BOM Description, on some parts description doesn't match the part's file property Description 1

[borsht]

I've am standardizing our hardware library. Specifically our data base of screws, (and those who came before did not adopt the SW toolbox). Many descriptions are all over the place as to how the pieces are described so I'm getting those all in line. I've made an assembly model of all the Shcs that we use then made a drawing of it and generated and sorted the bom of that. So I have the description column. On most of the screw models there is a "Description" file property filled in. So from the drawing bom I am going through and changing the verbiage of the ones that are showing as non standard, then saving the file, which is saving the changed part models as well.

On a select few I have found that changing the verbiage in the BOM will change the Description file property on the model, but it wont show up on the drawing that way. I've saved and opened the part, and the new modified description sticks with the part file. Also, I have deleted the verbiage in the Bom, then rmc/restore original value, and it restores the old description that I'm trying to get rid of.

This is happening to maybe 10 out of 100 parts so far. Has anyone a fix, or any advice for this?


SolidWorks Newbie since 2001
-Currently using SW2017

Inventor Newbie since 2019
-Currently using Inventor19

 

[Jboggs]

I think your answer is in configurations. Each part configuration also has optional properties for both the description field and the part number field in a BOM. You can access the description in both the Properties Dialog and the Configuration Property. The part number is only in the Configuration Property box. Different people do things different ways.

 

[borsht]

Jboggs, one of the first things I did to the files was to move any of the fields under the config specific tab to the custom tab, as long as there were no extra configurations. For the files I have encountered with this problem, there is only the default configuration.

But after posting I went to the configuration, and then rmc'd on the default config, and "configuration properties", which I never do, and voila. Staring me in the face is that evil description that somebody came up with. Under it checked is "use in bill of materials".
Thank You!


SolidWorks Newbie since 2001
-Currently using SW2017

Inventor Newbie since 2019
-Currently using Inventor19

 

[drawoh]

borsht,

I agree with Jboggs about configurations. Each screw type should be contained within one file, with standard descriptions. Use SolidWorks' design tables. These are awesome if you know how to mess with Microsoft Excel.

I have written an article on Office Suite Abuse, which covers most of the spreadsheet tricks you need for your design tables.

--
JHG

 

[SBaugh]

I used DT with all the hardware that I have made in the past. Unfortunately, all I have is the DT's and not the part files since I was laid off at my last job.

I think you can get the idea from how I laid out my fasteners per the table. Technically I used the original TB parts and modified them to what I found was required.

Attached is my Flange bolt example

Scott Baugh, CSWP
CAD Systems Manager
Dapco, INC

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376