Dimension unit in drafting.

[FBM]

When I have a 3D model, my dimensions are all in inches. When I transfer the 3D model over to Drafting it converts into some other unit of measurement. Does anyone know where or how to set the unit of measurement to always be in inches? Otherwise I had to right-click on each dimesion at a time, go to properties change the unit to in!!!!!

 

[navyn]

Hi FBM,u can rather use a macro to change dimensions unit as inches,coz changing dimension format manually is time taking than running macro,u can try this macro for this dimension unit change to inches:

Set mydimension = Drawingview.Dimensions.Item(1)

Set Dimvalue = mydimension.GetValue

Dimvalue.SetFormatName 1, "in"

I hope it works for u to some extent,


bye
Naveen

 

[ahbugeye]

What standard are you using? This will also determine what the default unit is for dimensions.

 

[FBM]

Hi ahubugaye
I am using CATIA V5R12.

 

[ahbugeye]

FBM
Standard I mean ANSI, ISO, etc. You can also set up and change these by changing the standards (you must be in Catia as admin) which are an xml file.

 

[itsmyjob]

Hi,

You should set an ENVIRONMENT.

In that ENVIRONMENT you can define sveral stuff, such as :

default settings (TOOLS/OPTIONS) and prevent the user to change them. Default path for saving file...

default toolbars, and position of toolbar, add icons for scripts, add or remove default function from a toolbar...

default standards, XML files used for drafting default parameters, styles or 3D parameters, default filters and layers...

and much more...

But for your pb, you should know which drafing standard you are using, and as a CATIA admin you should define the right parameter you need. Then once it is done, just update the standard of your drawing to the new well defined one.






Eric N.

catiav5@softhome.net

 

[FBM]

Ahbugeye
I am using the ASME standard. And also can you plz let me kmow clearly how to change the unit settings by changing the standards coz i have to tell to my admin to do it.

Naveen
I tried using the macro too but it didnt work me either. I am not sure if I am using it properly. can u breifly tell me that.

Eric (Its my job)
I already have my default settings defined and locked to in.

 

[coughcool]

Hello everyone and thank you for your comments thus far. I’m FBMs CATIAv5 admin and I’m new to CATIA.

We have setup a default environment for our engineers here. Our current problem is with drafting and the way it represents units of measurements. We design everything in American Standard Units along with ASME. So when working within our 3D part all units are in inches. Move the part over into Drafting and it changes the unit’s type. I’m sure this is just some setting in options somewhere but our problem is we don’t know which option in units it is.

Navyn- we have your script imported into our system but (and because we are new) we have no idea how it is meant to be run. For example – the first thing we did was import the script into the Macro area of CAITA. Then we opened up our drafting part and ran the scripted (which completed with out errors) but changed nothing. I’m assuming we just don’t know at what point your script is intended to be run. Can you clarify this for us?

Everyone else, thank you very much for your thoughts and Ideas.

RLord

 

[itsmyjob]

hi coughcool,

Do you need onsite help ? training ?

Have fun...

Eric N.

catiav5@softhome.net

 

[navyn]

Hi FBM and coughcool,that was only main script,thats why u got errors,
complete script is:

Sub CATMain()

Set DrawingDocument1 = CATIA.ActiveDocument

Set DrawingSheets1 = DrawingDocument1.Sheets
Set DrawingSheet1 = DrawingSheets1.Item("Sheet.2&quot 'here enter the name of sheet on which u working'

set Drawingviews1 = DrawingSheet1.Views
set Drawingview1 = Drawingviews1.Item("DrwDetail.1&quot 'here also change the name to ur current view'

Set mydimension = Drawingview1.Dimensions.Item(1) 'If its name is 'Dimension.1' in ur current sheet'

Set Dimvalue = mydimension.GetValue

Dimvalue.SetFormatName 1, "in"

End Sub

Now it works,

bye
Naveen

 

[ahbugeye]

coughcool

You need to start Catia as admin. Just being logged on as admin does not do this. Look in the help documentation on how to do this.

Once in there, go into Tools/Standards/Drafting. You will be able to edit the Drafting standard that you are using. I suggest saving it under a different name and location. That way when you go to upgrade your Catia version, you will still have the file to use. This is the standards where you can set up which unit to draft with by default, fonts, line types, etc.

coughcool, are you guys COE members? At the last couple of COE's, Catia User Conferences, there have been some good adminsitration presentations/sessions that explain how to do this. Go to

http://www.coe.org

and look under proceedings and you will be able to find the presentation that was given. You should find this helpful. If you haven't been on the site in the past, you may have to request a logon.

Hope this helps!

Jen

 

[FBM]

Naveen
Thx a lot. It worked for me.
Have a nice day.
FBM

 

[coughcool]

My thanks to navyn and ahbugeye for their help in tracking down and guiding me to the right location.

The answer to my question was

CATIAv5 Administration mode:

Tools > Standards > Category (drafting) File (company_ASME.xml) > Styles > DistanceLengthDimension > Default >ValueDisplayFormat > MainValue > Name (changed this to "in" for inches).

I repeated this step with Styles > RadiusDimension and Styles > DiameterDimension

This solved my issue.

Ahbugeye – we just recently signed up for COE and are planning on attending the next conference.


Again thank you.
RLord

 

[ahbugeye]

Your welcome coughcool. According to the COE pre-released schedule it appears that there are some administrations sessions going on. SYS-3: V5 CATIA Administration Advanced Tips and Techniques by Bill Duke, IBM might be a good session to attend.

Also, the DPC sessions sometimes give good heads up about enhancements to the code.