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IDW's/BOM's/General Workflow Guidelines

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Message 1 of 7
RogerTheShrubber
749 Views, 6 Replies

IDW's/BOM's/General Workflow Guidelines

I'm sure that this issue has been addressed, but I'm unable to locate any help on the subject. 

 

I create an IDW view of a subassembly by inserting the parent assembly, make it a non-associative view, then turn off visibility of unwanted subassemblies.  When later working in the model and adding a part to one of the non-visable sub-assemblies, that part becomes visable in the IDW views in which the subassembly was non-visable, requiting me to edit all veiws in which the subassembly was non-visible. This can be quite a number of instances.  Is there a way to prevent this?

 

I may have a more fundamental workflow problem:  I create assemblies composed of subassemblies that need to be detailed sperately.  I have found that in order to correctly create a structured BOM and to have the ballon lables to correspond to the structured BOM, I create the drawing views as described above.  If I would just insert the subassembly to detail it, I don't understand how to get it to relate the ballon labels in the subassembly view to my master BOM.  

6 REPLIES 6
Message 2 of 7
Cadmanto
in reply to: RogerTheShrubber

My first thought is why not create an assembly factory file and make iassembly members that have these parts turned on/off in the factory table.

Then in the drawing you will have views that represent the members showing only the parts you want shown.

 

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Scott McFadden
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Message 3 of 7
karthur1
in reply to: RogerTheShrubber


@RogerTheShrubber wrote:

.......

I create an IDW view of a subassembly by inserting the parent assembly, make it a non-associative view, then turn off visibility of unwanted subassemblies.  When later working in the model and adding a part to one of the non-visable sub-assemblies, that part becomes visable in the IDW views in which the subassembly was non-visable, requiting me to edit all veiws in which the subassembly was non-visible. This can be quite a number of instances.  Is there a way to prevent this?

 


Why not make a view representation, then lock it when you get it the way you want. Now place an ASSOCIATIVE view.  The ONLY time the view will then change is when you make a change to the view rep (you have to unlock it first, change it, then lock it back).

You can place a parts list based on this view representation, but Inventor DOES NOT totally support this. It will warn you about it when you place a parts list based on a view rep and the quantites in the parts list could be mis-leading.

 

 


 

I may have a more fundamental workflow problem:  I create assemblies composed of subassemblies that need to be detailed sperately.  I have found that in order to correctly create a structured BOM and to have the ballon lables to correspond to the structured BOM, I create the drawing views as described above.  If I would just insert the subassembly to detail it, I don't understand how to get it to relate the ballon labels in the subassembly view to my master BOM.  


Can you show a screen shot of what you mean by " I don't understand how to get it to relate the ballon labels in the subassembly view to my master BOM"?

 

Thanks,

Kirk

 

 

Message 4 of 7
RogerTheShrubber
in reply to: karthur1

Thanks Kirk.

 

I don't have a screenshot to send, but let me provide a longwinded explanation of my workflow:

 

My Top Assembly (Top.iam)  consists of Assembly 1(Assembly 1.iam) and Assembly 2 (Assembly 2.iam).   Assembly 1 is composed of Parts 1.1, 1.2, 1.3.....  Assembly 2 is composed of Part 2.1, 2.2, 2.3....

 

I have a structured BOM.  In Sheet 1 I place Top.iam in a view, create a Parts List referencing this view and I can balloon Item 1 and 2. I can edit the parts list, expanding the assemblies to show the individual parts and I can balloon Item 1.1, 1.2, etc.  OK - this is my Top Assembly view, I compress the Parts List so that the balloons are 1 and 2.

 

I create Sheet 2 and create view of Assembly 1 using Assembly 1.iam.  I create a Parts List referencing this view and get Items 1, 2, 3.  I want the Parts List to read Item 1.1, 1.2.... I delete that view and create a view using Top.iam, make it associative and turn off visibility of Assembly 2.  Create Parts List referencing this view, expand the structure of the parts list, turning off visibility lines so that only Items 1.1, 1.2...are visible.  Balloon the parts in the view and get 1.1, 1.2...GOOD.

 

Return to Sheet 1 and the Parts List is expanded to show Items 1.1, 1.2....and balloons read the same.  Turn of visibility of the Items 1.1, 1.2...in the parts list.  I have to override the balloon to read 1. GOOD.

 

Sheet 3 has view w/ Top.iam, visibility of Assembly 1 turned off.  Parts List references this view, expand list to show 2.1, 2.2...Balloon Items 2.1, 2.2...in view. GOOD.

 

I return to Sheets 1 and 2 and the Parts List has now expanded to include Items 2.1, 2.2...I turn off the visibility of these lines in the Parts List because I don't want them shown on these sheets. GOOD.

 

So now I make an edit to my model, adding a part to Assembly 1.

 

On Sheet 3, my detail of Assembly 2 now has the new part showing.  I am forced to make edits to the view and the Parts List.

 

Since often my top assembly consists of Assemblies 1-10, and I've used the method described above to create the details for these assemblies, there are a lot of views and parts lists to edit.

 

It would be nice if I could use Assemby1.iam to create the view, Top.iam to create the parts list and somehow have the balloons read 1.1, 1.2...when I label the view.  That is what I mean when I say  I don't understand how to get it (inventor)  to relate the balloon labels in the subassembly view (View Assembly1.iam) to my master BOM (Parts List referencing Top.iam)

 

I appreciate your suggestion to create the view reps in the model.  I will try that in the future.

 

Possible workaround to the Parts List problem you describe:  I often create a shaded isometric on the sheet.  This view could be the Master View Rep with unwanted subassemblies turned off.  The Parts List references this view.  Now hopefully all your QTY's are correct.  If you don't include a shaded isometric on the sheet, you can move it 'off-sheet' and still have the Parts List reference it.

Message 5 of 7
karthur1
in reply to: RogerTheShrubber


@RogerTheShrubber wrote:

... 

I create Sheet 2 and create view of Assembly 1 using Assembly 1.iam.  I create a Parts List referencing this view and get Items 1, 2, 3.  I want the Parts List to read Item 1.1, 1.2.... I delete that view and create a view using Top.iam, make it associative and turn off visibility of Assembly 2.....


When you place the view on sheet 2 of assembly 1 and use that view to create a parts list..... it is going to show 1,2,3,4...etc..... that's just the way it is.  Just like on sheet 1, when you create a parts list using Top.iam, it will show 1,2,3,4.... etc.   

 

Inventor is built around the idea of "One part - One drawing".  You can hide things, supress things, change the quantity.... etc but the more you do it, the more trouble it becomes and the more likely you are to make a mistake.  Or, you spend more time correcting your idw, than it took to actually edit the model.

 

Don't fight it, go with it... it wll be much easier.

 

There has been much written here about users wanting to have multiple details on a single sheet.  You can do that without any problem, but Inventor does not support (currently) having the item number as a selectable text property. This will prevent having an item number in the view label that correlates with the item number in the parts list.

 

The easiest way around all this, is DO NOT use the item number. Just use the part number, that way it all will stay linked and you dont have to do a bunch of editing to get it there. Is the item number really necessary? 

 


@RogerTheShrubber wrote:

.. 

Possible workaround to the Parts List problem you describe:  I often create a shaded isometric on the sheet.  This view could be the Master View Rep with unwanted subassemblies turned off.  The Parts List references this view.  Now hopefully all your QTY's are correct.  If you don't include a shaded isometric on the sheet, you can move it 'off-sheet' and still have the Parts List reference it.


This is the warning I was talking about (see below).  This from clicking the "Filter" icon in the parts list dialog.  You do know that you do not have to have a view on the sheet in order to use it for a parts list to reference it, right?

 

2014-01-08_1710.png

 

Kirk

 

 

Message 6 of 7
RogerTheShrubber
in reply to: karthur1

Thanks Kirk.

----------------------

Don't fight it, go with it... it wll be much easier.

 

I'm trying to find the path of least resistance for creating drawing sets of assemblies with structured BOM that include accurate Parts List.  I seem to be close to it, just having issues with the drawing set that pop up when I make edits to the model.  Thanks for the suggestions on View Reps and Parts List Filters.  It seems that it should solve most of my issues.

Message 7 of 7
karthur1
in reply to: RogerTheShrubber

Be careful with the parts list filters.  They can be very dangerous and your quantites may not be accurate.

 

I learned this the hard way.

 

Kirk

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