.idw file Parts List call out and filtering

[dwyingling]

In a .idw file is there way to call out parts and assemblies, by call out I mean balloon them and have the in the parts list, in one sheet and in another sheet have the parts of the assembly, you called out early, be called out?

Another way of putting it is; is there a way to have the Parts List in an .idw file show the only what is in a certain Level of Detail (LOD)?  Have it show only the parts and assemblies that are selected in the LOD with quantities.

I have I model of about 500 parts with several sub-assemblies, which I’m having a hard time making a parts list for.  In the one sheet I have parts and sub-assemblies that I want to call out.  When I try anything I only call out parts not any sub-assemblies.  So I made the sub-assemblies “Normal” in stead of “Phantom” in the BOM. The problem with that is when I want to call out the parts of the “Normal” sub-assembly in another sheet its only counting it as that one assembly not multiple parts. In the “Edit Parts List” I can expand the assembly, with the + button, to show each part but when I go back to where I want to just call out the assembly it is also expanded and calling out the parts not just the assembly.  I made a view rep for each LOD to filter only the parts I wanted but that doses’t change the parts list quantities and seems redundant since I already have a good LOD with proper parts and quantities.  I also tried to filter it by "Ballooned items only" but for some reason there are items that are said to be ballooned that aren't, on the current sheet at least. The parts list seems like it is a globe entity for the whole .idw file, when I need it to be separated for each sheet using the BOM as the globe standard.  Am I using the parts list for the wrong purpose, because it seems very difficult to do anything expect for simple assemblies?  

[mcgyvr]

#1-creating a single drawing for both parts and subassemblies is generally not a good idea.. The biggest reason IMO is if that drawing becomes corrupted (it does happen) you have lost all work.

But you can filter a parts list by design view reps but NOT LOD.. But in your model you can simply click on a LOD and select copy to design view rep..

Now if I'm understanding your problem and you want to keep the top level drawing and subassembly drawings in a single file you would do the following.

On the first sheet you place your top level assembly.iam file and place a parts list based on that model, then on the next sheet you place your subassembly.iam and a parts list for that, and on and on with more sheets for each subassy. The workflow is identical for trying to throw it all in 1 idw file or having a separate idw files for the top level assembly and another idw for the subassy.

[Dennis_Jeffrey]

Yes, to a degree. The degree depends on what version of Inventor you are using.

[dwyingling]

I understand you solution but the problem with that is the Parts list is the same for all sheets.  Even if I filter it by the view rep. technical all the parts are in the top assembly, when I only want to call out some parts and subassembly. So I did the whole changing the assemblies to "Normal" instead of "Phantom" in the BOM.  But that didn't help, when I wanted to call out the parts not the assemblies. 

I figured the best way to do this is to use a separate .idw for each view and filter it with "ballooned items only" or the "view rep."  And use the "Structured" and "Parts Only" BOM view options.  But that still doesn't change the quantities.

This just seems like a hassle, moving back in fourth between several .idw files.  Especially since my computer can't Handel much more than 3 or so .idw files open at a time.  It would be nice if the Parts List ballooning and "Part Only" or "Structure" were only based on that sheet instead of the whole .idw file.

Thanks for your help.

[dwyingling]

I'm using Inventor 2011 Professional

[mcgyvr · Accepted solution]

ntinney,

Let me try this again...

Start with sheet 1 (which will be the top level assembly base view and the parts list source is top level assembly) So place a parts list and make sure the source is that top level assembly

Then balloon the items. Now you have a ballooned drawing only showing the parts that make up the top level assembly.

Then sheet 2 (which will be one of your sub assemblies base view, and make sure the source for your parts list on that sheet is the sub assembly) So place your parts list on that sheet and make sure the source is that sub assembly. Then balloon the items. Now you have a ballooned drawing on sheet 2 only showing the parts that make up the sub assembly.

and on and on (new sheets) for each subassy. each sheet will have a parts list which shows the parts that make up that assy or subassy only. Seems you keep putting a parts list on each sheet that has only the top level as the source.

Sounds like a few days of training would be highly beneficial to you.

[mcgyvr]

A parts list filter is not required at all.

The way I use parts list filters ( and this is just one way) is as follows.

We have what is called a routing.. This routing is given to the assemblers which lists all the different steps required to build a product. It is broken down into "operations" where operation 1 is the first step, operation 2 is the next step,etc...

I set up a design view rep in my top level assembly called Operation 1 and another view rep called Operation 2. In operation 1 view rep I turn off the visibility of any part not required in that step. Then in the IDW I place my base view and use that operation 1 design view rep as the base view. Then I place my parts list and filter it to only show the parts used in operation 1 (by simply clicking on the parts list filter, selecting design view reps and selecting my operation 1 design view rep. Then sheet 2 of my IDW is for operation 2. The base view is design rep operation 2. The parts list on that sheet is filtered using the design view rep 2 and then it only shows the parts in operation 2,etc...

[dwyingling]

I think I got it now.  When I was making a parts list I was clicking on the view I wanted to list.   By default it was going to the top level assembly.  If I don't click on the view and find the assembly I want in the browser, it does everything I wanted it to do in the first place.

Thank you for your help.

I could use a few day of training but my company has a hard time justifying it.  I guess they rather pay for me to star at my computer screen than pay for the training.

[hansome_one]

Heyyy, that is a great way for your step process.     Some of our routing process's are similar. I just wish that would translate down to the part level for features!!!!!!  

OK just got the filter to work. Question, now does the filter ONLY go with the view on the sheet, so when i create my second sheet and use the same base view on the 2nd sheet the filter will not apply.

OK the filter apply's to the 2nd sheet. Any other tips on set up????

[jdmech]

This still doesn't answer the question of accurate 'part quantity'. The View Rep filtering is a very handy tool that I use often but there doesn't seem to be any solution to multiple assemblies in one .IDW and show accurate part quantities within multiple parts lists. What I mean is this - when a top level assembly is placed into a base view on Sheet 1, then a parts list is placed on Sheet 2, all the part quantities reflect the top level assembly. Now, add Sheet 3. Drop a new base view of a view rep from of the top level assembly. Now place a new parts list representing the Sheet 3 on to Sheet 4. Examine and compare the part quantities of both parts lists and you'll find that the part quantities listed in the second parts list are false according to the view rep shown on Sheet 3. The part quantities are still representing the original top level assembly on Sheet 1. This is very frustrating and could be streamlined and organized better if multiple parts lists could be placed accurately into one .IDW that reflect either LOD's or 'parts visible' in view reps.

IMO Respectfully - jdmech

[dwyingling]

To jdmech,

I think what your saying is the same problem I was having.  I'll try and reexplain it, let me know if I'm not understanding the problem correctly. 

By doing what you said even when you filter it with a different "view rep", and place it on another sheet, you will always be selection the top level assembly by default.  Even if you make a parts list on the same sheet and click the view you want under "source" you will still always select the top level assembly.

What you want to do is:

1. Click on "Parts List"

2. Under "Source" click the " Browse for file" button and from their find your lower level assembly

3. I then select "Parts Only" under "BOM View" because thats what I have set up

By doing that it only shows that parts and quantities of that lower assembly without any filtering needed.  This means the main part in getting the proper parts in the assemblies and sub-assemblies you want.