Text after Value

[Anonymous]

I was wondering if I could have some text show up after a dimension. Without editing the dimension I would like to add some text when I'm creating the hole feature. For example, when I create a 1" hole can I add text after the 1 and it shows up on the drawing when I pull the dimension.

[johnsonshiue]

Hi! Do you want to create Hole Notes? You can use Hole/Thread Note command in Annotate tab. You can also configure what additional information the default Hole Notes should include (Style and Standard Editor -> Dimension -> select a dimension style -> Notes and Leader tab).

Many thanks!

[jtylerbc]

Some examples of the types of text you're talking about would help, but I am also leaning toward what @johnsonshiue said.  The short answer is no, there is no way to enter text in the model and have it show up in the drawing when you dimension the hole.  I believe this is more a job for the Hole Note style in the drawing, as @johnsonshiue mentioned.  However, this solution only really applies if the text is a commonly repeated thing.

Unless, of course, you're using Inventor 2018 and there is something in the new MBD features that would allow it.  I haven't spent any time in 2018 yet, so I don't know if that's possible, but it's the only thing I can think of that might do something close to what you are asking for.

[blair]

Nothing new in IV2018 like that. Also if you are using the "Hole" function, there is nothing to add in the text. The "Hole" feature is different than the "Extrude" feature where you can create a circular sketch, dimension it and then Extrude.

By definition within Inventor, the second method is not a hole and this feature won't show up when using items such as the "Hole Table" functionality.

[Tom_Sturtevant]

I agree that using Hole Notes is likely the best solution.

That being said, there is a way to do something like this with Inventor 2018 MBD… After you create a 3D dimension there is a “Text..” command that allows you to add text to the dimension display.  Then use “Retrieve Model Annotations…” in the drawing to bring in the dimension.

[blair]

If you use the "Hole" feature, additional data referencing the Hole such as countersink and bevel angle are retrieved.

Nothing as I posted in IV2018 for "custom" information such as you are showing in your post directly without additional steps.  I've added a picture of the data already available by using the "Hole" feature.

One should stay away from "Fixed" text when using a parametric based CAD system. If you change model data, you want this information to update any downstream information such as your drawings.

[jtylerbc · Accepted solution]

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@Tom_Sturtevant wrote:

That being said, there is a way to do something like this with Inventor 2018 MBD… After you create a 3D dimension there is a “Text..” command that allows you to add text to the dimension display.  Then use “Retrieve Model Annotations…” in the drawing to bring in the dimension.

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That's exactly the sort of thing I was wondering about in my earlier post, as I haven't had a chance to use 2018 and look into the MBD features yet.  I don't know if this would really be practical for @Anonymous or not, since it requires the extra step of creating the MBD Hole Note and retrieving it, instead of just typing it in the drawing Hole Note.  I'm not sure that really saves any work, but it is the closest thing in the program to what was originally asked for.

To me, it depends somewhat on the intended use.  If one user is doing the model and drawing, then it seems to me like it would be less work to just type the added note at the drawing level.  If the extra note is being used to hand off additional information to a different person to create the final drawing, then the MBD method may make sense.