk hole patters? We only draw finished pieces, not the flat configuration before bending.

The inspector says that it is almost impossible to pass a part when dimensioning from the edges past a bend because what should be bent into a 90 degree angle or 45 degree angle is so far from those angles in a free state. He suggested references fixture in the drawing, but no one here has ever done that before.

 

[KENAT]

What drawing standards do you work to?

I'll assume ASME Y14.5 below because that's what I'm familiar with.

"We only draw finished pieces, not the flat configuration before bending." Well that complies with what ASME Y14.5 says about such matters so good start. That said, if your CAD can create the flat pattern some vendors do like this to help them - just make clear that it's supplied for reference only and the finished part drawing defines the part - similar to if you send a dumb model to help out a machinist with CAD/CAM.

Inherently there is not a separate standard for sheet metal GD&T - the standard and symbology is the same as for machined parts. It's how you use that GD&T and the values you apply that may need customizing.

Your inspector is not correct in his conclusion, though his reasoning is fairly sound. Bends and similar features in sheet metal have fairly large tolerances that need to be allowed for - especially if your dimension also includes the effect of material thickness variation. This doesn't inherently mean a bent up edge can't be used as a datum though - just that is must be allowed for in the way the tolerances are applied.

If the bent up edge is truly a functional datum then it makes sense per 14.5 to use it as a datum feature.

To accommodate the effect of this on hole patterns in the other sides use of tools such as Composite Positional and profile tolerancing may be appropriate.

http://www.tec-ease.com/gdt-tips-view.php?q=115

http://www.tec-ease.com/gdt-tips-view.php?q=136

http://www.tec-ease.com/gdt-tips-view.php?q=190

You may also want to look into allowing for fixturing of the part during inspection to allow for the free state variation section 2.7.1.3(b) and 6.8.

http://www.tec-ease.com/gdt-tips-view.php?q=152

That's just a starter but hopefully it kicks things off.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[drawoh]

naaron22,

What are you used to dimensioning?

Sheet metal is harder to dimension than machined parts primarily because the bending is less accurate. Sheet metal shops tell me they can do ±.015" (0.4mm) from a bend. I would guess that the punching that flat layout approaches the accuracy of machining.

You need to do tolerance stacks with your realistic tolerances. You are going to have to make the thing work. Open up holes for screws, or use slots. Arrange your assembly so that it can be assembled out of inaccurate parts. Don't stack five folded components, and expect the top piece to be located with any sort of accuracy.

On large flat sheet metal parts, my datum[ ]A is one of the large, flat faces. Usually, I include a note stating that the datum applies when the face is clamped to a flat reference surface. ASME Y14.5 has notes on Free State Variation, you need to read them.

--
JHG

 

[Sanguilocks]

We are indeed using Y14.5M-1994. We have composite positional dims, a surface profile (which the inspector cant meet), and radii and angles at the bends. I suggested making a datum plane at the center of the u-shape instead of one at each end of the shape, but others here didn't like that. So we have datums as drawn in this picture.

 

[Walterke]

Only hint I can give is: try not to use non-90° bends as any kind of reference. It's practically impossible to measure from them. But since you're making U-shapes I guess you don't have a problem there.

NX 7.5.5.4 with Teamcenter 8 on win7 64
Intel Xeon @3.2GHz
8GB RAM
Nvidia Quadro 2000

 

[KENAT]

Looks like a lot of datums.

Select the datum features based on part function.

Perhaps you need to look at composite profile too 6.5.9.

If functionally the edges don't butt onto something it might make sense to make the mounting holes/hole pattern a datum or some such.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[drawoh]

naaron22,

I agree with KENAT.

When you say your inspector cannot meet your profiles, I assume you mean he cannot accept your as-fabricated profiles.

Datums[ ]B and[ ]C are sufficient to fixture your part, assuming datum[ ]A is something parallel to your view. Face[ ]D is flexible, which is why you need to read up on Free State Variation, as I noted above.

Any design requiring dimension[ ]BD to be accurate is not going to work. My ±.015" tolerance noted above is for 90[°][ ]bends. Your 45[°][ ]bends will make things more challenging. You should chat with your fabricator to find out what he is confident he can make.

--
JHG