Displayed Objects

[lab2010]

I have just switched to version 8.5 of NX and have a pretty basic question. I was previously using version 6, and when I would edit a sketch, I would only see objects that were above it in the part navigator list. When I open a sketch in 8.5, it still shows me all the objects below, which makes it more cluttered. Other than manually hiding all the objects below it in the tree, is there an option to change this behavior when a sketch is opened?

For example, if my part navigator has:
Sketch 1
Revolve 2
Sketch 3
Extrude 4

In version 6, when I opened sketch 1, I would not see anything but the lines in sketch 1. If I open sketch 3, I would see the lines and feature of sketch 1 and revolve 2, but I would not see the features of extrude 4. I would like to have that behavior in 8.5.

Thanks in advance

 

[MEichWey]

Hi,

you have to switch a preference in NX:

Under "Preference - Modeling" you have a tab "Edit". In the third line you can switch the edit-mode for double-click with sketches to "edit with rollback". Default is only "Edit".
Then you will have the same behavior as in NX6.

Michael

 

[lab2010]

Thanks for the answer. I now have another issue which is most likely caused by some preference I cannot find.

In NX 6, I could use any line from a previous sketch for a constraint. For example from above, I could use the lines in sketch 1 to constrain my lines in sketch 3. It will now only let me select lines in the current sketch.

I had a completed assembly in version 6 with no issues, but one of my parts now says "Warning: Missing positioning reference. Missing horizontal direction reference". Within the part, I created a sweep feature with the first couple sketches. After creating the feature, I have a horizontal line offset from the feature with a vertical distance constraint. That reference changed color to red. I tried to just delete the vertical constraint and create a new one, but I cannot select anything on the feature or in the sketches that created it to make my constraint. No idea why the ability to use previous sketches within the part would be turned off by default...

 

[cowski]

Check the "selection scope" filter. For sketches in NX 8.5, it defaults to 'within sketch only', but you can change it to broaden the scope.

www.nxjournaling.com

 

[lab2010]

I don't think that is it. My selection filter says "No Selection filter" and it looks in "Entire assembly".

 

[lab2010]

I was wrong. The selection filter and scope I mentioned above were for general selection. When I actually went into the constraint dialog box, the scope was active sketch as opposed to within work part only

Thanks