Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Drawing showing Part Weight & Volume

pjsmith

New member
How can I set the parameters in my model and create automatic table on either the format or drawing that show part weight and volume?-by psmith
 

dougr

New member
Create a parameter in your model(model-setup-parameters), e.g:



weight=mp_mass()



You can then enter this parameter in the drawing:



&weight[.2]



2 being the number of dp you want displayed..
 

pjsmith

New member
Thanks for the input Doug.

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.
 

pjsmith

New member
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?
 

kvision

Moderator
Create a relation.

Enter weight=mp_mass()

regenerate model and do a model mass properties analysis to fill the value. Designate all parameters. In the drawing enter &weight and you will get the value.
 

dougr

New member
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..
 

pjsmith

New member
Dougr or Anyone,



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?



Thanks, psmith
 

dougr

New member
This is where it gets complicated.



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....
 

billtornio

New member
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?
 

robertib

Member
You may need to run an analysis to get a volume first -since there is no volume recorded, there is no data, hence "Invalid data type combination at right side of expression".
 

billtornio

New member
Thanks for the reply. I already had the mass properties analysis run. Ran it again just to make sure, then tried to create the relation, but got the same error.
 

lbotez

New member
If you have a family table just add the parameters to the table. They should update accordingly.


One more thing: add a model analysis feature at the end of your model tree to force mass properties calculation at each regeneration.
 

spetch

New member
Hi,

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-com:eek:ffice:eek:ffice" />
Step 1
Set the following config.pro option

mass_property_calculate automatic

Step 2
click on
edit
 

sanjeevkar1

New member
hi



write a relation: weight=mp_mass("")



run the analysis

and designate the paramter generated. its done.



in case relation shows error

edit program



just copy the line "partxxxx"

(the second line i hope)

and paset it at the end of the page just before "end massprop"

the last line.



i hope it works



for me it did
 

slashct

New member
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...
 

puppet

Moderator
hey guys,

when i enter "weight=mp_mass("")" into my relations editor i get the following error





errorMass properties for this model are not calculated yet.



if i calc model mass properties, then do it i get the same errror.







i mean i can beat this using a anaylsis feature as "Slashct" mentioned, but i was under the impression that it wasnt needed
 

Sponsor

Top