How to convert annotation units?

[Anonymous]

 Hello. I changed the units in my model from inches to MM but when I create annotations they are still in inches and I cant figure out how to convert them to mm. If anyone knows how to do it I would appreciate. 

-Thanks

[Anonymous]

Annotations in a drawing?
You need to use an English template if you want inches.

[jhackney1972]

Normally the drawing template is configured to be inches or millimeters (or some other units).  When you select the template and place your part on it and annotate it the dimensions follow the dimensional style assigned to the template.  If you have a drawing already started using an inch template, you can change the style to another style standard by using the Tools -> Document Settings command and under "Standard" select another active standard from the list.  This will not change existing dimensions placed with the original style of the template, you will have to select them, right click and change the style associated to each.  You can select as many as you like at one time.

[johnsonshiue · Accepted solution]

Hi! Is it in 2D drawing or 3D model? If it is former, you need to change your annotation standard (go to Manage -> Style and Standard Editor). If it is latter, go to Tools -> Document Setting -> Standard -> Annotation -> Active Standard. You may want to make the change in the template so you don't have to change it next time when you create a new file.

Many thanks!

[Anonymous]

It was in the 3D model this was the solution I was looking for. Thank you so much. 

[mdavis22569]

I have a few issues where with mine ..

I changed it over to Metric and some if it didn't change, they stayed English dim's ...

[johnsonshiue]

Hi Mike,

The behavior does not make sense to me. Could you share an example?

Many thanks!

[mdavis22569]

I'll email you ... I did make a PR 

[johnsonshiue]

Hi Mike,

I think I know where the problem is. The unit is indeed sort of mixed. For general dimensions, the unit is dictated by Active Standard. For hole notes, the unit is by the part unit (Doc Setting -> Units). For spec holes, the unit is from the thread table.

The 3DA behaviors are consistent with drawing annotation though. It is a bit confusing because you can have DIN 3DA standard, while part unit is set to inches. But, it is always better to keep everything in sync. I don’t think this is a bug.

Many thanks!

Johnson

[mdavis22569]

Yeah, @ChrisMitchell01 set me straight too ..

I agree it should all be sync, but I can see some (IE me) get confused at first....   But I now have clarification so if I have anyone asking in the future ...

Thanks, guys as always! 

Mike

[robin.engel]

So this seems to work fine for switching between millimeters and various imperial options, but I cannot find any templates that allow me to display the annotations in meters or centimeters. Do I have to create new templates for that?

[jhackney1972]

I will not be able to answer your question effectively at this time.  I am traveling and donot have access to a computer.  I will possibly get back to one by Wednesday,   You are appending your question to a old post.  Create a new one with your question and you will probably get a quick answer and not have to wait on me.  Sorry I could not help right away.

[johnsonshiue]

Hi Robin,

Yes, it is true you may need to create custom standards. Inventor is a mechanical design and manufacturing tool, driven by common standards (ANSI, ISO, DIN, JIS, GB, and so on). These mechanical design standards are either in mm or inch. "Meter" and "Centimeter" don't seem common in mechanical design.

Could you tell me what exactly you are trying to model?

Many thanks!