I have some problems with sketch groups with NX11: as soon as I group a set of curves in a Rigid Sketch group, I get the message "Sketch contains conflicting constraints". But if I look in the Sketch Relations Browser the status is ok for every constraint.
The same operation (New Sketch Group-Rigid) with the same geometry works without problems in NX10, so I think it may be something related to the new options for sketch groups (Normal, Rigid, Unique, Scalable): I cannot find any documentation about this.
I attach a file .prt with the geometry I want to group and two images, before and after grouping.
Solved! Go to Solution.
Have trouble reproducing your problem. I did notice I get three auto dimensions (two for position and one to fix orientation) and you only have two.
Something strange is going on. Can you post a movie showing how you get this problem?
I think the problem is related with the use of Mirror Curve inside the sketch. If you draw a profile without mirroring curves there is no problem.
I attach a movie of the sketch group made with NX11, withe the "conflicticting constraints" problem at the end (I suppose they are not "real" conflicting constraints, since the Sketch Relation Browser doesn't show any problem). If you do the same thing reproduced in the movie with Nx10 there is no problem.
This is looks like a bug. I advise you to write a PR so we can fix this.
The number of auto dimensions is incorrect and the solver is giving feedback that the sketch is inconsistently constrained. When you make the group active, you can see that the sketch solves correctly.
When the group is inactive you can fix a point and then rotate the group by dragging. After deleting the fix some auto dims should appear. They do not appear.
I can now confirm this is a quality problem. The problem is not related to the mirror curve operation.
The workaround is to save and re-open the part after creating the rigid group. There is nothing seriously wrong with your part. The sketch solver is just confused. A save and reopen of the part cleans the data and removes the problemr. This is why I could not reproduce your problem, you solved it by saving the part.
Close and reopen works only for the first group; if you add another sketch group after reopening the file, the status line, while in the sketch, says "Sketch need 0 constraints", and does not update after adding new dimensions nor is refreshed after saving, closing and reopening the file.
It seems that it only happens with the "Rigid" option though, that's why I would like to better understand the other new options. I cannot find them in the Help doc.
In documentation go to:
Home / CAD / Sketching / Creating and managing sketch feature / Using sketch groups
then on the right there is a topic under learn more.
You can also search for the word "rigid" and filter to CAD and then sketching.
I only find the description for the "Rigid" option, not for the others (Normal, Unique, Scalable); maybe I need to update the Help doc. I have more or less understood them but for instance how do I make a Rigid and Unique group like I did with the previous version? Not so important, but I find the sketch groups very very useful and I am trying to use them at their best ::