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You might want to set the units to 4 decimal places in the Documents Settings as well. This will at least stop some of the rounding that may take place as well.
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
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Delta Tau Chi ΔΤΧ
@Anonymous wrote:...If I type in 13-13/16"...it displays 12.932...if I type 13 13/16"... it displays 165 3/4 (no unit designation ' or")...
Not that it's much of a solution, but I got it to display 13 13/16 when I typed in 13 13/16.
I get that you wouldn't want to go back and change a bunch of part dimensions so that they display the way you desire but I would imagine that this would be a decent route moving forward.
Out of curiosity, your goal appears to be dimension appearance in the part file environment. Does your construction shop/yard get their dimensions from the part files? Not that it makes much of a difference to your goal but it would be odd to me if the dimensions you show in the drawing environment aren't the ones you really need to format.
I still don't get why you care what the dimension in the model looks like? You're not giving the model to the guys in the field to check dimensions against. Why does it really matter if you enter 14.25 in your model dimension or 1'-2 1/4"? Quite frankly, I find it easier to enter decimal inches than to enter feet and fractional inches. The drawings are where the dimension style matters, because that's what your man in the field will be comparing against with his tape measure, and those dimensions can be very easily set to feet and fractional inches in the styles menu.
Rusty
@Anonymous wrote:...if it can't do something as basic as dimension in fractional inches I am not wasting another minute on it.
Slow your roll man. 
There is a solution here. We do similar functions to what you want as well. Our work-flow is set up to allow our inputs in our part files to match any documentation provided by others so that it makes checking things easier (i.e. if we get a dimension from an architect that is 3'-1 1/2" we enter it EXACTLY like that, it displays like that, if we get one that is 32 3/4" we enter it like that, it displays like that).
As suggested before, set up your templates to use the proper units and modeling dimension display and you're golden but there are some things to note:
1.) Set up your part template settings to be just like this:
2.) Inventor is going to see the hyphen as a mathematical operator unless it is proceeded by a foot symbol. 3-1 1/2 (with these settings) to IV is three inches MINUS 1 1/2" and it will display 3 in - 1 1/2" and your dimension will be 1 1/2". However, if you input the dimension as 3'-1 1/2", IV will see it as three feet one and one half inches. You can skip the hyphen all together and type 3'1 1/2" and IV will see it as three foot one and one half inches and then add the hyphen for you.
3.) The only value formatting I have not been able to get IV to recognize is entering whole feet with just an apostrophe (e.g. 3.5') but it will accept feet if it is annotated with ft (e.g. 3.5 ft).
4.) Your drawings are going to display however you set them up to display in your Styles. If you want your drawings to display all the different formats (3'-1 1/2", 37 1/2", 37.5, etc.) that gets a little trickier but it's possible. If that's what you want, get back to me and we can go through it but it seems unlikely. In short, you need a style for each dimension type and you'll have to change the ones you want different from your default style after they are placed.
Here's a sketch where I put in all of the different value formatting in the same file and IV sees them all correctly and displays them the way I want:
I hope this gets you where you want to go and if you'll permit me I'll leave you with this small bit of advice.... The users on this forum are trying to help and we see a ton of new IV users (usually from other software) jump on here who are all to eager to hit the panic button and scream "Inventor SUCKS"!
Give us (and the software) a chance and we'll try to help you get to where you need.
Good Luck!
P.S. I'm pretty sure you are stuck with all the dimensions you previously entered because you'll have to go back and do those ones again. But, it sounds like you guys are just getting started with IV, and you just barely asked the question, so it can't be that many already can it?
Why would you send 20 fab drawings out to the field to verify the final product? Throw a couple views of the assembly on a sheet, put the dimensions on it that you want checked - or even just select the view and pick "get model dimensions" - and send that to the guys in the field. Not only will that give you the formatting you want, it'll also have the advantage of looking more professional, and a lot cleaner as well. Screen caps don't generally come out nearly as clean and easy to read as vector lines like you'd get in a PDF generated from an IDW.
Rusty
Is this in your drawing environment?
Did you create and save a new style? To creat & save a new dimention style see here http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-501BE8A0-3FBF-414F-988A-F835F80FFD6B
Are you selecting/setting that style every time you dimension? If your not selecting the desired standard simply click one on the wrong dimension/s, this will show the standard that was used, then while the dim is still selected go to the standards drop down and select the desired standard that dim will the updated to match.
Changing form the default style/format
Change to the correct style/format
Finally the correct/wanted dim style
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