Family Table Information

[ttx]

Hi,
Can anyone tell me the proper method and syntax for extracting a family table instance name and displaying it in a table on a drawing format? The format that I want to display it in has a table that is not a repeat region.

Thanks in advance,

JW

 

[3dlogix]

If you don't have a repeat region, then just enter the model name in the appropriate table cell. Use the Table/ Enter Text command.

The text should be entered as "&model_name" , don't use the quotations (&quot. If you have more than one model in the drawing, then make sure to select the correct model and make it active.



Steve

http://www.3dlogix.com

 

[ttx]

Thanks Steve,
When I open a new drawing,Pro/E prompts me for the model name, rather than automatically pull it from the family table. Is this the way you would expect it to work - I am guessing not?
I did enter <&model_name> into the format table.
What did I miss?

Thanks

JW

 

[Hora]

TTX,

If you open a new drawing in PRO/E without having any model in memory, PRO/E will ask you to enter the model name. If you let it &quot;NONE&quot;, no model will be retreived in your drawing. At this moment, your drawing has no 3D geometry associated with. If you already typed the &quot;&mode_name&quot; in your table, instead of showing the instance name, PRO/E will display this: MODEL NAME.

What you have to do is just click VIEWS. At this moment, PRO/E will ask you to select your model and then will continue with the normal placing wiew procedure. Once you placed the view, regenerate your drawing. Now you will see the instance name in the table.

TIP: look at the bottom of the DRRAWING AREA and you will see something like that:

TYPE: DRAFT NAME: NONE SIZE: A

NONE means that your no 3D model is associated with your drawing.

Now, if you place a model in drawing, you will see something similar with this:

SCALE: 1/1 TYPE: PART NAME: 838456 SIZE:A
Right after the NAME: is the model name.

Now, back at the NEW DRWING menu:

If instad of &quot;NONE&quot; you are browsing for your family table model, then and only then, PRO/E will open a new menu and will ask you to select the instance.

Attention to the parameter &model_name. Must be written in lowercase and NOT in uppercase.

Have fun!

 

[ttx]

Thanks (Hora),
I thought that I new enough about Pro/E parameters to pull this one off - I guess not.
It seems the only thing I missed was &model_name (lower case!)
I assumed that any text entered into a table had to be upper case - to be displayed as upper case.
Thanks for your very detailed explanation.

JW

 

[Hora]

JW,

You're welcome.

Because you opened this discussion about parameters, note that &model_name will work only in drawing mode.

If you try to obtain a model name in assemby or part mode, you cannot use this parameter. Try using this: (in part mode)

RELATIONS -> EVALUATE -> model_name (note that you must write model_name and not &model_name)

PRO/E will retur a ERROR :Invalid symbol 'model_name' found.

You may use this parameter:

rel_model_name

This parameter will return the name of the part.

Hora.