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Creating non-associative Bill Of Matls
- Thread starter CADALL
- Start date
There are no simple "text" table features in Solidworks (why?).
One workaround:
- Create a new blank drawing
- Insert a revision table
- Save this table as a template
- Close the new drawing you just created (needn't save it)
- Insert the new rev table into any drawing
- Modify this table to your requirements
---- delete columns, rename etc etc
This table will cut and paste to other drawings
Solidworks really does need a dumb text table feature that we can use for anything- completely unassociated with models etc.
One workaround:
- Create a new blank drawing
- Insert a revision table
- Save this table as a template
- Close the new drawing you just created (needn't save it)
- Insert the new rev table into any drawing
- Modify this table to your requirements
---- delete columns, rename etc etc
This table will cut and paste to other drawings
Solidworks really does need a dumb text table feature that we can use for anything- completely unassociated with models etc.
Insert\Object\ - Create new\ - Microsoft Excel Worksheet.
Or
Insert\Object\ - Create from file - Browse for a pre-made Excel file that has your column headers in it.
Either way it will have association to the model in the drawing, like a BOM will have.
Regards,
Scott Baugh, CSWP![[pc2]](/data/assets/smilies/pc2.gif "[pc2] [pc2]")
3DVision Technologies
faq731-376
faq559-716 - SW Fora Users
Or
Insert\Object\ - Create from file - Browse for a pre-made Excel file that has your column headers in it.
Either way it will have association to the model in the drawing, like a BOM will have.
Regards,
Scott Baugh, CSWP
3DVision Technologies
faq731-376
faq559-716 - SW Fora Users
CorBlimeyLimey
Mechanical
CADALL & solidmail ... SW & other modelling packages have gone to great lengths to create associative BOMs. Why would you want to go backwards and use non-associative ones?
If you really need it, you can easily insert an OLE compliant Excel or Word document as per SBaughs post & type in whatever you want. Or you could really go backwards & use AutoCAD?![[bigsmile]](/data/assets/smilies/bigsmile.gif "[bigsmile] [bigsmile]")
Also switching off the Automatic update of BOM under Tools > Options > Document properties > Detailing may help you.
BTW, in both the Excel & SW BOM, you can add whatever you want, but the entries will be lost if the BOM is updated, so you will have to make sure it is never updated.
![[cheers]](/data/assets/smilies/cheers.gif "[cheers] [cheers]")
If you really need it, you can easily insert an OLE compliant Excel or Word document as per SBaughs post & type in whatever you want. Or you could really go backwards & use AutoCAD?
Also switching off the Automatic update of BOM under Tools > Options > Document properties > Detailing may help you.
BTW, in both the Excel & SW BOM, you can add whatever you want, but the entries will be lost if the BOM is updated, so you will have to make sure it is never updated.
Good point CBL!
I was thinking something that will never have any association to the model. Even if you toggle that option. If a user was too turn it on by accident, then the BOM would or could be messed up and cause further problem, but it would be easier then manually entering all that data in.
Regards,
Scott Baugh, CSWP
3DVision Technologies
faq731-376
faq559-716 - SW Fora Users
I was thinking something that will never have any association to the model. Even if you toggle that option. If a user was too turn it on by accident, then the BOM would or could be messed up and cause further problem, but it would be easier then manually entering all that data in.
Regards,
Scott Baugh, CSWP
3DVision Technologies
faq731-376
faq559-716 - SW Fora Users
- Thread starter
- #6
FYI...Oh yes, I aggree, I would prefer associativity. But, I am drafting up several complex assembly drawings of cables and I don't want to model grease, sodder, flux, loctite, etc. just to show up in the BOM.
Product Designer of Contract
Product Designer of Contract
engAlright
Mechanical
Some random thoughts:
-if you want a 100% dissassociative BOM, Scott's suggestions is probably the safest bet
-if you want some of the items in your assembly to be in the BOM, but you have a lot of "manual" entries, you can insert a BOM then export to XL, enter in the extra data and re-import back in to the drawing as OLE object
-I haven't had too many problems with manual entries I've added to the Solidworks BOM being deleted - just add a row and type in the info that you need - any items subsequently added to the assembly will be added to the bottom of the BOM
-you could also create "dummy" parts that are empty, but have the correct part number, description and custom properties that you want then insert them in to the assembly (this was the only way to add oil, grease etc. to a BOM before the Solidworks BOM came to town)
-if you want a 100% dissassociative BOM, Scott's suggestions is probably the safest bet
-if you want some of the items in your assembly to be in the BOM, but you have a lot of "manual" entries, you can insert a BOM then export to XL, enter in the extra data and re-import back in to the drawing as OLE object
-I haven't had too many problems with manual entries I've added to the Solidworks BOM being deleted - just add a row and type in the info that you need - any items subsequently added to the assembly will be added to the bottom of the BOM
-you could also create "dummy" parts that are empty, but have the correct part number, description and custom properties that you want then insert them in to the assembly (this was the only way to add oil, grease etc. to a BOM before the Solidworks BOM came to town)
CADALL,
Dummy Parts, as engAlright mentioned, are the way to go. Just fill out the necessary info on the file properties and then drop and drag them into any assembly. That way you won't have to re-type the same information into a BOM everytime you want to use that item. I have placed these type of items (solders, loctites, greases, etc...) in our PDMWorks vault so that users here can drop and drag from the vault and the BOM is automatically filled in for them. It can't get much easier than that. If you are not using PDMWorks you could place these type of items in the design library for quick access.
Dummy Parts, as engAlright mentioned, are the way to go. Just fill out the necessary info on the file properties and then drop and drag them into any assembly. That way you won't have to re-type the same information into a BOM everytime you want to use that item. I have placed these type of items (solders, loctites, greases, etc...) in our PDMWorks vault so that users here can drop and drag from the vault and the BOM is automatically filled in for them. It can't get much easier than that. If you are not using PDMWorks you could place these type of items in the design library for quick access.
engAlright
Mechanical
Only problem we've had with dummy parts has been with parts that are borderline as to whether they need to be modelled or not i.e. weather stripping, seals, electrical components. Occasionally someone will come along and want to model a part that was a dummy part, now in whatever assembly used that dummy part there will be an actual physical model in there where it shouldn't be.
Not a big deal, just something to be aware of.
Not a big deal, just something to be aware of.
I also vote for "dummy" parts (I like to call them phantom parts because they're not dummy at all!). It's the only way of get consistency to your project. You don't need to model anything, but the required information will be there.
You invest a lot money and effort creating documents (parts, assemblies, drawing) that share the same database so you don't loose track on your design. Don't throw it away now creating dumb (now the right word!) uncontroled documents.
You can even have custom properties that give the exact information about the item to apply. Example you insert 1 phantom part called "Loctite 222", Qty to assemble "0.5", units "gr"; 5 parts called "Cable FV 2.5 blue", Qty to assemble "2", units "m". This information can be outputed in you boom and is controled at part/assembly level, giving consistency to your design.
Regards
You invest a lot money and effort creating documents (parts, assemblies, drawing) that share the same database so you don't loose track on your design. Don't throw it away now creating dumb (now the right word!) uncontroled documents.
You can even have custom properties that give the exact information about the item to apply. Example you insert 1 phantom part called "Loctite 222", Qty to assemble "0.5", units "gr"; 5 parts called "Cable FV 2.5 blue", Qty to assemble "2", units "m". This information can be outputed in you boom and is controled at part/assembly level, giving consistency to your design.
Regards
Gentlemen,
Many companies have problems keeping MS Office and programs like Solidworks in sync (compatible releases) so Excel is not always an option.
2D drawing packages should be able to generate text that can be fixed and easily formatted, for tabulations etc that have absolutely no physical relationship to a model.
We have to use AutoCAD to generate text tabulation drawings (200+ combinations/configs) at the moment because we can't do it in SW.
If SW can connect tables to models, they should be able to provide a table that doesn't without difficulty. The current BOM is too restrictive for this purpose, unfortunately.
Many companies have problems keeping MS Office and programs like Solidworks in sync (compatible releases) so Excel is not always an option.
2D drawing packages should be able to generate text that can be fixed and easily formatted, for tabulations etc that have absolutely no physical relationship to a model.
We have to use AutoCAD to generate text tabulation drawings (200+ combinations/configs) at the moment because we can't do it in SW.
If SW can connect tables to models, they should be able to provide a table that doesn't without difficulty. The current BOM is too restrictive for this purpose, unfortunately.
SOLIDMAIL,
Using Design Tables in Solidworks you can create tabulation drawings with ease. Plus you will have a solid model of each instance. We use design tables alot in our drawings.
Although I think solidworks should make anchor points for design tables so that they can be fixed in the drawing without too much trouble.
Just some thoughts.
A man should look for what is, and not for what he thinks should be. -Albert Einstein
A person who never made a mistake never tried anything new. -Albert Einstein
Using Design Tables in Solidworks you can create tabulation drawings with ease. Plus you will have a solid model of each instance. We use design tables alot in our drawings.
Although I think solidworks should make anchor points for design tables so that they can be fixed in the drawing without too much trouble.
Just some thoughts.
A man should look for what is, and not for what he thinks should be. -Albert Einstein
A person who never made a mistake never tried anything new. -Albert Einstein
If you use the Excel Table it is a problem because of the OLE limitation which is not a SW issue but rather a Microsoft. You can find this at the SW knowledge base.
The new Table BOM is very powerful but is still new, but is getting better.
DT as your tabulation? - Why not just use my method above for inserting a blank excel sheet into the drawing and using that instead. There is an OLE limitation still. A DT is not setup in the same fashion as a BOM is.
Regards,
Scott Baugh, CSWP
3DVision Technologies
faq731-376
faq559-716 - SW Fora Users
The new Table BOM is very powerful but is still new, but is getting better.
DT as your tabulation? - Why not just use my method above for inserting a blank excel sheet into the drawing and using that instead. There is an OLE limitation still. A DT is not setup in the same fashion as a BOM is.
Regards,
Scott Baugh, CSWP
3DVision Technologies
faq731-376
faq559-716 - SW Fora Users
SBAUGH,
We use design tables because we need to have each tabulated item as a model in our assemblies.
Unless I am mistaken...If I insert a new excel table into the drawing it will not generate model items for me.
Afterthought....Can I use the same header codes that the design table uses in a blank excel table? If so, I can see how it would generate models from that.
A man should look for what is, and not for what he thinks should be. -Albert Einstein
A person who never made a mistake never tried anything new. -Albert Einstein
We use design tables because we need to have each tabulated item as a model in our assemblies.
Unless I am mistaken...If I insert a new excel table into the drawing it will not generate model items for me.
Afterthought....Can I use the same header codes that the design table uses in a blank excel table? If so, I can see how it would generate models from that.
A man should look for what is, and not for what he thinks should be. -Albert Einstein
A person who never made a mistake never tried anything new. -Albert Einstein
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