NX 9: Looking for your best practice for applying text to create a product label

[BOPdesigner]

So you have designed your new product at a high level of detail. Why stop short of adding a product label right? So here are the issues that I have ran into (considering planer labels only, no wrapping around a curved product surface):

Option 1: Apply text to your model in Modeling (Insert -> Curve -> Text).
Problem: The text is hollow. It is assumed that you are going to Emboss or Extrude those text curves. So what do you do? Extrude the text a small amount or use the curves to Divide Face. That works ok but the model tends to become very heavy quickly. For example, A simple case where my blank label has 6 sides (a very thin cube) and I put some text on one side and then divide face and recolor the letters. Now the model has 20 faces. File sizes bloats up from a few hunderd KB to over a hundred MB (I have a PR opened on this issue). It becomes very cumbersome to manage and make changes using this method.
Option 2: Apply modeling text as in option one but then switch to Drafting and hide the drawing sheet. Now Crosshatch or Area fill the hollow lettering. Add the text curves and crosshatching to the Model reference set so that it appears downstream in your assembly and drawing.
Problem: This is a tedious process as you typically have to select only a few text curves at a time to crosshatch or it blows up. Then downstream in your drawing file the text shows through bodies that should be hiding it. So you have to hide the label in those views but if you have a partially hidden label, then you have to do view dependent edits to selectively trim the text curves etc so that it appears proper.
Option 3: Leave label design to Adobe Illustrator etc and then just take an image file (BMP, JPG etc.) of the label and apply it do your NX label face as a Decal (View -> Visualization -> Decal).
Problem: The decal only displays when you are using Studio rendering views and it doesn't show up in drawings.
Option 4: New for NX 9. Apply the text to the label as a drawing note now that you can finally use Windows system fonts in drafting annotations. This works good and is fairly quick to apply. No need to pick a face and then use a guide edge and you are not limited to applying one line of text at a time like with modeling text. Or import you label dwg file from AutoCAD. Thanks to the new AutoCAD import/export wizard the fonts and everything map across very cleanly compared to the past . I thought I had it all figured out here but then...
Problem: When you go do drafting the text is of course still drawing note. You can't use view dependent edit to selectively delete individual letters or partial text curves because it isn't curves, it is a note.

So does anybody have any better practices for this than what I have listed? Why can't NX hide the notes/curves in a drawing view when they are behind other solids or sheet bodies?

 

[csbk]

I cant respond to all your issues for now. I just want to post somthing. Maybe someone els can chime in
Here are some ideas:
If you are etching on a product, use Modern font works for a single line etch. Our experience is many tool shop cant use the 3D etch data well (maybe because of restricted to software). Maybe, just provide a 3D location and csys, then provide correlating text and csys in the drawing so it will be easier to export.
We put in 2D on a layer then reposition (parametrically you can use instance geometry, csys to csys) and project to the surface. The tool shop will have 2D and 3D in the same file.

For a decal Label. Instead of displaying the Label Text, just show label size in your BOM assembly, then show the label information on the drawing. You can use a user define symbol in your library.

You can add attributes to the label component at the assembly level

You can set up a label image generator with NX or PPT... then use the decal operator in NX. You can only show what it looks like using studio render option


CSBK

 

[Toost]

A few tips .
If you like to use the Modeling text, the simplest way of filling these is to extrude with distance 0. ( from 0 to 0)
will create sheet bodies inside all the characters in one step/ one feature. ( The text must be flat)

If the text is "on face" and curved, you can use the Subdivide Face , When selecting the text use the selection rule "Feature curves" , it will reduce the selection to minimum possible. ( Some characters needs to divided a second time)

Note that you can extrude the curves face of the characters if that is of interest. ( Quicker than Emboss) I think i need to select each character.

If you prefer to use Curves as the label, they can be hidden in the drafting views, but you must ask for it
Edit-Settings(?) the Drafting view where they should be hidden line processed, Hidden line - "Include model curves" = on.

Regards,
Tomas