Left / right hand part issue 1

[Agriego]

I have an issue that I have not been able to work out to my satisfaction, I hope someone here can help out.
I have a retainer that is essentially a strip of sheet metal, that is installed on the left and right side of a fairing. The problem is that if I create separate configurations of the part, there are two separate entries in the BOM. I'd like to keep the BOM associative, so I don't want to delete the extra instance and manually change the part quantity. I could create reference sets in NX, and that worked great, but using configurations in Solidworks essentially makes them separate components. Does anyone know how to have them show up on the same line in the BOM without manually editing?

I'm using Solidworks 2015, X64, SP 3.0 and Windows 7 Pro, Service Pack 1.

Thanks!

Al

 

[ctopher]

Click on the part in the feature tree, in the popup tool bar, select Component Properties.
In the popup window, bottom-right corner, select "Exclude from bill of materials".

Chris, CSWA
SolidWorks '15
SolidWorks Legion

 

[Agriego]

Then I would have to modify the qty on the other part, correct? I was trying to keep everything associative in the BOM. I'll do that if there isn't another way.

Thanks!

Al

 

[JMirisola]

If they are the same part, just create two instances in the assembly. If they are actually different parts, specific to one side or the other, how can you not show them both in the BOM?

Jeff Mirisola, CSWE
My Blog

 

[Agriego]

The part is flat for most of its length. It's only at the end that it curves inward to match the profile of the mating part. The curved portion of the retainer is highlighted blue. The flat part is placed where it needs to go, then riveted in place. The radius is fairly large, so it doesn't need to be bent ahead of time. It's a simple part, but solving this particular issue is taking more time that I expected.

Al

 

[EEnd]

In the properties for the BoM there is a section on Part Configuration Grouping. You might be able to get what you are after using those settings, probably "Display all configurations of the same part as one item."

Eric

 

[JMirisola]

Again, why two separate parts? If it doesn't have to be bent ahead of time then you're using the same part in both locations and forming it to fit, or am I missing something? It seems to me that you may be over complicating it.

Jeff Mirisola, CSWE
My Blog

 

[emorel22]

Jeff,

From the image he posted, it looks as if the part is modeled as bent, with a small angle at the end of it also. This would make it so that he can't simply flip the part over on the other side, the angle would be upside down relative to the mating part. In reality, he's going to use the same strip and bend it either one way or the other, but in SW, that means two different components.

Eric's solution sounds like it may be what you're looking for, Al. However, you may run into problems with Toolbox parts if you're using any. I just tried a quick example assy and I had two different lengths of a 3/8" socket head cap screw in my assembly, and by turning on this option it combined all lengths of the same diameter bolt into one line item with no delineation.

E. Morel
M.E.

 

[Agriego]

If I used a flat version of the part in both places, then it would be embedded in the seal instead of following the contour. I'm really trying to keep it simple, but I don't see how to do what I want. Again, I could do it easily in NX, but that's a more advanced package than Solidworks.

 

[emorel22]

Upon further tinkering: I don't think the BOM configuration properties will do what you want them to do either. It doesn't combine parts from different configurations, only the one being shown on the BOM. You can show BOTH configurations on the BOM and that will show that there is 1 part on each side, but that is cumbersome and would make it seem like there is two of everything unless done properly.

E. Morel
M.E.

 

[Agriego]

I tried Eric's idea, and it buggered the BOM. We use configurations for our nuts, bolts and washers, and when I displayed the configurations as one item, I lost the different fasteners in the BOM.

Al

 

[Agriego]

I'm going to jerry-rig it by making both left and right models in the same part file, import two into the assy, and hide one of them, so it doesn't look goofy in the drawing views. That way the BOM stays associative.

Well, at least it hasn't been boring this afternoon.

Thanks for your help, I really appreciate it.

Al

 

[EEnd]

2014 has an option: "Display configurations with the same name as one item" That selection might not mess up your fasteners, as they probably have unique values. To give the configurations the same name, you would go into the part, switch to the configuration tab, right click on each configuration, select properties, set the drop down under "Bill of Materials Options" to "User Specified Name" and enter the same string in for both configurations.

Eric

 

[49again]

Al -

I had to do something similar a while back. I modeled the "form at assembly" sheet metal part so it would look correct, made my opposite-hand version, and then excluded them from the BOM. Then I modeled the part in the un-formed condition (just a simple flat metal strip), added two of them to the assembly, and then hid them.

Probably kind of a whack-a-mole sort of work-around, but it got me what I needed....

Steve