Wildfire 4 drawing options for # of decimals

[jlambert-3]

im searching but these eyes must be missing it.

where is the drawing option for controling how many decimals display upon creation?

i want it to default to 1 place

so instead of creating a dimesion and having it show

318.863

it instead just automatically posts as

318.9

as of right now i have to manually change every dim i create. and for the life of me i cant find this option.

thanks in advance.

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[TomD.inPDX]

It appears to be controlled by the setting in the active model or the model the features are selected from.

So if you set the default_dec_places in the model to 1, subsequent drawing (driven) dimensions will be only 1 digit. Check to make sure they round correctly, though!

[rohit_rajan]

i think there should be an independent option in drawing mode itself to control the display of dimensions.

some times PTC approach does not make sense at all! huh!

[jlambert-3]

somehow i missed your answer and only read Gunter's below. thank you this is what i needed.

[TomD.inPDX]

No problem. Gunter confirmed my suspicions.

The good thing is, you can have the default_dec_places set to a higher number while modeling and only change it to a lesser number for drawings and it will make new drawing (driven) dimensions comply while maintaining already created dimensions in the model with more digits.

As Rohit pointed out, however, it would be nice to have a separate straight forward setting for drawings. The problem is, I want to see that 4th digit quite often when using fractional equivalents. .1875 is 3./16 and if I enter 3/16 in a dialog, I want .1875 to show up, not .188. In some cases, I have actually had Creo (1.0?) put in .188 as a real value with 3 decimal places by entering 3/16 in the dialog! But rarely, if ever, do I put 4 digit numbers on drawings. I have to select multiple driving dimensions and change their properties to 3 or even 2 places. It is good that I am giving each value consideration, but knowing all dimensions will be 3 places by default would reduce my effort by a few dozen mouse clicks.

[gkoch · Accepted solution]

There are only two different numbers of digits that can be controlled:

• The "real" number of digits, specified by the value entered
• The displayed number of digits, shown in model and drawing.

The latter can be set to a default by the option default_dec_places

If you need different number of digits displayed in model and drawing, the only alternate technique is to "abuse" secondary units. It will allow you to specify how many more or fewer digits to show in the drawing.

See for example knowledge base article CS139243 : How to set the different decimal place in drawing and 3D model in Creo Parametric:

http://www.ptc.com/appserver/cs/view/solution.jsp?n=CS139243

[jlambert-3]

"default_dec_places"
im not seeing this option under drawing options. is this a version specific?

i tried the 2nd method... and it does do what i initally want... but i still need control over certain dims to display 2 decimal places in specific situations. (my companies tolerances are controlled by how many decimal places are shown, 1 dec is 1.5mm tol and 2 is .25 tol) also the 2nd method gets rid of trailing zeros. i always need at least 1 decimal trailing zero to be shown (for the tol reason i just explained).

as of now my best method is to filter my selection cursor to "dimension", box select them all.... , then "properties" show 1 dec place. then go back in and change the certain dims with tighter tol to 2 places. problem with that is i gtta actually be done with everything to box select them all. if there is any additional dims created that i missed then i go in to every dims properties after that and change it.

so you can see what i want... i want to create a dim (drawing only) and have it display with 1 dec place.... and then have the ability to change it to 2 in case i need tighter tolerances (which is in the minority amount of instances).

[jlambert-3]

ok...

i got the secondary units method to show how i need it. i start with the default 3 dims displayed (from inside the dim properties). then i use the secondary units of -2 so that it only displays 1 dim.... then for the ones i want to show 2 dims i can manually change in the properties of dec places to 4 (thus -2 showing only 2 places).
problem is im not the only ones dealing with these drawings. i have a feeling this method will confuse alot of people down the road.

[jlambert-3]

alright... im an idiot. def_dec_places is a model option not a drawing option. ok. its working just how i want it to now. thank you.