Drawing showing Part Weight & Volume

[arroyopr]

puppet:


try this first


View attachment 1119


then assign material


View attachment 1120


then go edit/set up


View attachment 1121











and then click on generate report

 

[arroyopr]

I forgot after all this you go to the dwg. insert a note like this


weight(lb)=&mass and it will give the analysis results base on the mat. you assign to it.

 

[Brian_Adkins]

If you're using WF2.0, and are using the "Generate Report" button, there is no need to create a separate parameter or a relation to drive it...


just use the new system parameter pro_mp_mass


(I think this has already been pointed out earlier in the thread)


Then, on the drawing, you can put the note "MASS = &pro_mp_mass kg"





Note that, in WF2.0, there are now two system parameters holding the mass
<UL>
<LI>mp_mass("") (this is the 'old-school' one)
<LI>pro_mp_mass (this is the new one)</LI>[/list]


Simply running a Model Mass Properties using the Analysis menu no longer updates either of these values. The Analysis menu method is simply for reporting the current mass without impacting the parameters (i.e. for a what-if on a simplified rep or something).


To get the system params to update, you need to use the Generate Report method. Same goes for the other mass-props params like area, volume, etc.


excerpt from: http://www.ptc.com/appserver/cs/view/solution.jsp?n=122900
"Description
-----------------
When calculating mass properties through the analysis menu, model parameters (Pro_mp_mass) are not updated,
whether the config.pro option:"Mass_property_calculate" is set to "Automatic".

Alternate Technique
-----------------
After changing model dimension, Select #Edit;#Setup;#Mass Props;#Generate Report;
the PRO_MP_MASS value will appear correctly.


Resolution
-----------------
This is correct behavior, the analysis feature is not designed to change mass properties to avoid overwriting
of model mass properties with possible temporary results, for example in case of simplified representations.
"


-Brian
Edited by: Brian_Adkins

 

[puppet]

Thanks guys it was a combo of things





needed the config.pro option to be set.

mass_property_calculate automatic




then using the pro_mp_mass in the drawing




thanks heaps.





this might be slightly off topic but how can i divide a number in side of the drawing?

ie have the mass displayed as grams kg and tonnes? i wish to do this in the note.

 

[Siron]

I think that you guys are going about it the hard way. Here is what I do:

1. First run your mass properties and under Saved Analyses pick the Add Feature button. Give the feature a name (I name mine Mass_Prop)

2. Create a relation using the analysis feature (see pic)

This will give you a relation that looks like this "WEIGHT=MASS:FID_88" or very close to it. FID may be differant.

3. Now all you will need to do is add the &WEIGHT[.2] to your drawing table
and it will stay updated at all times as long as you do a regenerate.

NOTE: Because this is a feature you must make sure that it stays at the bottm of the feature list in your model tree.

Oh BTW I have this set up in my startparts and Assys with my insert mode above the Mass_Prop feature. Once I am done with the model I resume and regenerate.


Edited by: Siron

 

[sbpanda]

Dear Siron


Where u got this relation diloge box, I am using WF2.


thanks


[email protected]

 

[deepakbhat_nie]

tools<relations


Deepak Bhat

 

[sbpanda]

I got it


[email protected]

 

[elab.theken]

For family tables, you will need to add the parameter to the table and verify the table in order for each instance to have the correct values.

 

[sbpanda]

Dear elab.theken


What u want to say, can u pl make it more brief.


thanks


[email protected]

 

[sbpanda]

How to put density in table by automatic with assembly drawings.


thanks


[email protected]

 

[sbpanda]

View attachment 2697

 

[arroyopr]

Youhave to add that parameter to the part. Then if you wish to show in the part dwg. just insert a note Density=&mp_density inch^3. On the assembly dwg add a colunm with a repate region selecting material/parameter/ptc_mass_density andthat should take care it.


View attachment 2699

 

[sbpanda]

Thanks arroyopr for ur reply.


Can I add the unit , automaticaly say for weight gm/cc.


thanks


sudhanshu

 

[arroyopr]

Do you mean convert what ever pro-e default is to gm/cc? Yes, just add a relation like:


G_mass=mass*453.5924


I've been told that my relations method are old school(and as far it works for me, i'll stick to it) then on the cell titleproperties just typeMassgm/cc, then repeate the proccess, insert dwg note on part dwg. And on assembly repeate region will be &assem.mbr.(udf)G_MASS.

















View attachment 2706

















View attachment 2707

 

[nagabhaskar_m]

very very thanks for ur help.

 

[pjw]

In order to showw different masses for family table instances you need a model analysis feature as part of your model. Unless you have Behavioral Modelling then all you are permitted to do is show the model anaysis results - not add the analysis as a feature. Otherwise, all the instances will show the same mass as the generic.


If you let me know your e-mail address I will send you a UDF which will add this feature to your model tree. Beware - it must be the last feature after any soild geometry (surfaces and datums are massless). If you use this feature in assemblies it will calculate mass on an average density principle. Pro/ENGINEER calcuates mass by multiplying the volume of the part by its density.


Add the following to you relations to create new mass paramters:


MASS_LB = MP_MASS("")
MASS_KG = MASS_LB/2.204





Alternaively you can avoid having to create these paramters by adding 'Paramter from Deature' to your famiy table.





Regards Phil

 

[looslib]

Just add the relations in the generic part, then add a column to the family table for the weight.

 

[AGaribay]

I too am trying to add the Part Weight & Volume to the Drawing, but not very successful. What am I missing?

1. I added the Relation
2. I Assigned the Material
3. I added note to drawing.


View attachment 2711

 

[arroyopr]

Did you add the parameter to the part?