Thanks to Tracy Willis!:
Use the drop down menu in the Area analysis tool and create an analysis
feature...
The syntax in the drawing note will look like something like this…
&AREA:FID_XXXX or (ANALYSIS_AREA_1… the name of the feature)
The break down is this…
&AREA is the name of the parameter inside the Analysis feature.
:FID_XXX is the feature ID.
You can sometimes type the name of analysis in place of the “XXXX” and
Creo will automatically convert it to the ID number and display the area
value in the drawing.
If the model with the analysis feature is set as the active model in the
drawing when the note is created then you CAN use the "name of the
analysis feature" in place of the "XXXX" feature ID number.
If it's not the active model when the note is created then you need to
enter the feature ID number and then add a colon followed by the session
ID number.
Something like this FID_1234:0
To control decimal places:
FID_1234[.X]
X being the number of decimal places.
This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.
