Unable to change default units in CATIA V5 R26 Drafting Workbench

[Ratinoff]

I'm using CATIA V5 R26 at my job and I'm not the CATIA Admin, I'm just a user. When working in the Drafting Workbench, the default for Numerical Properties is "FEET-INC" (feet-inch) units with "0.01" number of decimal places. See screenshots below for these defaults.

<IMG>https://lh3.googleusercontent.com/p...Gf1DXkDmL67NTcXFFlig=w179-h83-s-no?authuser=0</IMG>

<IMG>https://lh3.googleusercontent.com/p..._URVOZPunTEIC6a0xRg=w172-h273-s-no?authuser=0</IMG>

<IMG>https://lh3.googleusercontent.com/p...pFrnv5PgZ2N0jXhE9lQ=w177-h270-s-no?authuser=0</IMG>

When I change the units to "in" (inch) and set the number of decimal places to "0.001", a measurement of .375" will display as ".375", as desired, however a measurement of .38" will display as ".38", not ".380" (three decimal places) as I desire.

Note: in my Tools -> Options -> Parameters and Measure menu, my default unit of length is inch.

Is it possible to change the default units for Numerical Properties to inch and to have it always display three (or four, etc.) decimal places? If so, how do I make this settings change? Do I need to have Admin privilege to do this?

Thanks,

-Ratinoff

 

[Ratinoff]

Also, if someone knows how to code the hyperlinks I provided so that they display as images instead of hyperlinks, please let me know so I can fix this. Thanks in advance.

-Ratinoff

 

[MrCATIA]

File + Page Setup can be used to choose a Drafting Standard with default dimension options. Choose ANSI or ASME to get default inch dimension values (I think it's NUM.DINC)

ANSI and ASME keep trailing zeros and maintains the decimal places. JIS, DIN, ISO drop trailing zeros.

You need ADMIN privileges to create or modify a Drafting Standard.

 

[MrCATIA]

I use the Insert and the Attach option to add images to my posts

 

[Ratinoff]

File + Page Setup can be used to choose a Drafting Standard with default dimension options. Choose ANSI or ASME to get default inch dimension values (I think it's NUM.DINC)

ANSI and ASME keep trailing zeros and maintains the decimal places. JIS, DIN, ISO drop trailing zeros.

You need ADMIN privileges to create or modify a Drafting Standard.

ANSI is already selected in Page Setup, so when I select ANSI or ASME and then click OK, there is no change to the number of leading or trailing zeros on dimensions already applied to the drawing. There is also no behavior change when I add dimensions. Is there anything else I should try to fix the issue?

 

[Ratinoff]

I use the Insert and the Attach option to add images to my posts
View attachment 3090

This worked. Thanks!

 

[MrCATIA]

View attachment 3092

ANSI is already selected in Page Setup, so when I select ANSI or ASME and then click OK, there is no change to the number of leading or trailing zeros on dimensions already applied to the drawing. There is also no behavior change when I add dimensions. Is there anything else I should try to fix the issue?

Click on the Update button after you choose a different standard. This will update all existing dimensions and annotations to the new standard. Then save the drawing with the new standard.

If the dimensions still aren't what you want, I guess you'll have to make a new Standard. Make sure you logon with ADMIN priviledges. A good way to start is to copy one of the original standards (xml file) and then just modify the settings.

 

[Ratinoff]

Click on the Update button after you choose a different standard. This will update all existing dimensions and annotations to the new standard. Then save the drawing with the new standard.

If the dimensions still aren't what you want, I guess you'll have to make a new Standard. Make sure you logon with ADMIN priviledges. A good way to start is to copy one of the original standards (xml file) and then just modify the settings.

After clicking the Update button, no changes were made to the drawing (including changing leading or trailing zeros of a dimension) as far as I can tell, so I've contacted the CATIA Admin at my job so they're aware of the issue. I'll post here what the resolution is after the issue is resolved. Thanks.

 

[Ratinoff]

File + Page Setup can be used to choose a Drafting Standard with default dimension options. Choose ANSI or ASME to get default inch dimension values (I think it's NUM.DINC)

ANSI and ASME keep trailing zeros and maintains the decimal places. JIS, DIN, ISO drop trailing zeros.

You need ADMIN privileges to create or modify a Drafting Standard.

This post essentially solved my problem, because I was able to download a template (.CATDrawing file) from my company's engineering repository (PLM system) and that possessed a particular Standard, in this case ASME-D-J. When this Standard is selected, the correct number of leading and trailing zeros displays (in inch units) when a dimension is placed in the CATIA V5 R26 Drafting Workbench.

If I wanted to manually get the correct number of leading and trailing zeros (in inch units) to display in the Drafting Workbench, I had to select NUM.DINC in the Numerical Properties toolbar.

See image below for reference.



Thanks again @MrCATIA.

 

[MrCATIA]

Thanks for the update! That's a good idea to check older drawings for another standard.

Have you tried to edit the ASME-D-J standard to use the NUM.DINC property?