Parametric Editable Embossed Text?

[NA_11302913]

I'm modeling an object that I want to add embossed/debossed text onto, in a manner similar to what's illustrated here.

I want to be able to make the text easily editable, because it will serve as a label providing identifying information on the different permutations of this object.

If I try to go back and edit the text in the original sketch, it breaks the offset command later in the feature tree, because the specific curves that were projected in order to define the sketched region to offset no longer exist.

In the offset command, is there a way to tell Creo to project whatever closed curves exist in the original sketch, such that when the sketch is edited to include new text, the offset feature will be updated to reflect the new regions present in the sketch it's projecting from?

Apologies if any of this is weirdly phrased or if this is an obvious question, I'm a beginner in Creo.

Using Ver. 10.0.3.0

[kdirth]

Unfortunately Offset>Expand>Sketched Region does not support text.

I am assuming the surface is not planer, I would suggest creating an offset surface then extrude up to the part surface and surface and set Side 2 to extrude up to the offset surface.  

[tbraxton · Accepted solution]

AFAIK this is not possible. You are not able to create text (using the sketcher text function) in an internal section of a feature (i.e. extrude or offset). To create the text, you must first create a sketch and then reference this text in the feature to make the offset.

The use of intent curves could in theory enable this, but Creo does not permit the inclusion of more than 1 chain or loop from an intent curve. You will get this error when attempting to use an intent curve for the text geometry.

Intent curve can only contain one chain or loop to be used as a sketcher reference.

An intent curve will update as the text is modified in the external text, but you are not able to reference this in sketch mode such that it is inclusive of all curves in the reference.

[kdirth]

Here are a couple of ways to get what is shown in the video and allow for changes.

Copy the surface.

Extrude a solid of the text up to the surface.

Copy the outer surfaces of the text, using intent selection.

Trim the original surface copy by the text surface copy.

Select the outer surfaces of the text, by intent, and use remove.

Thicken trimmed surface.

or

Copy surface.

Extrude text as solid.

Copy outer surfaces of text using intent selection.

Use copy of original surface to Solidify remove material to remove text solid.

Trim original surface copy by text surface copy.

Thicken trimmed surface.

Hide or remove text surfaces.

[aputman]

Depending on the shape of the surface where the label will be affixed, you can use the spinal bend feature.  Extrude the text onto the surface of the label while it’s flat and use a curve to define the final shape.  If the surface is always round or always flat, you can create parameters and use flexibility to drive the appearance of the label along with the dimensions of the spinal curve.  If the surface is irregular (like the example below), you’ll have to do something different to define each unique shape. 

[Dale_Rosema]

Check out this thread:

https://community.ptc.com/t5/3D-Part-Assembly-Design/How-to-Extrude-Wrapped-Text/m-p/260291

or

https://community.ptc.com/t5/3D-Part-Assembly-Design/How-would-you-a-cylinder-out-of-text-characters/m-p/115882

[tbraxton]

A tip for selecting text when doing this type of feature is the method to select the text with a single pick. This is an example of projecting the external sketch of the text for an offset surface feature (the internal sketch) with a single selection of a sketch. Set the selection filter to sketch (lower right corner) and then you just select manually one segment in the sketched text and Creo will include all curves in the text for projection. This also make rerouting the offset feature easier if one has to update the text string in the external sketch.