topic Re: Changing the default tolerance settings for annotating dimensions in Inventor Forum

Changing the default tolerance settings for annotating dimensions

Anonymous — Fri, 03 Aug 2018 19:05:31 GMT

I'm annotating dimensions on my solid while it's still an IPT file and I can't find where to change the tolerance for all dimensions to 4 place decimal instead of 2 place. I want 4 place tolerance to be default for all models without having to change it every time I create a new solid. Please help!

Re: Changing the default tolerance settings for annotating dimensions

TheCADWhisperer — Fri, 03 Aug 2018 19:11:00 GMT

Tools>Document Settings>Units tab for the number of decimal places and Default Tolerance tab for bilateral tolerances.

then

Save Copy As> Save as Template

Re: Changing the default tolerance settings for annotating dimensions

Anonymous — Fri, 03 Aug 2018 19:10:44 GMT

Tools, Document Settings, Units, Linear Dim Display Precision

Re: Changing the default tolerance settings for annotating dimensions

Anonymous — Fri, 03 Aug 2018 19:38:54 GMT

It is set to 3.123 but still annotates 2 place

Re: Changing the default tolerance settings for annotating dimensions

Anonymous — Fri, 03 Aug 2018 19:55:18 GMT

Tried this too, still annotating as 2 place. I even restarted Inventor to see if it would take and it didn't.

Re: Changing the default tolerance settings for annotating dimensions

Anonymous — Fri, 03 Aug 2018 20:25:58 GMT

I suspect this does not work the way you want it to?

Re: Changing the default tolerance settings for annotating dimensions

Anonymous — Fri, 03 Aug 2018 21:10:23 GMT

I think mine is broken, lol

Screencast will be displayed here after you click Post.

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Re: Changing the default tolerance settings for annotating dimensions

SBix26 — Sat, 04 Aug 2018 18:53:22 GMT

Sounds to me as if @Anonymous is using model annotations, not referring to sketch dimensions. In 2019, at least, I don't see any way to alter the default decimal places of the MBD dimensions; the only choices I see are the Annotation Standards in Document Settings > Standard tab: ASME, ASME (mm), DIN, ISO. I don't know where these standards are stored, nor how a user can alter these or create their own.

Sam B
Inventor Pro 2019.1 | Windows 7 SP1
LinkedIn

Re: Changing the default tolerance settings for annotating dimensions

peter.hamas — Sun, 05 Aug 2018 15:10:21 GMT

Hello,

Unfortunately there isn't currently an easy way to edit 3DA styles from modelling environment, but there are 2 workarounds that might help:

1. Editing 3DA styles from drawing Style Editor (please see this video). We need to make sure Style Library is set to Read-Write in the project settings. Then we open drawing Styles Editor and set the filter to All Styles, to show also the styles in the Styles Library. We select the Default (ISO) - 3DA dimension style and we change the Linear Precision to e.g. 8 decimal points. We need to save the edited style, and then save the style to the style library (please make a copy of the Design Data folder before making any changes). After that we can open the part document with active ISO standard, and place a simple linear dimension. Notice the dimension still shows 3 decimal points instead of 8. This is because we still need to sync local document styles with the Styles Library. We need to use Update style command in the part's Manage tab and after this is done, either existing or newly created dimensions will have 8 decimal point precision.

2. Editing the library files manually. To find the location of the Design Data folder please see your Application Options File settings. Once in the folder you could open the dimension.xml file and edit the Default (ISO) - 3DA style there. In this case we are searching for LinearPrecision attribute under the UnitVals element. But this method is not advised.

Hope I could be of some help,

Kind Regards, ~peter

Re: Changing the default tolerance settings for annotating dimensions

Anonymous — Thu, 09 Aug 2018 17:18:19 GMT

Thank You very much!