Part No. Column in table based bom acting funny

[Olid]

Guys,
I am stumped and need some feedback. I have a bom in an assembly drawing in which 2 component part numbers keep reverting to what appears to be the document name even though I am specifically asking for the configuration name to show up on bom in the configuration properties window for each of the components. I have "fixed" this many times and every time I close and reopen the drawing it reverts back. The components have not been changed in any way. I have never had this happen before with the table based boms. I recall the numbers and balloons acting funny once in a while but not the actual values. Where else can the part number be possibly be getting its value from?

We are running on SW 2004 SP 3.0

 

[CADGemini]

Just curious are you using PDM Works?

There is a "Number" property in there that could be screwing things up each time you check things in/out.

Best Regards,
Jon

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

Solidworks 2005 SP3.0

 

[Olid]

No. We do not use PDM Works. We use Smarteam which has it's own set of issues. However, we get our bom data straight from Solidworks where ever it comes from.

Regards,
Dan Olid

 

[CADGemini]

Well what you are doing is correct for the process to work.

Are the parts(read-only)that you are editing to set it to configuration name?

Have you tried using "User Specified Name" also?

Best Regards,
Jon

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

Solidworks 2005 SP3.0

 

[Regg]

OLID,

I had a similar problem which was fixed by recreating the BOM and then saving both the drawing AND assembly. There is no reason for this to have worked but it did. Just out of curiosity, are you opening the drawing with the lightweight box checked. I found that if I opened the drawing with lightweight checked, the part numbers were being substituted as you described. If I opened everything fully resolved, the BOM would be correct.

Regards,

Regg

 

[Olid]

Jon,
The parts in question are read only. But like I said nothing was changed in those. They have always been set to
specify the configuration name. I will try using the user specfied to seee what happens.

Regg,
I don't believe we have ever used the lightweight box.
I will try recreating and saving again to see if it works for me.

If all else fails up I will just save the bom as a CSV file and put back in through Excel.

I'll let you know the results.
Thanks for suggestions.


Regards,
Dan Olid

 

[Olid]

Well, that was interesting. I just tried a couple of things.

I also thought it might have something to do with the fact that the components were read only. So I checked them out of Smarteam and cycled through the configurations just to refresh them. It made no difference. Also tried using the "user specified" option. That also made no difference. Recreating it worked the first time the bom was created. Closed and opened the file and had the same problem.

This one is really strange. First file that I have this happen to. Oh well... I'll just chalk up it a corrupt file.
That is only thing left that I can think of.

I ended up saving to a CSV and inserting as an Excel file.

 

[CorBlimeyLimey]

I'm running SW2004 SP2.1, if you want to send the files to me I will see if I have the same problem.

My address is "my forum handle" AT Lycos.com


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520

 

[SolidsMaster]

Olid, are the configs you are having trouble with "derived"?

J

 

[Olid]

The parts in question do not contain derived configurations.

 

[CorBlimeyLimey]

OLID ... Took a look last night & the problem is that the BOM is reading an assy config which has the "problem" parts suppressed. If you RMB the assy view, & in the properties section, select a config which has the "problem" parts resolved, the BOM shows the correct config names.


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520

 

[Olid]

CBL, thanks for taking a look.
However, that does not solve the problem for me. As you noticed I have a lot of configurations in the assembly and the only way to get them right is to suppress the parts that are not applicable to a particular configuration. I just tried what you suggested and that only makes another set of parts, which are now suppressed, display the wrong part number. Solidworks give us the ability to list many congfigurations on a bom and I a have been doing it this way for a long time without any trouble.

I am curious did you close and open the drawing after you switched the drawing configuration property? Did you maybe also do a ctrl-q to rebuild the bom?. I still get the wrong value showing up. For me, that rules out the actual parts being the cause of the problem. I am starting to think that maybe it has more to do with the actual bom template. Is there any way to see what and where a particular column on a bom looks at to get it information?



Regards,
Dan Olid

 

[CorBlimeyLimey]

Vreate views of each assy config. Each view can then have its own BOM. You can do this on seperate sheets or all on one larger sheet.


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520

 

[CADGemini]

I'm not sure if this will solve your problem but:

Just a thought but for your configurations instead of suppressing items just hide them. I had done this for an assembly I was drawing and it fixed the numbering problem I was having. Also make sure that your views are linked to the same BOM. You do this by right-clicking on the view and go to Properties and make sure "Keep Linked to BOM" is checked and that they are linked to the same BOM.

Doing this helped me in the past.

Best Regards,
Jon

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

Solidworks 2005 SP3.0