I did as desribed and I'm not getting the results I think I should. I added a note on the drawing: &weight[.4] and this is what shows up...=mp_mass()[.4]. Is the parameter added to the model a String or Interger or doesn't it matter? I added it as a string.
I'm still having no luck with this. It tells me the value for the parameter has to be a whole number. In Part Mode when I create a parameter it asks for parameter name: I type weight, then it asks for parameter value: I type mp_mass(), thats when it tells me I have to input a whole number.
In Drawing Mode am I correct by entering the &weight[.4] in a note to show up in the General Notes of the drawing?
Apologies, first create the parameter weight and then write the relation weight=mp_mass().
Note that refers to model path which in part mode can only be the part itself. In assembly mode refers to the top level of the assembly but you can write a path to another sub-assembly or component to compute the mass properties for that.
Note that regenerating a model does not automatically compute the new mass properties, you have to run another model analysis to update mass propery values..
We have established the weight and volume on the print.
However, we have created drawings from a family table part and the weight and volume is the same on the new drawing. We no that it shouldn'y be this way because the model analysis show that. Why can we not get the correct values to show on the second drawing of the family table component?
First try opening your drawing model instance and compute your mass properties there. Unfortunately everytime you run a mass properties analysis this will get overwritten.
One suggestion I received years ago to handle instances was to create an assembly with all instances and use the path feature () to calculate the individual mass props - hope you don't have many instances.
I'm not sure but I don't think PTC has ever seen fit to resolve this....
OK, I found this thread and it is just what I need. But I am having problems. I created a parameter for volume - real number. Then when I try to create a relation volume=mp_volume() I get an error "Invalid data type combination at right side of expression". What am I doing wrong?
I just tried to do this operation for creating automatic entries for volume on a drawing in Wildfire 2 and I could not get it to work even after following these instructions and having had success in the past (pre Wildfire). I can only think that Wildfire 2 is different from previous releases. I have however found a solution (after 2 hours!) and it is as follows:
<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />
Set the following config.pro option
I can suggest a pretty easy soloution to the problem, create an analysis feature, and in your options create a parameter say called "volume". Now move the analysis feature to the footer. You can set a relation to make a parameter equal to the feature parameter called volume, or you can just access the feature parameter. Since the feature is at the footer everything gets regenerated at the end so there are no regen problems. For a Family table you will need to add a parameter and put it in the FT.
This works on WF 2.0 not sure about 1.0, we used this on a start part to make the COG and such really easy to access instead of the traditional internal parameters...