I started this.... here's what I have so far.
Then, using Frank's technique...
From here it gets a bit tricky. However, I was able to use a wrapped sketch to do some crazy cuts before so this starts to look possible.
Having the text from the line above anchor the lines below is a bit sketchy though. I think I could do this much nicer if I had a line between the text that could anchor the tops and bottoms of all the lines. Trying to anchor the text using tidbits of other chunks of text is possible but won't look very pretty.
Although... if you can get this to work, you could print this on a 3D printer and turn it into a nice candle holder if you put a tea light inside of it. Hmmm... maybe I just figured this out. If you write a love letter to your girlfriend in text around a cylinder... then 3D print it... you can make a nice, unique, and relatively cheap gift.
You're busted David! 
Thanks!
-Brian
The trick is cutting out the letters from the cylinder with the basic package. I ended up having to extrude a sketch by projecting each character, or a small group of characters and subtracting it from the cylinder. Of course, this works well, because the wrapping corrected the form of the letters. In my case, I ended up cutting out the letters, but if you have multiple surfaced to cut, then you can reverse the material removal. The beauty of this is that you can then thicken the text to get appropriate edge-angles.
Have you priced 3D printing lately? Flowers are still cheaper
The angle of the text, how it clears or intersects, can be controlled with a little reference geometry and maybe a relation or two in the original sketch. All you need is the circumference and text height to know what angle is required to get the desired effect.
One tip; in the text extrusions, if the projected sketch bysects the "edge" of the cylinder, it creates 2 line segments that are collinear, but the length of one of the lines may create errors. Deleting the two segments and replacing it with one will solve this. I could not even get Absolute Accuracy to allow this. You will see what I mean if you run into this.
tip two: before you put in too much effort, know what you're going to write and be happy with the overall initial wrap. Making changes is much like a hand written letter... you pretty much have to start over if you want it nice and clean.
I'll take this to the next level. It's a fun thing to see just what limitations there are between surfaces and solids in Creo. Remember my reference is the base Creo parametric platform.
Remember I am using a surface cylinder so I do not need to be concerned with surface normals for the extrusions. Thickening happens later. The text used was the TTF_FONT which I knew to be troublesome due to the extensive curves. In fact, it reversed some features from the 3D_FONT I used the 1st time. Quite troublesome for "parametric" technology.
The initial cut was quite stubborn. You cannot do a solid extrude and subtract if from a surface. You have to know that you must make it a surface extrude, and you can then "remove" the material in the extrude command. The material removal direction too is critical, obviously. This action failed several times before an edit finally made it "work". It has since been stable.
The "N" did not want to extrude and posted warnings about Accuracy. Nothing I adjusted in accuracy would fix it so I ended up making a tangent plane to the cylinder pretty much centered on the "N". This finally worked.
The last bit of troubling capability was to try to remove the last remaining piece of the original cylinder. Extrude would not let me cut away the entire section. Odd! There was enough of the original cylinder with the remaining text to expect this to work. But alas, no dice.
The thicken was probably the easiest part of this. The entire surface feature was still a single feature, so it was one click, pick a side, and thickness. Done.
Last was extruding the remnant. This was a no-fuss cut now that it was solid.
I have attached the original Creo 2.0 file for your decompiling pleasure.
Anybody know how to angle the letters in Creo 2.0??? I can do it in S/W, but can't figure it out in PTC.
Thanks for the help.
D
If you are asking about a sketched text in modeling, you can manage this easily. To create the text, you draw a line to represent the height in the sketch. You can dimension and constrain this line any way you want. Furthermore, you can also have text wrap around a curve in text. You can also use a number of fonts to do this. Here is an example of what you can do with Creo with minimal effort:
This is text extruded into a sphere. This is the same font as the original real world part.
I've done text in Solidworks and it didn't seem any easier to me.
What were you really after and what method did you end up using?
Well, what i wanted is ABC rotated about a line to get the font to extrude. In SW i just drew a line and rotated it to line them up. In Creo I had to draw multiple individual lines to place the text on (see pics). Any way, that portion is done.
What I need now is to add the p/n. Can anyone walk me thru the torodial blend? I'm having trouble figuring out the steps. (see pics of how it was done in SW, wrap function). I did a wrap sketch in Creo, but don't know to get an extrude out of the sketch.
Thanks
D
