How to make the mass of a solid body occur as a note on master model drawing?
Solution
- open the drawing template part from TC to NX e.g. Drawing-A1-Size-template-A
- in NX - FILE - Utilities - Attribute Templates:
- in Definition Title type in : DB_DWG_TEMPLATE_MASS - Enter - OK
- Menu - Insert - Annotation - Note
- Category: Relationsship - Insert Part Attribute - select the just created DB_DWG_TEMPLATE_MASS - OK (may add a Name e.g. Weight as text Input ->Weight
WRef1*0@DB_DWG_TEMPLATE_MASS) and Setup on drawing - close the dialog- save and close the drawing template part
- in NX create a new model part - Insert a design Feature - add a material to the Body - OK
- in the part properties go the "Weight" tab and select"Update Data on save" - OK - save the part
- open the properties Dialog again and add Attribute MASS (defined in DB_DWG_TEMPLATE_MASS):
- Title: MASS , Data Type : String, select "Expression Formular" delete the "" arrow down go to Reference - Formatted Expression... - in the Relationship Dialog select Reference: Part Attribute , NX_MASS, OK - OK
- save the part
- File - New - Item - Drawing (master model) , Chose the configured drawing template Drawing-A1-Size-template-A
--> see the Weight appears on the drawing
Notes and References
IR 9110484
Hardware/Software Configuration
Platform: INTL64
OS: window
OS Version: 764SP1
Product: NX
Application: NXMANAGER
Version: V11.0.2
Function: ATTRIBUTES
Ref: 001-9110484