Inventor 2012 (sketch) dimension properties

[ahardman]

I'm in sketch mode and my drawing dimensions are all in decimal format.  How do I change that to a fractional format? 

I thought it would be in the styles editor, but when I open that up, I don't see ANY dimension style listed (see picture).  I also tried right clicking the actual dimension to view the properties, but that only lets me change the decimal precision (also attached).  The help file mentioned the "ANNOTATE" tab, but I don't even have that tab on my ribbon so I'm guessing it's unique to autocad?

[JDMather]

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@ahardman wrote:

I'm in sketch mode and my drawing dimensions....

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Drawing environment or part environment?

In sketch you can just enter the fractions and Inventor will convert to decimal.
If you edit a dimension the underlying fraction will still be there.

[ahardman]

Its the drawing (sketch) environment and im trying to get my dimensions to display in fractional rather than decimal format.

[JDMather]

You can enter fractions as the sketch dimension - but when you accept they will be converted to decimal.
And even if it still showed as fractional they will hide when you exit sketch mode.
You could Retrieve Dimensions - but since they will be decimal that doesn't help.

Therefore - I would simply redimension using a fractional or architectural dimension style.

[s.mutschler]

When I want to force a fraction to appear in a dimension within a part sketch, I explicitly enter the units suffix after the number OR enter a multi-factor number (containing a space).  For example, all the following will preserve the fraction display:

1 7/8

7/8 in

7/8"

0 7/8

[mflayler2]

In a part sketch...edit your dimension and then click the arrow just in front of the approval of the dimension (this is the same place you grab Named Parameters).  You can choose Fractional from this list for that dimension.

[s.mutschler]

I have noticed that the formatting options do not appear in the dimension-edit popup menu (but the rest of the menu items do) if the dimension is entered as a formula and/or if it contains named parameters.   In these cases, the result always displays as a decimal value in the sketch.

Is this intended behavior?

[mouthpear]

Thank you this helped me out a lot.    Now I ask you if you know how to make the driven dimensions show the same?

[mouthpear]

Thank you this helped me out a lot.    Now I ask you if you know how to make the driven dimensions show the same?  In drawing mode and in part sketch mode?

[mflayler2]

Not easy to do, but if you can toggle off the driven dimension (look in the Format Panel in the Ribbon next to centerline).  You can then change it to Fractional and then change it back to Driven.  You may have to make another dimension driven so you can toggle it off on the other dimension though.  To me, this is not worth it for simple showing a value in another format.

[mouthpear]

I understand what you mean about not worth the time it take to do it.  Is there any way to do this as a default.  I work with wood and most of the time it is plain stock. As in 2x4s and 2x8s. And most of the time cuts are in 1/16 of an inch. I would like it to reflect that as I am designing. I would like it to display it as fractional so that I don't have to keep cross referencing so much. I am not that smart when it come to conversion.

Thanks for your help so far it has already my work easier.