more BOM issues

[JimSteinmeyer]

Ok I am still struggling with the BOM feature in Inventor. I have an assembly with two subassemblys that are each repeated twice. A couple of parts are in both assemblies. I would like to show a BOM of all parts and their TOTAL quantitys. I am able to extend both subassemblies so that all components show in the BOM, great. However when the assemblies are first exploded they show the hirearcy of 4.0, 4.1, 4.2 ect. which would probably kind of work but the numbers started with 4 and skipped a few numbers, Simple- renumber, Now the numbers run from 1 to 14 with the parts common to both sub assemblies showing twice and no subassembly heirarcy showing at all, no 4.0, 4.1... just 1 to 14. The other problem when we loose the heiarcy is that it shows a qty of 2 for each subassy and the correct number of parts for EACH sub, but you don't know which parts belong to which subassy and the listed qty is half the qty needed in the top level assy. I have messed with the grouping, but that only seems to make things worse.

If any one understands what I have said, do you have any suggestions?

Thank you

Jim

Inventor 2012

Vault 2012

win 7

[jtylerbc]

Try doing the renumber from the assembly's Bill of Materials, instead of the Parts List, and see if that fixes your heirarchy problem.  It seems to do so for me in the example I tried.

Also, your screen shot shows a Parts List dialog box, but you mention BOM in your question.  Be careful with these two terms when referring to Inventor - although in most people's heads they mean pretty much the same thing, in Inventor they're two seperate (but related) concepts.  Not trying to be picky about terminology, but the differences between the two could lead to people giving you the wrong help.

[JimSteinmeyer]

Is there a way to place a BOM list in the drawing? Would that work mort like what I am wanting?

Thank you

[jtylerbc · Accepted solution]

Actually, the Parts List is the way to put the BOM information in the drawing.  Think of it as the BOM being the raw data from the assembly, where the Parts List is the version formatted into a table to show on a particular drawing.

The BOM contains the "master" version of all the information - the Parts List just echoes what the BOM says, unless you have overridden it.  Because the BOM is the master, there are some things that you have better control of there.  In this case, if you do your renumbering in the BOM, and not the Parts List, it should fix your heirarchy numbering issue, since (unless you renumber the Parts List) the numbers in the Parts List match the ones in the BOM.

If you do the BOM renumbering after having already placed a Parts List, you'll probably have to use Sort in the Parts List to put the item numbers back in the proper order.

[ozitag]

In the assembly, you can choose a couple of different types of BOM lists, ie structured and parts only. If you just want the parts, use the parts only BOM list, if you want the assemblys etc (4.0, 4.1 etc) then use structured. (Right click on the tab and enable/disable those you want.

Fix up the list how you want it in the assembly with all the item numbers, sorting etc.

Then, in the drawing choose a parts list, which refers to the BOM of the assembly. You can then choose whether you want the structured or the parts only again, but you can only use one of them for that drawing. 

I see also in the screen shot you posted that there are blue item numbers. This means you have changed them in the parts list and they are different to what is in the BOM. If you want to save them back to the BOM, you can select the icon second to the right in the parts list editor window and it will save the item number changes back. If you have already changed them and want what is in the BOM, right click on the cell and select static value.

Hope this helps.

Ozitag

[JimSteinmeyer]

Ozitag,

The two blue lines are grouped. These are the two parts that are in all 4 (two sets of two subs) of the sub assemblies and the qty, shows the correct number for and one sub. THe grayed lines are the two subs that I have decided to not show as the parts are in the list and would be confusing.

I will now attempt to use your suggestions and see where I get.

Thanks guys.

Jim

[ozitag]

I mean't the cells that have a dark blue border not the light blue lines.

Ozitag.

[JimSteinmeyer]

Ok, I have things showing as I want them with one little catch. The top level assy I have been working with is not actually not a top level, it is a sub of another assy and to have all the subassy drawings linked to the top level I have been creating a drawing of this assembly on a new sheet of the over all top level assembly. In doing this I find that I am not allowed to set the parts list to parts only in the drawing, No matter what I select, when the assembly is selected it reverts to structured which the top-top level drawing is. Then the block grays out and no further selection is available. I am assuming that only one type of parts list is allowed per drawing.

Working on this created another question, what is the difference between parts and parts legacy or structured and structured legacy in these lists?

Thank you

[JimSteinmeyer]

The dark blue ones were after I had used the renumber button. I did not manually over write any of the numbers, that was my last resort.

Thank you

[jtylerbc]

Afraid that someone else will have to answer your "Legacy" question - those were already considered obsolete formats by the time I started using Inventor, so I've never touched them.

You are correct that you can't place a parts-only list on the same drawing sheet as a structured list.  You may be able to in another sheet in the same drawing - I'm a bit fuzzy on that.  You definitely can place it in a second drawing file.

As I recall, there is a workaround where you create the second parts list elsewhere, then copy and paste it into the sheet with your structured list.  For some odd reason, this is allowed, but initially creating it there isn't.

[ozitag]

That is right, you can only have one type of parts list per drawing. Start another drawing if you want the other type.

Someone else will have to answer the legacy questions.  Never used them so don't know.

As far as the blue border is concerned, whenever there is a forced change to the parts list (ie in the drawing), a blue border is created. Blue bordered item numbers can be saved back to the BOM with the second to right icon. So whether you changed them individually or with the renumber, they were changed in the Parts list editor window, which means there is a difference to the BOM. If you want the BOM value, you can right click on the cell and select static value.

Regards,

Ozitag.

[JimSteinmeyer]

Thank you. That is good information to know.