How to shorten a dimension line for a very long radius center point

[mistralunizion7]

Hi, I try to find how to split a dimension line in two with that kind of "Z" shape between both ends, for a far center point for a very big radius that would otherwise be outside the drawing in Inventor if the size of the part is at regular viewing dimension. I did found out how to shorten the radius value line itself, by using the right click/option/shorten. But for the location of it's center point I have no clue.

Please see attached screenshots.

Thanks for helping.

[James_Willo]

Right click your dimension and under options select 'jogged'

[SBix26]

This is a problem without a good workaround solution.  Here is the best I have to offer:

1. In the model (part file) create a very tiny feature at the center of the radius, such as a .005 inch diameter cylinder
2. In the drawing create a broken view, bringing the center point onto the drawing sheet.
3. Place dimensions to the center point as you normally would; they will be correct and will "break" the dimension line to show that they are not to scale

In your case, this may still not be an adequate workaround because your center is off the sheet in both directions; I believe you can only create one break for each view.

Update: I just tried this in Inventor 2023, and found that I could break the view in both directions, bringing the center onto the sheet:

This workaround does maintain associativity with the model, and allows for adequate communication of the design intent; but it should not be necessary.  A functional Displaced Center drawing tool should have been created a couple of decades ago!

What version of Inventor are you using?

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Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

[IgorMir]

The question is about jogging Linear Dimension - not the Radius one.

Cheers,

Igor.

[johnsonshiue]

Hi Folks,

I think this article summarizes the status quo nicely. Please take a look.

https://knowledge.autodesk.com/support/inventor/troubleshooting/caas/sfdcarticles/sfdcarticles/Is-it... 


[Edited to remove article with broken link]

At the moment, the closest alternative is to use Linear Foreshortened dimension.

Many thanks!

[mistralunizion7]

Thanks for the info and helping out. Sorry for the late answer.

I am not sure about the purpose of the tiny element (little cylinder) in the part drawing... ? What is it used for? Maybe a video tutorial could help me if ever you had time but I would totally understand if you don't.

When I use the broken view in the drawing, it want me to place the broken view onto the selected view but this cuts it in two and I don't want that.

Sorry if I am not understanding your tips, I am still learning a lot in Inventor.

Thanks,

Jonathan

[Frederick_Law]

Move dimension to outside of circle.  Unless you need to dimension center point.

[SBix26 · Accepted solution]

You can't break a view outside the bounds of the model itself.  The tiny invisible feature at the center of the radius increases the bounds of the model to include the center.  This allows the view to be broken between the center and the radius, thus bringing the center onto the drawing sheet.  Now your dimensions to the radius center point will show accurately, with squiggles in the dimension lines indicating that they are not to scale.

Look carefully at the image I included in message #3 above.

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Sam B

Inventor Pro 2023.1 | Windows 10 Home 21H2

[mistralunizion7]

Ok now I understand. Thanks so much!

[mistralunizion7]

I am using Inventor 2020 (forgot to answer your question).