Drafting-Extra Zeros

[mechanicalman1]

Firstly, I apologise as I am sure this will have been covered before. But the search function is down at the moment.

I am in the drafting workbench; here is what I would like to do,

I want extra zeros to be displayed as defult. If a dimension is modeled as 3.41, then it will display 3.41. But if a dimension is 3, it will disply 3. I would like it to dislay 3.0, or even 3.00. I have admin access to Catia, and can edit my drafting standerds. But I cant find the option to activate this function.

 

[ferdo]

Hi,

First

http://www.eng-tips.com/faqs.cfm?fid=1179

You can right click on dimension, Properties-Value-Format-Precision

or

You can right click on dimension, Properties-More-Standards-More-ISO-DistanceLenghtDimension-MainValue-Precision

or by CATScript.

Regards
Fernando

 

[ferdo]

Or even a better answer here

http://www.catiav5forum.de/thread.php?threadid=955&hilight=Dimension+Precision

or

http://www.catiav5forum.de/thread.php?threadid=1626&hilight=Dimension+Precision

Regards
Fernando

 

[jackk]

jamesphillips,

Fernando's threads tell you how to customize the drafting standard if you have administrative privileges.

If you don't have those privileges, an easy way to get those zeros displayed is go to FILE + PAGE SETUP and change the standard from ISO to ANSI.

 

[looslib]

Are you modeling your parts in metric or english units?
Trailing zero's are not allowed on metric dimensions, if your drawings comply with ASME Y14.5m.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
Sr IS Technologist
L-3 Communications

 

[mechanicalman1]

Thanks for all the suggestions.

None of them work! I am beginning to think I have an instillation problem. I had real issues getting into admin mode for the first time; even the Catia support engineer could not work it out. It turned out it got sorted with a re-boot!

Right, I am defiantly in administration mode, I have tried these;

You can right click on dimension, Properties-Value-Format-Precision;

and it makes no difference, like wise;

You can right click on dimension, Properties-More-Standards-More-ISO-DistanceLenghtDimension-MainValue-Precision

I have also tried changing the sheet format to ANSI, both in admin mode, and in normal mode. Neither work.

 

[catiajim]

You are probably looking more for a parameter that effects the display of trailing zeros. I'm not sure it's supported in ISO, but it is in ANSI. Look to the online documentation for Drafting Administration.

 

[zrxoddie]

http://www.catiacommunity.com/feature_full.php?cpfeatureid=10445

 

[Albigger]

And if you are trying to change an existing drawing from ISO to ANSI you must hit the "update" button next to the box or it won't update the drawing to the new standard.

-- Jay

 

[adminhost]

Changing to ANSI will not work. ANSI is defaulted to NUM.DIMM as the dimension properties. To have the trailing zeros, the Dimension Properties has to be in NUM.DINC. If you are in Admin Mode, go to the Tools > Standards > Drafting / ANSI > Styles > Length/Distance > Default > Value Display Format > Main Value > Name - Change to NUM.DINC. Do the same for angle, radius, diameter if desired.