modeling text in nx

[ebie]

Does anyone know how to parametricly model text in nx and control it through the annotation editor rather than using the CGM method? Is there and GRIP program or user definded feature availible rather than creating my own?

 

[mjcole]

What version of NX? ALso do you want the text to be used to create features or just as a cosmetic feature for display on a surface.

The best way to keep the text visible is by placing it on the Drawing of the part using Annotation editor to display PArt attributes using Relationships -> Part Attribute or typing <W@PARAM_NAME> this way you can change the part attribute and have it change the drawing text. In order to keep the text associated I recomend using Associative origin and picking the point on your geometry to place the text relative to so if you move your view or the surface of place ment moves you wont have to update location of all the text as you would if you chose to place it relative to view.

You can place the text in the model by choosing to not display drawing sheet then orienting your model and WCS to place text. Text placed like this won't be visible on the drawing so you'd have to do twice the work you can decide to do this or not.

Michael

 

[Xwheelguy]

Any version below NX3, you have about 3 options for modeling text in 3D:

1. This is basically the CGM route, but works for any 2D text that are lines, arcs, splines. Import 2D geometry into modeling from dxf, cgm, iges, etc.; position the text & extrude. The extrusions are associative to the curves, so there is some intelligence to this method.

2. Sketch the curves in sketcher, then use projections, extrusions or whatever you need. The idea here is to use the sketches to control the shapes of the letters versus just importing and replacing curves, as would have to be done for method 1 above.

3. Purchase Wiedemann Engineering's True Type UG. This does nothing relative to NX's Annotation fonts. It only works with True Type fonts as far as I know. More info here:

http://www.w-eng.de

That's it. Those are your ONLY options up to NX3. Starting in NX3, there is a Text feature, but it only creates and positions the curves to be used for extrusions. It's NOT associative, therefore NOT editable. It's a one time shot, then re-creation. This function is supposed to mature in NX4 to become a fully associative feature.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[Vikingbro]

Just to add to Tim's information, concerning the True Type UG program, it DOES recognise NX's annotation fonts, however, the VAST majority of them are made up if lines of no width (ex.: an "I" is made up of three lines, a horizontal line on the top and bottom, and a vertical line connecting the two.)

True Type fonts tend to be "shapes" of the letters, (ex.: in the above example, a True Type "I" would have 6 horizontal lines and 6 vertical lines.)

If you were to extrude the NX font, you would end up with sheet solids, where the True Type extrusions would be solid bodies.

One of the beauties of the True Type UG program is that you can create your own fonts to use in the program.

I hope that this helps!



Chris Cooper
Cleveland Golf / Never Compromise

http://www.clevelandgolf.com

http://www.nevercompromise.com

 

[ebie]

Thanks for all the help. My company is still on NX2 and will not upgrade for at least 6-9 months. I knew about the CGM method as well as sketching the text using curves to extrude the model. The TrueTextUG looks like it will be a perfect fit for my application. Thank you all for the help.


-Mike