Best Practice for dimensioning a Sheet metal Bracket : 3

[ninjaz]

Which is the best practice while giving dimensions for a sheet metal bracket.
1. Taking the fixing holes as a reference dimension and dimensioning the other features based on this fixing hole?

2. Taking some other flat surfaces as base reference and dimensioning all other features including the fixing holes based on those flat surfaces?

 

[tbuelna]

Sheet metal brackets present a unique situation. Sheet metal brackets are often first defined by a flat pattern shape that is cut from raw sheet metal. And sometimes the bracket holes are produced as part of this flat pattern. It is usually more cost effective to put all of the features, including holes, in the flat pattern. So you would want to locate any critical features, such as tooling holes, relative to features of the flat pattern that will result in the least tolerance error after forming.

 

[drawoh]

ninjaz,

Both your schemes are valid. My primary concern would be the functionality of your part.

Sheet metal presents a special problem. Bend edges can be located to [±]0.15", or [±]0.4mm. If you need more accuracy than this, you cannot locate from the bent edge. My understanding is that the flat layout is punched accurately. You have a couple of solutions...

Use a flat feature as your datum. This could be your mounting holes as you noted above, or it could be an un-bent edge. Your mount holes make a lot of sense to me. If you bend all the edges of your part to provide gussets, you don't really care where they are. You need accurate holes, and sloppy profile tolerances on your gussets.

If you are determined to use gussets as datums, you can apply a composite true position. Locate the holes to 0.8mm[ ]diameter WRT all your datums, and locate to 0.1mm WRT your primary datum. In this scenario, your gussets are not a good register surface at assembly.

You can make your holes grossly oversize. If your true position cannot be anything less than 0.8mm[ ]diameter, your holes must provide a minimum clearance of something more than 0.8mm. Maybe this is okay for you!

You can fabricate your small, accurate holes after bending. I would chat with my fabricator about this to make sure he does not just assume that I am an idiot.

The final solution is to machine the part.

--
JHG

 

[Tunalover]

I agree with drawoh. Take dimensions from straight, unbent (e.g sheared) edges. But the drawing should show the end-item and should NOT include the flat pattern. Flat patterns are best left to the fabricator because that is process information. Remember that the engineering drawing is an end-item document primarily used for engineering and inspection. While drawings are needed in manufacturing, they are not meant to be a work instruction containing process information. Work instructions are manufacturing documents not necessarily subject to formal revision control and could include the flat pattern for a sheet metal part. The designer needs to be aware of how the part is made, though, so that he doesn't design something impossible to make or use bend radii that are too small for the material.


Tunalover

 

[looslib]

WE had enginerring put the flat pattern in the CAD file and depending on the part also on the drawing. Most simple 90 degree bent parts would not have the flat on the drawing. We also put a note under the flat stating the dimensions were for our internal manufacturing only. If the part was subbed out, we expected the sub to deliver the finished part and create their own flat and inspection drawings.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[tbuelna]

Flat patterns of formed sheet metal parts are mostly created for manufacturing purposes, and they are usually not subject to dimensional inspection unless they are a deliverable product. If your part requires a hole pattern to be located in a certain position relative to some formed feature on the finished part, then you should make a drawing of the formed part defining the dimensional requirements for the hole pattern.

 

[happystamps]

Normally when I do brackets I tend to use-

Datum A- Surface of initial mounting hole
Datum B- Mating surface around that hole
Datum C- Third item, usually second mounting hole (if there's one available!) or cut edge.

These are tube mounting brackets, usually welded on so I'll put an offset surface profile on the mating surface and a note giving a general surface profile elsewhere. Also a flatness on mounting surface.
But then it all depends on how it'll be fitted/gauged.