Some problems with BOM's

[RBasniak]

Hi everyone,

I'm new in this forum and I have some questions for you. So, I hope to be helpful sometimes as well

1 - I'm having some troubles with my BOM's, I usually create an exploded view and add another sheet to create the BOM over there. But when I insert the BM, it comes classified by item number, and it's no so useful to me because I need the BOM classified by the part's code. I thought it wasn't a big problem because I can do it using the MS Excel's tools, and it works well. But doing that, the item number column don't stay classified alphabetically, I know it's a stantard from Excel, and it's right. But if I change the item number in this BOM I think SolidWorks must update the item numbers in the balloons automatically. Am I correct? I change the item numbers in the BOM and the exploded views don't update!!!

2 - My other question about BOM's is if is there any way to externalize the BOM. Something like create a linked .XLS file with the BOM. One of the many reasons that I need it is because the BOM of some machines are a little big Some BOM's can have up to 10 pages... and I can't divide this BOM in parts inside the SolidWorks... Is there a way to export the BOM to an external file?

Well, I think it's enough for now
Thanks,

Rodrigo Basniak
Curitiba, PR
Brazil

 

[Demojock]

Hi there

here is the first round of answers before the API boys start to talk about macros.

1. SW should change the ballons automatically if you change there number in the BOM, and vice-verca, if you change a balloon number it should update the BOM, you may have an option switched off that automatically updates the BOM with the model, (although this is not a bad idea if the assemblies are as big as you say.) but either way, it sounds s if you need some sort of macro either in excel or SW to solve this prob.

2. dead easy this one, if you click on the BOM and then go to save-as, it will have the option to save an excel file. the only problem is that this breaks the link to original drawing, its a snapshot of the assembly at that time.
You can also use the SW explorer to generate a BOM without having to create a drawing and this can also be saved as an EXcel spreadsheet.

anything more advanced woult either require the use of a macor/api script, or a document/product data mangement piece of software

hope this helps

demojock...

 

[dsi]

If you want your BOM created in a separate xls file and link it in SolidWorks, just do an Insert > Object, select Create From File, and pick the file. You have two display options. You can show the worksheet on the drawing or just display an icon link to the file. If you don't want the icon on your print, just move it off of the drawing sheet.

If you want to export the BOM, just double click the BOM and do a File > SaveAs. DimensionalSolutions@Core.com
While I welcome e-mail messages, please post all thread activity in these forums for the benefit of all members.

 

[SBaugh]

RBasniak,

I hope I'm understanding you correctly?

1 - When building your assembly at the model stage, is the way the BOM is built. If you add part "Z" first then it's the first Item Number in you BOM, and then you add part "A" second it's now the second item in your BOM...etc.

Since you want to control the BOM with a part code instead of a Item number. Have you tried to make a custom BOM? This away you will have a BOM to fit your parameters. You still have to build the assembly in the way I mentioned above though.

Everything comes back to the way you built your assembly. If you do not have any in-contexted parts, you can easily move your parts around the Feature Manager Tree (FMT) so it will show in the BOM the way your looking for.

2 - Is there a way to export the BOM to an external file?

Do a single click on the BOM so it is selected and then go to File, Save As.Don't double click it and activate the BOM since it can not be saved when activated.

Hope that helps, Scott Baugh, CSWP
George Koch Sons,LLC
Evansville, IN 47714
sjb@kochllc.com

 

[RBasniak]

Hello, thanks for all of you!!

Well, the problem with the number of balloons is that I have some sub-assemblies inserted in the main assembly... I think just insert them in a main assembly in the correct ballon item order won't work, because in the BOM I don't need all of them together :-( I think I'll need some programing on this :-( Does anyone knows a site where I can find some information about macro programing in SW. Anything... some tutorials would be apreciated.

I did use the save as command in my BOM. But in the custom fields I have some fields that use the name of dimensions... i.e. I work with parts made of sheet metals bended, and I have a field in my BOM called DESCRIPTION where I put the dimensions of this metal sheet flattened, but I use some nice resources of SW I don't put these values manually, I just click on the dimension on the model and and a link is created in the field with that dinension, in the BOM it appears right, but when I save the BOM to an external file the values won't come in numeric values, they come this way:

CHAPA #"D1@Base-Extrude@2930-02-0.SLDPRT" x "D4@Sketch1@2930-02-00.SLDPRT" x "D6@Sketch1@2930-02-00.SLDPRT"

So I can't use that :-( Is anyone knows a way to correct it I would like to know... if not, no problem, 'cause I discovered that I can export the BOM to an DWG file... and there the values appear correctly... it's not the better way to work with it, but it's a way ;-)

Thanks people,

Rodrigo Basniak
Curitiba, PR
Brazil

 

[RBasniak]

Wow, Sorry people.. forget my questions about source code... I saw it on FAQ s-)

 

[dsi]

SolidWorks 2001 SP9 fixed the display problem in the BOM. Before the latest realease, you would see the entire link to the dimension rather than the display values. They recoded the BOM so that you see the display values when you activate the BOM.

If you need help working through any code problems, just post a new thread. DimensionalSolutions@Core.com
While I welcome e-mail messages, please post all thread activity in these forums for the benefit of all members.

 

[Bovee]

Demojock,

How do you use SolidWorks Explorer to generate a BOM without the use of a drawing?