Assembly designer annotations on drawing 1

[Azrael]

Strange red X over the annotions in drawing.

Scenario: Open assembly and add "annotations with leader", create drawing and add 3D view, pick view from spec tree in assembly.

The view with annotations as set in assembly will appear but every annoation will have a red X over it. The red X is ordinary text and can be removed but it annoying.

Any suggestions how to get rid of the red X???
Any ideas??

 

[catiajim]

V4 or V5? This sounds like the infamous "Dead Bugs" of V4. In that case, you have a Project File error. Have your Sys Admin import the file back into your environment.

 

[Azrael]

No, it´s actually V5R14SP4

 

[catiajim]

And the annotations are red x? I've only seen a Red X in V5 on an entire view - not just on the text.

Question: are these annotations on the Drawing? Or in 3-D? I'm not very familiar with the 3D Annotation, so perhaps someone else can chime in?

 

[Archangelz]

Azrael,

I have just a few ideas you might want to try. First, try going to the view's Properies and check the 3D Wireframe and Is always visible options under the View tab. This displays the space geometry in the view. Second, uncheck Enable occlusion culling in either the view's Properties or globally by going to Tools | Options | Mechanical Design | Drafting | View tab. This option can be unchecked unless CGRs are being used in the views.

Archangel

 

[Azrael]

catiajim: I use annotation in assembly designer to make annotations with leader in 3D and then I get them on drawing with insert 3D view. The result is that I get the annotation on the drawing as I want but I also get an additional red X over the annotation. This red X is ordinary text position linked to my annoation

Archangelz: There is no problem with the visualization, I see what I want and more, those red X over each annotation

 

[Archangelz]

Azrael,

This is a direct quote from the Dassault documentation entitled Creating a View from 3D (found under the Generative Drafting topic. It describes the same problem you have for a Datum B that has a red X overlaid on top of it. It is my suggestion that you read this topic and take from it what you will ...

"You can notice that one of the extracted annotations (datum B) bears a red cross mark, which indicates that the leader cannot be extracted linked to the geometry. This is because the 3D annotation leader is linked to 3D geometry which is not visible in the 2D view (i.e. hidden geometry).

Such a red cross mark will be used for any annotation or dimension with a leader linked to hidden geometry (i.e. 3D geometry which is not visible in a 2D view). You can either change the properties of the view from 3D (Edit -> Properties) to display hidden lines, or transfer the marked annotations to a 3D view where the associated geometry will be visible when extracted."

Archangel

 

[Azrael]

A star for you Archangel

Now I know why, but I don´t see a way to get around it. I´m using the ABF module and the weld id feature on drafting stink, due to when I move them around and place them, they will jump back on original position next to the weld when updating. This weld point symbol in 3D isn´t an element so I guess I will always get the red X. So they only way looks like to see if there is something in a setting file that can be turned of.