I have an ordered sketch that had a perpetual include line. Now the include relation was lost and I want to repair without losing many downstream relation to the line that was origionally included.
How do I go back in repair what was once included?
afaik, you can not really redo an include... as include will giv eyou an new element and as you state you need to keep what you have bcz of downsteam effect...
IF your included entity is basic in geometry I suggest just constraing using the relationship tools...
Colinear, connect, etc.
for complex geometry ro curves... I dotn knwo of an easy way to do this and some times you need to bite the bullet, delete and recreate... i've been there many a times myself...
I have done that before. Included the new line then added a co-liniar relation to the old line I had origionally included.
I'm filing an IR or ER on this one. My provider is helping me file some IR/ER's. I hope to have a spreadsheet with my 30+ submitted issues soon.
This is a constant headache for me when trimming an assembly full of sheet metal parts, where included geometry is used liberally.
Wherever possible, change your downstream process to be more robust, so that losing that line or recreating it does not affect your part. This is unavoidable in some situations, yes, but the more you reduce the housekeeping aspect, the more painless it is to make fast edits.
LOL Change my downstream process.
In almost every sheet metal part I have, the very first step is to include planes to create the first sketch of the first assembly driven part.
The include command is the basis of almost everything I do. This is what I call the perametric box method.
The only way to make my workflow more stable to to move to sync, I figure another 40 hours of testing and re-tooling my processes is needed before I can start to do that.
While working with a siemans sheet metal diveloper on some ER, they sugested I stay compleatly in ordered because of my workflow. I would if it was stable and repairable, but it's not.
You don't have to re-include.
While in the sketch/profile go to Tools tab>Edge Locale>Peers.
With that button on you can create geometric relationships to peer part edges.
As Matt said it may not be practical if you have a complex profile.
You want your profiles simple anyway.
The Include I want to repair is from a plane. No geometry exists yet, as the include is the first step.
In your case, I'd recommend the "Collinear" relationship be used instead of the include anyway.
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Eye opener for me. I didnt realize I could establish a relation from a sketch to a plane without using perpetual include in ordered.
This was exatly what I was looking for. Now I can copy a part and re-establish relation in ordered sheet metal assembly driven parts. I had no way to get that done before. I have modled the same part about 100 time because of this. Now I can just copy, rename and re-insert a part that I use all the time (The parts size is driven by each assembly model)
In the future, you can "repair" an include so that downstream geometry is not affected.
to do this, you must re-include the feature, but make the line a construction line. then you can force the old line colinear to it. This also works for holes that have lost or broken includes. Re-include the hole and force the old hole concentric.