Annotation

[ISUdesigner]

In the past I was a I-DEAS user and was able to attach a text description to a part in the modeler that was separate from drafting. Does UG have a tool that lets me attach a text description to a part in modeling, which will allow me to distinguish it from other similiar parts?

Thanks,

Chad Richardson
DARcorporation

 

[SolidNX]

Hi Chad,

When adding a component, there is an option to define a component name. If you added three blocks, you could name them block1, block2 & block3. You can also name them later using MB3 > Properties.

Then you could add this as a column in the Assembly Navigator or turn on Name Diplay (under Preferences > Visualization).

Another way entirely is to add attributes (also under MB3 > Properties). These can be added as columns in the ANT too or in a Parts List for BOM purposes.

Cheers,
-Mike

 

[ISUdesigner]

Mike,

Is there a way to put the component name with a leader in the model view? I am putting solid spheres that represent center of gravity locations for aircraft components. These can get cluttered and I would like to put the name with a leader attached to the sphere.

Thanks,

Chad

 

[SolidNX]

Hi Chad,

Probably the easiest method is turning on Name Display, but alas, no leaders. They can be moved around though.

Next best might be adding labels with <Wcomponent_name@attribute_title>. However, if you have many of the same component with different names, this could be as tedious as labeling them individually.

Probably the best method would be adding ID symbol labels and using Parts List to generate a table of what each component is. After adding the labels, their values will update automatically and in NX2 I believe the whole process is automated (including adding the labels).

Cheers,
-Mike

 

[kamaraj]

there is a method of displaying text in 3d model by naming it in attribute .after naming go to visualisation perference and toggle on the name display

 

[vanishingpoint]

If you want to attach text to a part...

1) pick application + drafting

2) pick Drawing + Display Drawing (make it unchecked). You should now be in what looks like modeling, but is actually drafting.

3) Orient the WCS so that X is pointing in the direction you want the text to go. Y direction up for text up, Z out the direction you plan to view the text. Note the text will always be in the x-y plane. For example if you want to put a label on the face of a part make the face the x-y plane by moving the WCS.

4) Add the leader, label, annotation or dimension to part.

5) switch back to modeling and you should see the text.

If you want the text to display in a next higher assembly, you ***MUST*** add it to a reference set. It will not display in an NHA if &quot;entire part&quot; is the reference set.

Ken