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Losing Constraints in Sketch

kdirth
18-Opal

Losing Constraints in Sketch

We recently installed 7.0.8.0 and I am having some difficulty in constraining a sketch.

 

I want to keep the squiggle below at a constant thickness.  As I constrain the center points of the inner arcs to the outer arcs, some of the coincident constraints that I just created disappear.  When I recreate them, others will disappear.  Anyone else experiencing this this issue or have an idea of what is going on?

kdirth_0-1653678522450.png

 


There is always more to learn in Creo.
1 ACCEPTED SOLUTION

Accepted Solutions

I have been able to complete the sketch.  The problem was most likely that I was attempting to over constrain the sketch.  I started with making the arcs equal and the lines parallel, then i started making the arcs coincident.  The solver did not like the added coincident constraints and deleted them as I added more. 

 

The real issue here is that Resolve Sketch dialog did not pop up to show me the constraints in conflict so that I could choose one to delete.  Which brings up another issue with Resolve Sketch.  Many times it does not show all of the constraints that are creating the conflict and I end up selecting Undo, deleting the unwanted constraint, and recreating the constraint I was trying to create.


There is always more to learn in Creo.

View solution in original post

4 REPLIES 4
pausob
17-Peridot
(To:kdirth)

Maybe one squiggle too many?

Not seeing your issue here in a Creo 4 sketch, but it took me quite a bit of "wrangling" to get to this state:

pausob_1-1653690862355.png

tbraxton
19-Tanzanite
(To:kdirth)

There are situations where the sketcher intent manager is not able to apply the intended constraints. To fix this I have found that adding construction geometry or simplifying the sketch will resolve the issue. In Creo 7.07.0, I was able to mimic your geometry broken down into two sketches and it seems to behave.

 

tbraxton_0-1653823106505.png

 

 

 

I have been able to complete the sketch.  The problem was most likely that I was attempting to over constrain the sketch.  I started with making the arcs equal and the lines parallel, then i started making the arcs coincident.  The solver did not like the added coincident constraints and deleted them as I added more. 

 

The real issue here is that Resolve Sketch dialog did not pop up to show me the constraints in conflict so that I could choose one to delete.  Which brings up another issue with Resolve Sketch.  Many times it does not show all of the constraints that are creating the conflict and I end up selecting Undo, deleting the unwanted constraint, and recreating the constraint I was trying to create.


There is always more to learn in Creo.
pausob
17-Peridot
(To:kdirth)

One that bugs my OCD is that it accepts certain "over constraints"  For example, if you have a horizontal centerline and a horizontal line segment, and then you create a coincident constraint between the two entities, it will accept a sketch that has 3 constraints instead of only 2 that are necessary.

(Yet if you have a horizontal line and try to constrain its endpoints to be horizontal, it will complain)

 

Another one that I realized as I was working out your squiggle example, is that if you place a point on a line, and then make it a midpoint, the system keeps both constraints - but only the midpoint constraint is necessary...

 

I wish it would flag these "over constraints" and force user to resolve them so as reduce the clutter.

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