Problems with BOM 3

[mkmech]

When I edit my BOM in Excel, exit after editing and rebuild the drawing file, the BOM expands to list the same items again and sometimes 3 times. For example, if I had 5 rown in the original BOM, it now has 10 or even 15 at times. The same 5 items are repeated 2 or 3 times. Why could this be happening? This also happens if I edit one of the parts and go back to the drawing.

Thanks

 

[Standing]

mkmech,
Try this, in the SolidWorks tree delete your BOM, then reinsert it. If that does not work, then try using the original Excel BOM that came with SolidWorks.
Good luck,


Bradley

 

[SBaugh]

Are you saying the BOM is updating and removing your changes or is the BOM repeating itself and your getting multiple copies of the BOM in the drawing?

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[mackman]

mkmech

if you are using SW2004 or earlier, and using the excel based bom. You do not want to edit the bom through excel, or by double clicking and editing the bom in the drawing. Because, when the assembly and drawing updates, it tries to overwrite all the info you typed into the bom and match what is in the feature tree. This could be causing other problems as well.

 

[manxJim]

This can happen if you delete the columns from the standard SolidWorks BOM
Don’t delete the columns you don’t need just hide them

 

[CorBlimeyLimey]

This has been discussed in depth before, but the only reference I can find is thread559-28539 which did not resolve anything.

Scott, do you remember anything about this problem.

mkmech ... what version & SP of SW are you using.

& all the best.

 

[mkmech]

Thanks everyone. I am using SP01+.

Scott, the BOM is repeating itself and I am gettinmg the same list under the original list repeated 2-3 times or even 4 times.

manxjim, I am indeed deleting some columns from the std Excel template and adding some of my own columns. I will try hiding the columns instead of deleting them as you suggested.

mackman, how else do I edit the BOM if not through Excel? I am using SW01+.

Thanks

 

[macduff]

All,
Editing the Excel is a snap. But you need to follow these basic rules:

1) When you need to add parts in your Excel BOM that are NOT SW parts you must insert them BEFORE or AFTER the SW parts. Inserting Non SW parts/items (i.e. Loctite, Grease etc...) in between will be deleted When your drawing is updated.

2) When you do add non SW parts, try to color the text in Excel (like the color RED for contrast). This allows you and other users know that these items were added manually and not affected by drawing updates.

3) If you don't like the way the parts are displayed in your Excel drawing BOM, go to your main assembly and rearrange the parts in the command manager tree. Then update or recreate your BOM in your drawing.

4) Pay attention to the configuration properties when inserting the Excel BOM. there are many options to choose.
"Show parts only"
"Show top level subassemblies and parts only"
"Show assemblies and parts in an indented list"
Depending on which one you select; it will give you different results and will sometimes repeat part numbers.

Hope this helps.


Macduff
Meggitt Airdynamics Inc.
Dell Precision 370
SW2004 Pro SP4.1
XP Pro SP2.0
NIVIDA Quadro FX 1300

 

[SBaugh]

Dont' delete the columns that are there by default or the $END symbol. Simply hide the default columns and add new ones as needed for your columns. But keep the $END to the right of you new columns or the BOM will fail.

Because you removed the default columns is why your getting the problem.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[mackman]

mkmech

have you created BOM templates? You can make different templates for different types of Boms. If you have to add parts to a BOM that are not in your assembly, I would actually create the BOM in excel, and then insert an object and browse for the excel file. The only problem with that is the Bom is no longer linked to the drawing. like I said before, SolidWorks overwrites the BOM everytime the BOM needs to be updated because of a drawing or assembly change. The SolidWorks BOM is tied directly to the feature tree ie. the parts and order of the parts in the tree is how they show up in the BOM.

 

[MElam]

If you are adding items to the BOM that are not in your assembly, many people handle this by creating empty parts (no geometry, only custom props) and add them to the assembly.

This way there are no manual updates to the BOM and the parts can be used repeatedly - instead of repeatedly making manual updates.

 

[macduff]

mackman,
I played around with the Solidworks BOM and prefer not to use it. It's not very user friendly and cannot modify to our company standard heights and widths. I know there are options to modify these, but my changes to not save correctly when inserted into a new drawing.

All an all, I wish both BOM's (Excel and SW) were more user friendly.

Best,

Macduff
Meggitt Airdynamics Inc.
Dell Precision 370
SW2004 Pro SP4.1
XP Pro SP2.0
NIVIDA Quadro FX 1300

 

[mkmech]

macduff, what, if not SW, do you use for creating BOM?

 

[macduff]

mkmech,
There are 2 types of BOM's for Solidworks.

1) MS Excel BOM: This has been around since the birth (?) of SW. And is still an option in SW2004 and SW2005. You insert it just like a SW BOM. It has default templates you can use and modify. This is the one I prefer to use.

2) Solidworks BOM: This is an off shoot of the Excel BOM (changing code and what not) that Solidworks created back in SW2004(?). It has many options, and in my eyes very cumbersome. It has default templates to use and modify. I choose not to use this one.

Both of these options are available under "Insert"/"Tables" when creating a BOM in a drawing.

Best,


Macduff
Meggitt Airdynamics Inc.
Dell Precision 370
SW2004 Pro SP4.1
XP Pro SP2.0
NIVIDA Quadro FX 1300

 

[mackman]

I agree with Macduff, the BOMs could be a little more user friendly. We use SW2004 and I still prefer the excel based bill of material. This was suppose to go away in 2005, is this true? mkmech, I find when I have trouble, I tend to make the Bom in an excel sheet outside of SolidWorks. Then insert the excel sheet as an object into the drawing. I also don't care for adding the empty parts to complete the BOM, just my opinion.

 

[macduff]

mackman,

You Wrote:
"This was suppose to go away in 2005, is this true?"

Nope, Exel BOM's are still available in SW2005. I hope someone gives us a heads-up if it goes away in SW2006. Because the SW BOM still needs help.

Regards,

Macduff
Meggitt Airdynamics Inc.
Dell Precision 370
SW2004 Pro SP4.1
XP Pro SP2.0
NIVIDA Quadro FX 1300

 

[ctopher]

I agree with Macduff. We rarely use BOM in SW. We use an Access database for BOM's (or PL's).

Chris
Sr. Mechanical Designer, CAD
SolidWorks 2005 SP0.1