Margins don't show up in the Filter list for a Cylindrical Dimension

[CGAArt]

This is a problem that has plagued me since Nx 6. I am on 7.5 and when you create a margin, you name an entity (mostly I use lines) MARGINX, MARGINY or MARGINZ. The filter in the baseline command give an asterik for a wild card (MARGIN*). I have used this command forever. Jet engines use a lot of Cylindrical dimensions. Here's my problem, when I change the name of the line to MARGINY, it doesn't show up in the baseline list. The box is empty. Does anyone know if naming a margin has changed, what is the new criteria to name a margin if so? This seems to be intermittent and usually never happens on my machine, I have loaded others with a fresh version and it doesn't work there either. Is there a setting for margins?

Thanks for any help!

CGAArt

 

[JohnRBaker]

I'm note sure exactly what your problem is and I was not able to reproduce what you've described. Have you tried to use a simple '*' alone with no additional letters?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
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[CGAArt]

Yes I have John, I have a line with the name of MARGINY in my file. I have tried just the astrik and it gives me lines used in sketches. I've never had this problem before and I have not reloaded Nx. I just opened a new part so I was thinking there was a setting I was unaware of. I uploaded a word doc with some screen dumps pasted to it. Haven't used this upload before so I am not sure where it went. It doesn't seem to be attached.

Your file's link is:

http://files.engineering.com/getfile.aspx?folder=b038e386-b53c-406b-b77e-bc647bc5f65f&file=Doc1.docx

Thanks for the help.

Art

 

[cowski]

It appears that you have an associative line (feature 13) and you have renamed the feature rather than the line object. When selecting the line object, set your selection filter to "curve" or use the quick pick list to make sure you have selected the line object as opposed to the feature.

Quick pick list showing the line feature and the line object (line object is highlighted).

When naming the line object, you will see entries for the name and the feature name. Enter a value for the name, do not change the feature name.

www.nxjournaling.com

 

[CGAArt]

Cowski,That was certainly it. Thanks a lot! Nx 6 still had the old line command that allowed you to click unbounded. They dropped that off of 7.5 and I never noticed that two features show up in the object list. I have the associative feature button off but it still makes the line associative. Its there a way not to create an associative line anymore? Now that I know to look for this it not really an issue but somehow I have been getting lucky and inadvertently naming the line correctly. Man this has bugged me for a long time. I owe you a beer!

Thanks again, Art

 

[cowski]

I have the associative feature button off but it still makes the line associative. Its there a way not to create an associative line anymore?

If the associative option is toggled off, the created line should not show up as a feature in the part navigator. It should be equivalent to creating a line with the old "basic curves" command. If the option is toggled off and you still get an associative line feature, there must be something else going on.

www.nxjournaling.com