Autodesk Inventor

[#1]

This following happend frequenty.  

1.  We spend a lot of time creating a drawing with dimensions and leader text.  

2.  The part or assembly changes (feature or components are deleted or replaced)

3.  Dimensions that reference deleted geometry disappear.

From what I can tell, the dimension will turn pink/purple and not disappear ONLY if one of it's attachment points is still valid.  However, if all the attachment points for the dimension or leader text are gone, then the dimension or leader text simply disappears.

Is this standard behavior? 

We spent a lot of time creatin these dimensions and/or leader text and would like to know if there is a problem.  We have had many instances where we though the drawing was done only to find vital info missing.  To make sure this doesn't bite us again we currently have to carefully compare archived revisions of the drawing with the current drawing to make sure everything is there.  This is a waste of time in my opinion.

Anyone have a better way of dealing with this?

[#2]

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michmaju wrote:

This following happend frequenty.  

1.  We spend a lot of time creating a drawing with dimensions and leader text.  

2.  The part or assembly changes (feature or components are deleted or replaced)

3.  Dimensions that reference deleted geometry disappear.

From what I can tell, the dimension will turn pink/purple and not disappear ONLY if one of it's attachment points is still valid.  However, if all the attachment points for the dimension or leader text are gone, then the dimension or leader text simply disappears.

Is this standard behavior?

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yes, this is standard behavior.  Why would you expect a dimension to stay put if the item it was attached to was deleted?  Notes, I could see why they may be desired to leave behind when something is deleted, but not dimensions.

Depending on the situation, something I've done in the past was to locate work points on their own sketch, orientated in such a way that the work points always ended up at the location I would be applying a dimension to in the idw.  That way, the part or feature could be modified and the dims would hold on the idw.

However if the part is outright deleted, that work-around gets deleted also.

[#3 · Accepted solution]

In a drawing file (template, for instance): Document Options > Drawing tab > Preserve Orphaned Annotations

[#4]

I don't think that's standard behavior.

I re-use drawings a lot, replacing / adding / removing parts or assemblies within them, and it's not uncommon for me to find that every single dimension has come unattached both ends.  No valid attachment points remain.  Dimension is still there, though, and just needs to be reattached.

Edit: Sbixler nailed it.  I didn't even know about that option ... learn something new every day. 

[#5]

it used to be standard behavior, until they added that option!