Sheetmetal Method Question 3

[BodyBagger]

Hello all,
I do not do much in the way of sheetmetal so I would like to get some proper methods input for a simple part. I have a 10AWG flat plate about 18 inches wide that will have left and right flanges bent down 90° 1" in from each side. In the fixed face region I need to put some drilled holes and some tapped holes. Should the holes be put in prior to bending and should they be dimensioned from the edges before bending? Or should they be put in after bending and then dimensioned from the now bent face?

Thanks in advance,
BB

 

[ctopher]

YouTube shows how to do some of this.

http://www.youtube.com/watch?v=ZvtyBgfOlfM&feature=related

Add the holes after making the features, then flatten it.

Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion

 

[BodyBagger]

Hi ctopher,
Youtube is banned here at work but I will look tonight. All of our holes have a 0.010" tolerance and I'm not sure if they can hold that on a plasma table or not. I would think that if the tolerance can be held that they would cut the shape and the holes and then bend to complete the part but I could be wrong.

 

[ctopher]

Add your holes in the flanges, then flatten.

Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion

 

[BodyBagger]

The holes are not in the flanges, they are on the fixed "center" section. My dilema is really more like order of operations. I want to model and dimension it in the fashion that works best for production and incoming inspection. If I add the holes and dimension them from the edge, incoming inspection will not be able to measure to print as it is now in the bent shape.

 

[BodyBagger]

Here is a picture

 

[ShaggyPE]

Are the locations of the holes FROM the bend critical? Or is it moreso the location of the holes relative to each other that is critical and the bends are relatively loose from the holes. From your attached picture, this appears to be the case.

If that is the case, I would treat one bend as the datum surface, dimension everything off of this, and then dimension the overall with a looser tolerance. The other option if using GD&T... is composite positioning. Using composite positioning, you can specify that a pattern of holes are "loose" relative to the surrounding features and "tight" to each other. This will allow you to tightly control the hole to hole spacing and loosely control the hole to bend spacing.
See the link

http://tec-ease.com/tips/april-03.htm

In general, you always want to dimension you finished part. This will allow for inspection and not tie the hands of the fabricator. If you dimensioned the flat, but the flat was wrong... your finished part would be wrong.


-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[TheTick]

It actually shouldn't matter. The flat pattern should develop the same either way.

 

[Gurjjeet]

We at our work keep the flat pattern as a reference. We expect the manufacturer to do a trail on that & make the part according to Final part drawing. That keeps his job easy by having all flat pattern dimensions on the drawing & saves our **s by saying it is for reference only.

It is always advisable to dimension the final part dimensions. As if you do Flat pattern dimensions & the final part is not as per your expectation, then we have no method of finding out if the flat pattern was cut wrongly or the drawing was wrong.

One more suggestion ask your fabricator for thier favourite bend radius & try to make part around that information, as that is the biggest factor which can cause trouble between flat pattern & final part.

 

[MadMango]

Gurjjeet touched upon a critical aspect of sheetmetal, know your tooling if you need accurate parts. Talk with your shop or vendor to find details/recommendations. If you are cutting the holes the same time you are cutting the blanks with the same process, then put your holes in before the bends. If they are a secondary process, you can put them in after (but not necessary).

Composite positioning as suggested by ShaggyPE will yield you the highest tolerances. Incoming inspection is going to inspect the final, bent shape, so dimension from the bent flanges. A locational tolerance of .010 from hole-to-hole should be easy to maintain, .020 from flange to flange is fairly easy on 10ga as well.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[BodyBagger]

Thanks to everyone for all the good information and I think I have enough to move forward. Damn, I love this forum.....I just wish I could contribute more than I request

 

[MadDogMcDurmott]

BB,

You may also need to experiment with the correct K-factor that will yield the most accurate real world results for your bends. Take a piece of scrap sheet metal, measure accurately the length, then have your press brake operator bend one or two 90° angles. Measure the bent piece and duplicate it in Solidworks. Adjust the K-factor until what you are modeling is equal to what is being fabricated. The K-factor will vary with different material thicknesses.

Mad Dog McDurmott