David's link will give you options.
This is one method to consider:
- Create the nomenclature in a sketch.
- Create a Fill feature by projecting the geometry of the note sketch.
Otherwise, yes, you can extrude the original sketch to create a solid.
I prefer the solid option; but be aware of accuracy issues. I also prefer to make the "silkscreen" a separate part assembled in the next level.
You can project or wrap a datum curve. Complex logo's are going to be tough in any feature if you're trying to have a bunch of entities in a sketch. You might have to make several sketches. I made these labels in Pro/E, and made some curved ones as well, I just can't find the images. You can also float a surface .002 or so off a solid surface for silkscreening. 
I'd imaging that if you can project or wrap a cosmetic feature onto your contoured surface, you can do it with a curve. Not sure if the hatch thing will work on a projected or wrapped curve, somehow I don't think you can.
A pic of a finished part showing what you're trying to do would work wonders. 
.....I invented the "Woodward swoosh"!
The die-casting was kinda fun. Got to design a high-voltage (20 kv) enclosure and drive the design of the electronics packaging in tandem. Got to extrude the logo and ground symbol in the casting (turned out sweet!) and do the labels too. Sometimes you get to have a little fun! 
Datum curves are actually quite limited:
- Through points
- From Equation -or-
- from Cross Section
However, Cosmetic Curves are simply sketches or filled sketches (area).
The only way to have complex curve data that is not fully constrained in a sketch is to import a DXF or DWG file into a part. This remains an "import feature" and does not require full dimensional detail as a sketch does.
The more practical way to manage complex detail curves is through a symbol. Symbols act more like drawings, meaning that curves drawn are not parametric. Symbols are annotation so they can be added to a model but in my opinion, are difficult to manage in models. But if it is a logo that will be used in many different ways, it is a good way to manage it as an option when appropriate. The only limitation to symbols is that you cannot use them as underlays for projected curves into sketches. (I may have gone way over people's heads by now, but I wanted to post all options).
When I created a PTC logo, I left the definition with weak dimensions in the sketch.
You have to be careful in how you use it, but it has served well with appropriate attention.
If you wish to clearly define your requirements, we might be able to come up with a good method. Again, as with everything with PTC, there are -many- ways to do something. There is no -best- or -right- way.
you won't like this in Creo either...
I don't see a "curve from sketch" but there is a hidden "curve from file"
Thanks all for the answers.
Below is shown the printed drawing in to the aluminum foil. Drawing is made from a part where sketch is extruded to the label base. Geometry line thickness is too wide but not enough to fill all of the center areas. Result is blurry and messy.
When I make an annotation note in drawing, the result would be accurate enough for me (see another photo), but then the texts will not follow the model and the placement handling is not so flexible as it is in part level when feature is sketched. Also drawing notes are not shown in assembly.
I copy paste these labels all the time and modify them so easy handling speed is needed. Maybe Creo is not the right platform to do these things but I have been happy that I can modify the panel cut outs and these labels at the same time and see the result in assembly.
Propably filling the text is not even a solution. I would need accurate printable text somehow in to the part´s surface.
There are a few tricks in how to achieve this but this is a comparison of the 3D model (cosmetic fill of 3D text); CAD view in a drawing; output PDF; which can be achieved. Not even close to perfect in my book, but certainly does what I tell it to do. Again, I don't know how well this would go directly to a printer or even if a pen table can be used for direct printing. Others will help you with that.
I´m using pdf export from drawing. View is "shaded with edges" and pdf output is 600dpi. Using pen table or not doesn´t seem to make the difference to the result in pdf exporting. I changed model´s absolute accuracy to the finest as possible. I don´t get why pdf looks like it is heavily compressed.
This what I got. I almost nailed it
.
How do you create pdf?
Frank, I think you will find that datum curves have been replaced with cosmetic features. They have added intent curves in the datum region to designate cosmetic curves (and other edges or curves) as designated datum "intent" references.
I also do not see a hatch in part mode. They now have the "fill" cosmetic. I know what you are talking about because I remember using it in the past. That would be an excellent solution to this issue sinced you can have curves (hatch) print "solid" where the shaded view is not satisfactory in quality.
David Schenken wrote:
Perhaps what PTC does with PDF is junk, though they do so little it's hard to see how they can ruin it.**
Fair enough
David, if you look closely at PDF prints that have both a shaded images and a wireframe image overlayed directly, you will find that the output of the shaded image matching is really poor along the much crisper wireframe. It is simply not a very good output even though the views are explicitly aligned.
This is where I 1st noticed it:
The shaded views are seriously tessellated along non-linear curves.
Darn, Frank! Of course, as always, you have a genius insight.
Marko; extrude the artwork as a solid and define a section through the artwork (stay with me...)
In the drawing, display the view in a drawing as a section.
Edit the section (model tab; highlight the hatch; properties) and change the hatch to "fill".
Print monochrome with a very thin pen thickness in the pentable, and whallah! Really crisp edges.
You might still consider the scaling option since that can only help matters in the print function.
Also, change this setting in your adobe reader:
(uncheck this option!)
Take a look at the attached PDF...
Scale: 1:1, Line weight .025"; font (Swiss condenced) .22 high; circles .625" OD
In order to get this to extrude, I had to change the part accuracy to .0005"
