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Assembly Drawings, how to show Available options via Configurations?

Question asked by Tyler Harding on Feb 2, 2021
Latest reply on Feb 2, 2021 by Jim Sculley

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We have a top level Assembly Drawing, with lets say 50 parts. We'll call this PN 123456-####

Our standard product might be 123456-1111. Let's say the last digit corresponds to a NA power cord.

We'll also offer an EU power cord, which would make this 123456-1112

Every digit after the "-" in the part number, corresponds to an available option.

On our assembly drawing, if I only want to show 1 assembly, let's say 123456-1111, is there a way to stack an EU balloon, on that NA power cord that is shown?

Because it's a different configuration, that EU power cord is suppressed, and I can't seem to balloon it unfortunately. I wish you could link balloons to your BOM directly, instead of just the model itself, which is suppressed.

What I'm trying to avoid is excess complete assembly models on a single drawing.

Our BOM is showing every configuration in case that matters. Shows the BOM for every configuration.

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Josh Brady Feb 2, 2021 11:04 AM

Instead of suppressing, you could keep it unsuppressed and then hide it in the drawing view after you have attached the stacked balloon to it. You would need a special config of the assembly where everything is unsuppressed, but that config wouldn't have to be shown in the BOM.

Edit: Might not work... I just remembered that I think any annotation attached to a part when you hide it gets hidden as well. Maybe you could just change it to a phantom line font?

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Tyler Harding @ Josh Brady on Feb 2, 2021 11:52 AM

So I've explored this option already. I start by creating a "Master BOM" configuration. Everything turned on. It does technically work, but Solidworks doesn't play well with this. Time consuming and buggy.

I'm actually exploring Display States with the configuration I want shown, to just show those options, using hidden lines like you suggested. This isn't a bad option.

This does indeed work if there are only 1-2 options. I can even set the view to show component lines as phantom lines.

I guess what I really want to do, is to combine some ITEM numbers in my BOM. To have ITEMs 3-6 combine into ITEM 3, and then the rest to reorder accordingly. The issue is you can't skip ITEM number rows on real parts. You can only skip on manually added rows.

Man that would literally solve everything for me.

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Jim Sculley @ Josh Brady on Feb 2, 2021 11:23 AM

Josh Brady wrote:

Edit: Might not work... I just remembered that I think any annotation attached to a part when you hide it gets hidden as well.

Correct. And when you stack the balloon

and then switch to a display state that hides the component, it seems to work

but a rebuild causes the balloon to go danging

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Jim Sculley @ Josh Brady on Feb 2, 2021 11:29 AM

And, to add insult to injury, the Knowledge Base has this:

Solution Id: S-06385
Product: SolidWorks Office Professional 2006
Created: 4/13/2006
Technically Reviewed Date: 4/5/2017
Area: Drawings
Sub-Area: Balloon

Question: Is it possible to attach a balloon to a part that contains no geometry and have the balloon update with changes to a bill of materials (BOM)?

Answer: Balloons need to attach to bodies so it is not possible to create a balloon for a part that contains no geometry. A possible solution to this would be to create a body within the part. In the drawing a balloon could be added to this body. If the body is then hidden the balloon will display the item number and update with changes to a BOM.

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Tyler Harding @ Jim Sculley on Feb 2, 2021 11:36 AM

I've found you can have the balloon stick to the origin of a part with no geometry. I do this for threadlocker call outs.

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Kevin Chandler Feb 2, 2021 12:28 PM

Hello,

Add the EU configuration outside of the drawing's border and crop its view so only the cord displays.
Drag the cropped EU cord into the title block and in its view's properties, set it to be linked to the main BOM.
Add a balloon to the cropped EU cord.
Add a note linked to the cropped EU cord's view (pointing at the EU cord)
1. The note reads "IN LIEU OF " then click the balloon of the US cord.
  As an alternative:
  1. Place another US assy view outside of the title block and balloon the US cord (view linked to the main BOM)
  2. Change the balloon to item number only, no border
  3. The note reads instead "IN LIEU OF ITEM " then click the no-border balloon of the US cord
    This is what this note is doing:

Kevin

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6 Replies

Josh Brady Feb 2, 2021 11:04 AM
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Correct Answer
Instead of suppressing, you could keep it unsuppressed and then hide it in the drawing view after you have attached the stacked balloon to it. You would need a special config of the assembly where everything is unsuppressed, but that config wouldn't have to be shown in the BOM.

Edit: Might not work... I just remembered that I think any annotation attached to a part when you hide it gets hidden as well. Maybe you could just change it to a phantom line font?
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- Tyler Harding @ Josh Brady on Feb 2, 2021 11:52 AM
  Mark Correct
  Correct Answer
  So I've explored this option already. I start by creating a "Master BOM" configuration. Everything turned on. It does technically work, but Solidworks doesn't play well with this. Time consuming and buggy.
  
  I'm actually exploring Display States with the configuration I want shown, to just show those options, using hidden lines like you suggested. This isn't a bad option.
  This does indeed work if there are only 1-2 options. I can even set the view to show component lines as phantom lines.
  
  I guess what I really want to do, is to combine some ITEM numbers in my BOM. To have ITEMs 3-6 combine into ITEM 3, and then the rest to reorder accordingly. The issue is you can't skip ITEM number rows on real parts. You can only skip on manually added rows.
  
  Man that would literally solve everything for me.
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- Jim Sculley @ Josh Brady on Feb 2, 2021 11:23 AM
  Mark Correct
  Correct Answer
  Josh Brady wrote:
  
  Edit: Might not work... I just remembered that I think any annotation attached to a part when you hide it gets hidden as well.
  Correct. And when you stack the balloon
  
  and then switch to a display state that hides the component, it seems to work
  
  but a rebuild causes the balloon to go danging
  Like • Show 0 Likes0
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- Jim Sculley @ Josh Brady on Feb 2, 2021 11:29 AM
  Mark Correct
  Correct Answer
  And, to add insult to injury, the Knowledge Base has this:
  
  Solution Id: S-06385
  Product: SolidWorks Office Professional 2006
  Created: 4/13/2006
  Technically Reviewed Date: 4/5/2017
  Area: Drawings
  Sub-Area: Balloon
  
  Question: Is it possible to attach a balloon to a part that contains no geometry and have the balloon update with changes to a bill of materials (BOM)?
  
  Answer: Balloons need to attach to bodies so it is not possible to create a balloon for a part that contains no geometry. A possible solution to this would be to create a body within the part. In the drawing a balloon could be added to this body. If the body is then hidden the balloon will display the item number and update with changes to a BOM.
  Like • Show 0 Likes0
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  - Tyler Harding @ Jim Sculley on Feb 2, 2021 11:36 AM
    Mark Correct
    Correct Answer
    I've found you can have the balloon stick to the origin of a part with no geometry. I do this for threadlocker call outs.
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Kevin Chandler Feb 2, 2021 12:28 PM
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Correct Answer
Hello,
1. Add the EU configuration outside of the drawing's border and crop its view so only the cord displays.
2. Drag the cropped EU cord into the title block and in its view's properties, set it to be linked to the main BOM.
3. Add a balloon to the cropped EU cord.
4. Add a note linked to the cropped EU cord's view (pointing at the EU cord)
  The note reads "IN LIEU OF " then click the balloon of the US cord.
  As an alternative:
  Place another US assy view outside of the title block and balloon the US cord (view linked to the main BOM)
  Change the balloon to item number only, no border
  The note reads instead "IN LIEU OF ITEM " then click the no-border balloon of the US cord
  This is what this note is doing:
Kevin
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Assembly Drawings, how to show Available options via Configurations?

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