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catia standards

catia standards

catia standards

could someone help me How can I create my own standards in catia drafting.....i tried Tools/Standarts but i cannot change any value...... is there any other way to create my own standarts.?
I'm using catia v5r9

please help me

RE: catia standards


You can change the Standards and create your own standards for that you have to copy a standard file (eg Ansi) and rename it as whatever standard you are going to create. there in that file you have to change the values of some parameters and you can customise the standards. But there are some limitations. only some values you can change. Also the details of parameters are available in Help if you have

The path of Standard file is

dir where catia is installed/intel_a/reffiles/Drafting/.....
the standard files you can open in Wordpad or notepad and you can change the parameters. Make sure that you are not changing the original standards. keep your own standard in the same directory and when you will start the drafting the standard you have created will appear in the list of standars

if any help is required just search in the help for Standards there you can get all the information.


RE: catia standards

ok.....thanks but in v5r9 are this files obsolete and replaced by XML standart files install\intel_a\resources\standard\drafting. And I haven't got help and I don't know how to change this files...

RE: catia standards


regarding the help search for "Managing Standards" and you may find some help. Because in V5r7 help files its available. i could do some changes through that only.

RE: catia standards


Yes V5R9 is the first Rx to manage standards using XML files. As I work very short time with R9 i migth not be of greqt help but amitkulk is right : look on the online help.

First have a look on the environement to be sure of the path for Standards files, then copy your xml file into xml.save and edit your xml file to make change.
restart CATIA.
It worked for me.
I made change for CATPart and CATDrawing... Changing Colors for Solid, surfaces, setting parameters for CATDrawing..


RE: catia standards

Another tip...

Run CATIA as CATIA admin to save the change you make in the option/standard...

to run CATIA as ADMIN, the best is to set a new environement and create your ADMIN icon...

Look into the online Help about Environement, and then set-up your Standard..

I had problems changing path into my new R9 ENV.. i used a text editor to set the right path..


RE: catia standards

To create an admin icon for Catia V5Rx, make a copy of the icon to start Catia. Open the properties of the copy and add after the text ...CNEXT.exe" the option -admin
In the environment file, you have to add paths to CATReferenceSetttingPath and CATCollectionStandard.

After that it's time to launch Catia with the new icon (please, remember to rename it...) and make your changes to Tools/Standards
One problem. If you're to change the ISO standard, you aren't able to get it ISO compliant. It's a V4 thing...

Good luck.

RE: catia standards


The XML files can be edited by tools/standards even if you didn't set the CATCollectionStandard !

Stan Garret

RE: catia standards

The .xml files can also be opened in MS Word, just use the plain text option.

A further question:
Having created my own standard, there are still greyed out boxes when I try to modify the properties of dimensions.  Is there anyway to make these active (without being in admin mode)?

RE: catia standards

A question for anyone in a previous post “ogabriel” posted this.

“In the environment file, you have to add paths to CATReferenceSetttingPath and CATCollectionStandard.”

Where do I do this? Is this a file or menu option in either case where can where can I find it?

Thank You in advance

RE: catia standards


have a look on


Have fun,



RE: catia standards

Or view Properties (NOT Alt-Enter...) for the V5 icon. The start command gives the path and the environment name for the Catia session started by that icon.
Example. My startup line in Properties looks like this:
"E:\Program Files\Dassault Systemes\V5R8\intel_a\code\bin\CNEXT.exe"  -env CATIA.V5R8.B08 -direnv "C:\Documents and Settings\All Users\Application Data\DassaultSystemes\CATEnv" -object empty

First is the location of the executable. Then it's the environment name after -env. The environment file name is CATIA.V5R8.B08.txt, located in the directory given by the path after -direnv. The option "-object empty" starts Catia without loading an empty Product.

I hope that will clarify everything

Best regards

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