I am having a problem in Siemens NX 9.0. I was using sketcher and wanted to add a datum csys on a point of the sketch. When this happend, I was no longer able to snap to any point. I can still snap lines in parallel and in tangency, but it will not snap to a point. I have checked the inferred constraints dialouge and everything is selected, it is enabled. Also, the curve ribbon bar and half of the home ribbon bar have grayed out. I am wondering why these have disappeared and how can I fix it? This setting will not change even from part to part. I have tried restarting the software and reseting the toolbars, but nothing has changed. I have attached two pictures for demos.
Thank you for your help.
Was the point that you're trying to select created in the sketch you're currently editing? If it was created later on in the feature history you won't be able to select it. If it was created in an earlier sketch or exists as a point feature (or a non feature based point) then you would be able to select it.
I suspect that the commands on your ribbon are greyed out because you're editing a sketch created earlier on in the part history. I.e, you have features created after the sketch that is currently being edited. If your sketch was the last feature that you created in your part history, then you should find that you have all of the command available on the ribbon.
Hope that helps.
Snapping to 'points' is NOT controlled by the Constraint settings but rather by what options have been enabled in the Snap Point tool on the selection bar.
Make sure your points are not hidden. Using Show Hide show all of your points. Also try turning you model to static wireframe. I find it easier to select this point when in wireframe mode.
HOpe this helps!
When I was in sketcher, I could select the point. I was in sketcher when I created the Datum CSys on that point. I have noticed this problem before, but I had forgotten about it. I believe it is a glitch in the software that I have to be more careful about. Even after moving the datum around in the tree, it doesn't help. A datum usually has it's own set point anyways, i.e. if you edit a sketch, a datum CSys will not move with that change to stay at that point on the sketch. (unless it is attached)
One must create the datum CSys outside of sketcher or NX will throw a hissy fit. You can still reference the point outside of sketcher.
You cannot 'add' a Datum CSYS feature to a sketch. Sketches are a feature onto themselves and as such cannot contain other features. If you attempt to add a Datum CSYS feature, at least using the 'Dynamic' type, while in an 'active' sketch, the system will automatically 'Finish' the sketch and the Datum CSYS will be created as a non-dependent objects. However, if you use any of the other types, such as 'Inferred', you will be able to associate the Datum CSYS to elements of the sketch such as points and lines, however it will still be its own feature with a timestamp AFTER the sketch.