Sketch on Face - "some external references are missing"

Colle

Maybe i'm missing something obvious but i'm having an issue where i create one sketch then extrude a part from that sketch.. then sketch on one of its faces to create a second part .. so far all is good.! Now if i go back to the first sketch and change the spacing of of some attachment points. on confirming these changes this of course makes Sketch 2 go red...

When i edit sketch 2 i get the warning "some external references are missing" but the sketch is black and there are about a half dozen references between the two sketches is there no way to tell which reference is broken.? all i have been able to do is delete parts of sketch 2 until it goes black then redraw what i had to delete.. this then causes the issue to ripple to the next (sketch 3) that was drawn on a face or linked to Sketch 2.... and so on...

Is there a way to get a list of what external references are missing and simply resolve the those references.? or how should i be structuring things so that when i make a change on an early sketch it doesn't break the references on later sketches.?

Thanks you for your time,

Colle

jakeramsley

While in the sketch with the errant references, click the "Show constraints" checkbox which will show all of the constraints in the sketch.  The failed/errored constraints will come in as red.  Any missing reference will say "Dangling" if hovering over them.  From here, you can select the constraint and hit the delete key to remove it.

For example, I projected a bunch of faces that I then removed upstream.  This means the references will go missing.

1. Open the errant sketch and notice it is red with missing references.


2. Click the "Show constraints" checkbox.  All constraints will appear on the screen.  The red ones are constraints that the solver has failed to solve.  In this case, the constraints are dangling, referencing geometry that doesn't exist at this point in time.


3. Select an errored constraint in the graphics area and when it is highlighted and hit delete.  This will delete the constraint.  Do this for all errored constraints.

Colle

Thank you so much for the very clear answer Jake. I real appreciate it.!!

Isoworks

 

paul_bunnell

Rather that deleting a dangling reference is it possible to replace the missing reference with sketch geometry that does exist?  (I fear that the answer is 'no,' but I know PTC Creo has very good capabilities for identifying and fixing broken references.  Now that PTC owns OnShape hopefully that will be one of the improvements they make.)

NeilCooke

No, Onshape doesn't have a "Reroute" feature (one of the most powerful features in Creo and one of my favourites, though often misunderstood), or a "Sketch Replace" feature.

ayman_el_refaie

If they can only re-create the powerful collaboration features of Onshape (Atlas) with the incredible power and tight data structures of the Granite kernel.  I have used Creo for 30 years and also UG, NX, Solidworks, Inventor and a little Catia. Creo is clearly the absolute winner when it comes to repairing references when major changes have changed... and then it does not crash like the other CAD tools when doing these repairs. 

outstanding

Made a votable Improvement Request. Please chime in if you find this is still needed.