how to make dual dimensions in Inventor
hi everyone!
I am new to Autodesk Inventor. I want to make a basic 3D model and I want to use both In and mm so that it shows in both styles on my sketch and also later on my drawing. Is it possible to do that like in SolidWorks?
Accepted answer
Inventor cannot display dual dimension on the model sketches. It can do it on the drawing only. I'll walk you through the process as best I can:
1. Click "Styles editor" on Styles and Standards under the "Manage" tab.
2. Click the plus sign next to "Dimension" on the left column
3. Select a style similar to what you desire to start from.
4. Click "New" at the top
5. Give the style a name that you will understand in the future. Hit "OK".
6. Click the "alternate Units" tab near the top.
7. In the drop down list near the bottom, select a dual dimension style such as "xx/xx".
8. Select "mm" in the alternate units drop down if it isn't already selected.
9. Adjust your precision, leading, and trailing zeros as desired. (You will be able to override the precision later on.)
10. Click "Save" at the top.
11. Click the plus sign next to "standard" on the left to expand the standards if they are not already expanded.
12. Select the appropriate Standard. The current one is highlighted. Select that one if it is the standard you wish to use the new dimension style.
13. Click the "available styles" tab at the top.
14. Click "dimension"
15. Make sure the new dimension style you just saved has a check mark beside it.
16. Click "Save and Close" at the bottom.
When creating a dimension you should now be able to choose this new dimension style on the "Format" tab.
Once the dimension is created you can double click on the new dimension to override some values like the number of decimal places.
If you wish for this new dimension style to apply to all new drawings then do the following:
1. Click "Save" on "Styles and Standards" on the "Manage" tab.
2. Make sure both the new Dimension type and Standard type that you just created are set to "Yes" under "Save to Library".
3. Click "OK".
4. This new dimension style will automatically be available in new drawings that you create.
To use this new style in existing drawings first open an existing drawing.
1. Select "Update" styles and standards on the "Manage" tab.
2. Make sure "Update is set to "Yes" on the new Standard you previously saved.
3. Click "OK".
You must do this for each existing drawing in which you want to use the new style.
--------------------
Inventor can kind of show dual dimensions in the model sketches. If you actually enter sketch dimensions in a specific unit like "1 in" or "25 mm" then you can force display of these individual units.
1. Right click in an open area of the display beside the model.
2. Select "Dimension display"
3. Select "Expression"
It will then display the exact expression you entered but it will not display dual units for each and every dimension.
1 Other answer
I did it by using one of the presets and i just need to make some minor changes such as the unit string, leading and trailing zeros. The only thing I think that updated the dimension to dual dimension is to choose the "dual format" style that I ignored it. This is what shows the dual dimensions.
Last thing is I need to see if the two dims can be centered because right now it's left justified although the style I picked looks centered from the drop-down menu. other than that, thanks so much for your help!
