Assembly Weight in Drawing

[verge]

How do I use my format to automatically pull in the weight of an assembly? I have the weight calculated and entered as a parameter. I have a two-cell table set up to display the name of the assembly (using asm.name for the report symbol) and the weight of the assembly (which is a parameter called ASM_WEIGHT).


What do I use for my report symbol to pull in the parameter ASM_WEIGHT? I'm thinking this should be darn easy, but so far I'm striking out...

 

[vlad1979]

[url]http://www.mcadcentral.com/articles/templates/proe.asp?artic leid=23&zoneid=2[/url]

 

[markp]

The way weight is handled in Wildfire is different from previous releases of Pro/E. Check out this from the PTC knowledge base:


https://www.ptc.com/appserver/cs/view/solution.jsp?n=120455


We call out the weight of an assembly in a table cell in the format using the parameter, &PRO_MP_MASS. Then you do not need a relation in the assembly to pull out the weight.

 

[verge]

I've read the article on Assembly Weights in the Drawing. It really helped as far as pulling the weights of each component into the assembly drawing. What I'm hoping to figure out now is how to pull the weight of the entire assembly into the assembly drawing without running a summation from the components' weight column. We want to remove that column from the format, as all we really need to know is the weight of the entire assembly. Running asummation also makes it so that I have to place the total weight of the assembly somewhere in the same table with the components' weight column, and I don't want to do that, since I don't want the components' weights displayed to begin with.


What do you think?

 

[markp]

Add the parameter called &PRO_MP_MASS to a table cell in your format.


View attachment 3272


Go to the assembly and pick Edit>Setup>Mass Props. Choose Geometry and Parameters in the Source drop down box. Choose Generate Report. The weight of the entire assembly should show up in that drawing table cell. You might have to regenerate the drawing.


Hope this helps get what you want.

 

[verge]

That worked perfectly. Can't thank you enough. This should be prominent in Pro-E help, but unfortunately doesn't seem to even appear there.

 

[verge]

One more simple question: How do I control the decimal places of the weight? I don't need to display the weight down to the thousandth of a pound, just to the pound would be fine...

 

[markp]

I think there is a way to control the number of decimal places by adding [.#] after the &PRO_MP_MASS parameter where # is the number of decimal places. Another way is to choose Format>Decimal_Places, enter the number and then choose the weight number. But then that changes the number of decimal places for any dimensions added after that.

 

[verge]

That worked nicely. Thanks!

 

[iamsagar89]

Add the parameter called &PRO_MP_MASS to a table cell in your format.


View attachment 3272


Go to the assembly and pick Edit>Setup>Mass Props. Choose Geometry and Parameters in the Source drop down box. Choose Generate Report. The weight of the entire assembly should show up in that drawing table cell. You might have to regenerate the drawing.


Hope this helps get what you want.

thank u..but if there is change in one of its part then it show new weight ??

 

[silverado8405]

After regeneration of the model, yes it will update the weight.

 

[iamsagar89]

assembly weight in drawing

Add the parameter called &PRO_MP_MASS to a table cell in your format.


View attachment 3272


Go to the assembly and pick Edit>Setup>Mass Props. Choose Geometry and Parameters in the Source drop down box. Choose Generate Report. The weight of the entire assembly should show up in that drawing table cell. You might have to regenerate the drawing.


Hope this helps get what you want.

...........yes it works but it show whole assembly weight in each part...is it possible to show individual weight of part in bill of material??