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Breaking external references still refers back to original assembly

Question asked by Alan Knapper on Jul 1, 2019
Latest reply on Jul 2, 2019 by Richard Gergely

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I ran into this a few years ago, and here it is, back in 2019.

The assembly that shows at the top of the dialog is the assembly that these operations were broken from. There should no longer be any reference back to that assembly. However, if I try to edit this component, where I would be adding an external reference to the NEW assembly, it circles back to the original assembly, which no longer exists, and that it should no longer refer to, because all the references are broken.

When I try to add a new reference, the message I get says the part is locked, because of the reference to the old assembly. As you can see, there is no opportunity to unlock anything here.

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Adam Holmes Jul 1, 2019 5:25 PM
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Hi,

You need to open the part up which has these references and edit the sketches and go to Command Manager > SKetch > Display/Delete Relations.

Then select External from the drop down and delete all of them:

Then re add via the smart Dims tool.
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- Tom Gagnon @ Adam Holmes on Jul 2, 2019 11:21 AM
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  Adam Holmes wrote:
  
  Hi,
  
  You need to open the part up which has these references and edit the sketches and go to Command Manager > SKetch > Display/Delete Relations.
  
  Then select External from the drop down and delete all of them:
  
  Then re add via the smart Dims tool.
  Yes, this.
  
  I'll add that you will also need to reassign the Sketch Plane(s), as I can see at least one within your external references screen capture at the top of its list. When I need to do this, I usually end up creating a new reference Plane within the component for the sketch to use, where it may have been upon the face of another component in the previous assembly. If the plane is orthogonal to primary planes, I usually accomplish this with a measurement, copy value, select primary plane, create reference Plane, paste dimension value.
  
  If and only if the reference planes are orthogonal to primary, then you can also consider using internal primary planes instead of any other planes or faces for sketches, and then controlling the feature's start condition as other than from sketch plane. This, however, does not remove the future need to reassign it when reused, because here the reference only moved from the sketch plane to the feature definition.
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Jeremiah Feist Jul 1, 2019 5:33 PM
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unfortunately, "break" is not the same as "remove"
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- Alan Knapper @ Jeremiah Feist on Jul 2, 2019 9:58 AM
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  Maybe not, but it has worked that way in the past.
  
  And what is the use of having the "break" option if it doesn't REALLY do anything?
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  - Jeremiah Feist @ Alan Knapper on Jul 2, 2019 10:08 AM
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    I have NEVER seen break remove the external references. and I never said there was a good use for the break option
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    - Alan Knapper @ Jeremiah Feist on Jul 2, 2019 11:19 AM
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      Trust me, it has worked that way before. It worked for me that way in SW2018. It's pointless otherwise. The process above works, but holy crap, what a tedious method, especially if you're trying to work with parts having more than a handful of external references. Exporting and working with dumb solids is an option, but you don't always want to lose all that history.
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      - Jeremiah Feist @ Alan Knapper on Jul 2, 2019 11:29 AM
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        are you sure you did not have this option turned on?
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        Richard Gergely @ Jeremiah Feist on Jul 2, 2019 11:46 AM
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        Jeremy Feist wrote:
        
        are you sure you did not have this option turned on?
        If he does have that option turned on he would be able to add new reference which at the second he can't.
        
        This may well be the best option at the second ticking the box and allowing the function. The assembly has had all the external references broken - so no warning lights. So OK that is fine.
        Where the problem begins is that adding new external references are locked due to the shadow of the broken external references.
        
        Ticking 'allow multiple contexts for parts when editing assembly' would then allow the OP to do what he wants to.
        
        Advisable after you have done the modifications un-tick the box to revert back to normal.
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        Alan Knapper @ Richard Gergely on Jul 2, 2019 11:54 AM
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        It's a possibility.
        
        I went in and checked my settings, and the multiple contexts was unchecked. If it was checked in other releases, I can't recall, but I do know I don't change my settings much, after 22 years. Such things do get modified when new releases get loaded, though, even if you don't change them yourself.
        
        I still don't know what "break" is for, if it still refers to the original assembly...
        
        I think that may have done the trick. It's usually one little thing like that.
        
        Thank you for the help, and thank you, everyone else for the alternate methods. It's always good to have more than one option for getting around.
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        Richard Gergely @ Alan Knapper on Jul 2, 2019 1:55 PM
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        Well break all will stop any updates or changes from the original external references but there still is an imprint that the assembly was associated with some original assembly in some way. But they won't change anything anymore.
        
        You just need to be careful when ticking the 'allow multiple contexts' box that you don't end up with references all over the place or some kind of horrible circle regen problem.
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Breaking external references still refers back to original assembly

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