BOM to match Balloons

[CADGemini]

Hello everyone,

Due to cost restrictions my company is using 2001+ to do all there models and drawings.

The problem I am having is that I have an assembly with the three different configurations listed below:

Configuration A= Assembly exploded with detail parts suppressed.
Configuration B= Detail assembly 1 with main parts of assembly suppressed and detail parts of config "C" suppressed.
Configuration C= Detail assembly 2 with main parts of assembly suppressed and detail parts of config "B"suppressed.

On sheet 1 I have assembly "A" exploded and have the BOM generated from that view. It only shows the main parts of the assembly and will not show the rest of the components in the tree.

On sheet 2 I have both configurations of "B" and "C" detailed out with balloons and detail views of each. It appears that each configuration sees only the parts that are resolved in the tree.

What I want to accomplish is to have the BOM on sheet 1 with all components listed. And have the balloons on sheet 2 match the BOM on sheet 1. Is there something I am missing. I know with future releases of solidworks I have not had a problem with this. Any help one may be able offer me would be greatly appreciated.


Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[rporter]

Jksolid.

If you want the parts to show on the bom just hide the parts that you dont want to see in the configuration. That make the bom show the parts not shown show up in 2003 anyway.

Regards
Roger

 

[rporter]

I forgot to mention that you may need to reset the properties of the BOM

 

[CADGemini]

Okay I have tried hiding components but the configurations on Sheet 2 do not correspond with the BOM on sheet 1 when I do that. I even creted a configuration to show all components and the generate the BOM from that view and then hide the view. still no success. What is happening is that each configuration that is on sheet2 is being numbered seperately.

Any other suggestions. I think I have been through the obvious ones.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[Standing]

Insert the assembly onto sheet 2 that you want a BOM of. Right mouse click in white space of sheet, not within a view. In sheet properties dialog find the box that asks for “Use custom property values from model shown”. Or something to that affect. Set the main view that the BOM is going to be linked too.
Do not hide the parts in the assembly you do not want shown on the drawing. Do this in the tree of the drawing itself. This way if someone does a “show all” in the assembly model, it will not change your drawing.
Good luck, I have worked for companies that lost more money “trying to save money”. The bean counters do not realize the money they save upfront cost big time in the end.


Bradley

 

[CADGemini]

Bradley,

I do not see the option "Use custom property values from model shown" Do I have to Ctrl select the view and sheet. I'm using 2001+ just as a reminder.

The thing is I already have all my views laid out and do not want to spend the time re-doing all the views if I don't have to. I really miss working with the future versions of solidworks. I guess I will just have to settle with what i have and create seperate BOM's for each configuration shown on page 2. Although I would like to find another way.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[Standing]

Jon,
The box is there, find the one that has the name of all your views. Have you inserted a view of the one you want a BOM of? What we did and still do is have the whole assembly as a view off the sheet. That way it will not print. No need to change what you have.


Bradley

 

[CADGemini]

Okay nevermind,

I found it. Thanks Bradley. A star for you!

Just needed to wipe the sleepers out of my eyes to see it. I figured it was something simplistic. I have found it very hard to get used to 2005 SW and have to go back to 2001+ to figure out how it was done the old way.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[CADGemini]

Bradley,

For somereason I cannot give you a star. The company i work for has alot of internet restrictions. I will try to give you a star when I get back on my home system.

Thanks again for the post!

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[CADGemini]

okay I have done what you said Bradley and the ballons are still being numbered seperatly with the two configurations on sheet 2.

How do I fix the balloon numbering sequence.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[Standing]

Jon,
Just had a thought. Delete any BOM’s on sheet 2. You may have to delete it in the tree. Reinsert the BOM using your new view of the full assembly. Now does the balloons match?


Bradley

 

[CADGemini]

currently I have no BOM's on sheet 2 and just a BOM on sheet 1 linking to the configuration showing all the parts. The configurations that are shown on sheet 2 have components suppressed in each configuration. do i need to have the components hidden instead of suppressed?

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[CADGemini]

seems like hiding the components instead of suppressing them is what I need to do for each configuration to be numbered correctly. Thank you all for your valuable posts.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[Standing]

Jon,
Components that are suppressed will not show on BOM. Components that are hidden will show on BOM.
Insert on sheet 2, the same assembly view that is the view on sheet one that is giving you your BOM. Move this view of the sheet. Now click that new view you put in and insert a BOM. If you do not want that BOM showing on your drawing, then hide it. But it does need to be there. You can also hide this extra view you just added.


Bradley