Text along a sweep... possible?

[chris]

Has any figured out how to get excluded or embossed text along a swept path?
I'd like to add my hose text if possible.

[blandb]

Planar linear sweeps are fairly easy, but one that would twist around in 3D space I'm kind of blanking on...

I guess you could do it always bend your part afterwards, but that is not always the easiest to make match a weird sweep path.

[dan_inv09]

I think you might need to use a texture.

Do you need it to be embossed so that it will show up in a drawing view? (or why else?)

[Be aware that a texture might find some wacky ways to mess it up.]

[chris]

@blandb Multiple bends dont work to replace sweeps
@dan_inv09 Textures don't work because there is no UV space in Inventor

Stuff like this is where Inventor falls apart

[johnsonshiue]

Hi Chris,

There isn't a command in Inventor to create the exact emboss geometry you are looking for. However, you may use a combination of Geometry Text, Extrude, Thicken, and Combine to approximate it.

Please take a look at the attached 2026 file.

Many thanks!

[chris]

@johnsonshiue I need it to be parametric and updatable through iLogic, custom parameters and custom iProperties

[johnsonshiue]

Hi Chris,

It might be doable to certain degree. But it will be a hack, as opposed to be a full blown parametric model embossed to the 3D pipe.

Many thanks!

[pkomatlapalli]

Hi @chris ,

Did the info from johnsonshiue blandb dan_inv09  help answer your question?

If it did, it’d be great if you could click the "Accept Solution" button so others can easily find it too.

If you’re still needing more help, feel free to share an update here. The community will be happy to jump in with any next steps to help you get where you need to be.
 

[dan_inv09]

Well, you might not be able to do all of that

[abu-CAD]

Hi Chris! Yes this is possible. The key is using the Geometry-Text feature inside the Emboss sketch to follow the curved path, combined with a custom iProperty and iLogic rule to make it fully parametric and updatable.

I've put together a demo video and the Inventor 2024 part file with the iLogic rule already included is attached below for your reference. Hope it helps! 

Don't forget to accept this as a solution if you are satisfied! 

[blandb]

Yes, that works for just a linear arc, but I believe he is wanting it to also work for a 3D splined option (bends in X, Y, Z)  as well.. I could be wrong though

[chris]

@blandb correct, I'm looking for it to work on a 3D spline

[obulesub]

Hi @chris ,

I wanted to check in and see if you still needed assistance, or if you found a solution to your question already? Let us know if you need further assistance by providing an update or if you have found a solution, please share it with the community so other members who may have the same question could learn from your experience.
 

[obulesub]

Hi @chris ,

It's great to hear you have found a solution, 

Please click on Accept solution or provide the solution.

[chris]

@obulesub I don't remember posting that I found a solution...?

[blandb]

Look at the attached video, would this be something similar to what you are looking at? This is just fixed at 4 characters long, but the concept is there.

[abu-CAD]

Thanks for sharing the video. I'd appreciate if you could share the part file so I can see the exact iLogic implementation and sketch structure. That would help me understand your approach better.

Regardless of the method used, the documented constraint remains: Geometry-Text in the Inventor API only accepts a single line, a single arc, or a single circle as valid geometry input at a time — this is stated in the official Inventor API reference. Splines are not supported by the feature.

From the video, the text appears to be positioned on a single geometry, but I cannot determine from the visual alone whether it addresses continuous spline projection. Would you be able to clarify how your method works, or share the part file? That would help me provide accurate feedback.

[blandb]

As you mentioned, geometry text was not used due to the known limitations. Instead, the text is essentially "faked" into position. That's also why I specified a limit of four characters in the input field.

To create the text placement, I first offset a surface from the tube at the desired text height. The text location itself is driven by a work plane patterned along a 3D path. From there, I created an axis, work plane, and work point to define the placement of the first character. That work plane was then patterned again to generate the remaining character locations, resulting in four total character positions.

A separate sketch was created on each work plane, with the text center-justified and constrained to the projected work point. Each character is therefore controlled independently within its own sketch.

For the solid geometry, each character is extruded bi-directionally as a separate solid body. Initially, I attempted to create all characters as a single solid, but the Split command consistently generated errors. Creating each character as an individual solid resolved the issue and allowed the Split operation to complete successfully. Once all operations were finished, the bodies were combined back into a single solid.

The text itself is driven by parameters. There is one user parameter for the complete input string and separate user parameters for each individual character. An iLogic rule parses the input string, extracts each character, and assigns it to the corresponding parameter used by the sketch text.

Character spacing is controlled by the distance of the secondary work plane pattern, while the overall location of the text along the tube is controlled by the initial work plane pattern that follows the 3D path. This provides independent control over both the text position and the spacing between characters.

All of this could more than likely be controlled via code, but this was just a simple proof of concept. I have since made it to where I can also control the text height as well.

[abu-CAD]

Thanks for the detailed explanation, blandb. That’s solid work—your method places characters at calculated positions, while Geometry-Text handles continuous curve following but only on a single line, single arc, or single circle. Neither solves true continuous spline text projection at the API level.

Both approaches are valuable. Chris, you have three options to consider:

(1) Geometry-Text — native API support for continuous curve following on single lines, arcs, or circles
(2) Blandb’s workaround — discrete character placement with more control on 3D surfaces
(3) Custom development — if continuous spline text projection is critical, either request an enhancement from Autodesk or explore a custom add-in solution with significant development time and investment

Feel free to explore whichever approach works best for your use case. If any of these options helps address your question, please mark it as the solution—it helps other users find answers quickly.

Thanks to all for contributing.