Creating a BOM only based on parts bubbled?

[rparrish85]

I am trying to figure out whether it is possible to create a BOM for a multi-sheet drawing that will only populate with the items that have been called out with bubbles in the drawing. We have a model provided by a customer with which we had to add supplemental equipment to. We are only concerned with calling out the items that we've had to add to it. I've added bubbles to the items that we want to include, but when I try to create a BOM, it creates one with every single component in the drawing view. I would try to go through the model that we recieved to exclude each piece from the BOM, but there are over 1200 different components related to the main assembly and that would take forever. Plus, we are going to have to repeat this same process for multiple main assemblies. Thank you for your help in advance.

Ricky

 

[SnowCrash]

Select all the components with a drag box, right to left, or shift select from the feature tree. Right click in empty space. Select component properties and set everything to 'exclude from bill'.
Then go back and re-select what you do want in the BOM and clear the exclude box.

--
Hardie "Crashj" Johnson
SW 2011 SP 2.0
HP Pavillion Elite HPE
W7 Pro, Nvidia Quaddro FX580

 

[CorBlimeyLimey]

Hiding and Displaying Table Rows or Columns

http://help.solidworks.com/2011/Eng...s.htm?id=270fe523b4c64b11909128d42c6e308c#Pg0

 

[CorBlimeyLimey]

Could you create a sub-assy of the new parts?

 

[EEnd]

In general, you could insert your customer's assembly into a new assembly and add your components to that new assembly. In that assembly, you would only have 1 item to exclude, the customer's assembly.

To get there from where you are at, create a new assembly. Insert your finished assembly into it and then drag your additions up / out of the old assembly into the new high level one.

Eric

 

[ShaggyPE]

I vote for the method EEnd proposes. While SnowCrash's method works perfectly, the idea of adding equipment to a customer provided system/device screams sub-assembly. I am always a big fan of having the structrue of the model replicate real life.

When I have done this in the past (installing equipment onto existing or customer supplied equipment)... within the drawing, I change the line weight of the customer equipment to thin and change it to gray. It basically ghosts out the "reference" device and makes my parts pop out. Unfortunately, the only way to do this is to create a layer with the gray line color and then set that component/sub assy to that layer.

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[rparrish85]

Thanks everyone for your replies. I figured the subassembly method was going to be the best way, but our customer in their infinate wisdom has given us in mind-numbing detail exactly how they want their file structures and feature trees to end up (even if that means its unusable). I will try to argue with my supervisor again to try to illustrate the points you have made. I was really hoping that there would be a work around, but it seems that following best practices rules again over willy nilly processes. Awesome.