Only by selecting a Drawing Standard that has these options set. Look thru the existing Drawing Standards to see if any meet your need. If not, you will need to create your own standard.
The Drafting Standards are contained within a .xml file in the dassault systems folder. It is accessed through Tools>Standards>category (drafting). Chances are you'll need admin right to add or change.
You don't need Admin Rights to run CATIA in Admin Mode - you just need to have write access to the CATCollectionStandard and CATReferenceSettingPath directories. Search the forums for more information on Admin Mode, as it has been discussed many times.
jrochte (sorry for not giving a complete answer earlier)
To change an existing dimension style, select it first. Then look at the top of screen for something that looks like NUM.DINCH or NUM.DMM. These are the dimension syles (graphisms) and you can change them by using the down triangle to choose a different style.
On the right of the style is the precision. It's probably set to something like 0.01 Again you can choose a different precision setting from the list, or you can click the panel and type in your own value. '8' will round off your inch dimensions to the nearest 1/8" and '16 will round them off to the nearest 1/16"
You can probably find the same options if you go to the properties of the dimensions.
Follow Bob and Jim's advise to set up your own standard, so your dimensions will be added with the correct graphism.
I have searched over the help files. The help files say two different things one says that you can edit standards inside the program when you load catia with the command line option of -admin. The other says that the Standard menu is only a view. Personally I have never been able to edit the standards inside of catia by following the instructions. So I lean to the later.
I have had success by using Peter's XML editor (freeware) and editing the standards outside of the program. It takes finding the value in the viewer inside Catia and then using a little logic to find it in the XML file. It is not necessary to restart Catia after you change a standard file outside of the program. All that is required is to save the changes then go and update the standard.
I would be very careful editing the xml file outside of CATIA (or inside it for that matter). Make backups before you start as they corrupt very easily, and debugging a 5000+ line of xml is not my idea of fun.
