How to change driven dimension units

[j.pavlicek]

Hello, I have document (read only) where I'm drawing some sketch and want some driven dimensions to be shown in different units than document default. How to do it?

[nedeljko.sovljanski]

Hi,

You can use isolate function, here is help doc.

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2014...

(almost at the end of article)

Yuo can see, do is driven parameter in mm. isoparam is value without units. This iso param is used then in d1 but, pay attention on 2mm * isoparam. You must specified new dimensions when multiply unitless parameter.

[j.pavlicek]

@nedeljko.sovljanski  Thanks, this is good workaround. But what to do when I want to show this value in a sketch (as dimension)?

[Gabriel_Watson]

I don't think you have any way to modify the unit on a driven dimension, as it sits greyed out as Reference, under Parameters:

We can suggest changing styles on a driven dimension for the developer team to maybe implement this (post into the Ideastation?)... perhaps into the API so this can be changed at least via iLogic:
https://forums.autodesk.com/t5/inventor-ilogic-api-vba-forum/edit-driven-dimension/td-p/7744762

A good workaround, however, is to use 3D annotations to convey your driven dimensions. You can alter the 3D annotation styles (by opening a drawing file and saving changes to the styles library, then updating your 3D model with those changes):

[nedeljko.sovljanski]

What value you want to display? Isoparam or d0? Can you create that sketck and notify what dimension you have and what dimension you want to display?

[j.pavlicek]

Short story long:

I have a model created in imperial units, and want to create a modification for connecting to a metric system part. There is multiple parameters in inches which I can change (want to keep it in round numbers and inches as units) and want to see (online) what dependent (driven) dimension value is in mm to choose suitable counterpart.

All of this is happening in sketch environment. I also tried to create.

[nedeljko.sovljanski]

Unfortunately that is problem, but if you decide to put in in Ideas forum I will vote for it.

[johnsonshiue]

Hi! This is an interesting request. All model parameters and reference parameters follow document unit. There isn't a way to change it selectively. User parameters unit can be changed easily. However, there isn't a way to show dual units.

Many thanks!

[SBix26]

If you can live with the number being reported via a custom iProperty, then all you need to do is check the Export Parameter box for each reference parameter, then right click on each one and choose Custom Property Format...  Set your units and precision and click OK; there they are in Custom iProperties with names the same as the parameters.  They aren't easily displayed on the model, but would be accessible through a drawing, or with a very small amount of iLogic programming.

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Sam B

Inventor Pro 2022.2.1 | Windows 10 Home 21H2