WT AND RELATION

[ASTALAVISTA]

Hi all,
I wanted to show wt. in my drawing cell..
This is what I did...
1.part-tools-relations-added relation 'mass=pro_mp_mass'
2.Generated report and then in drawing in that particular cell typed
Wt.
&mass Lbs.
I get the correct answer.But then I had to edit that part thickness and the 'Wt.' doesn't change in drawing.
I am having to delete that 'relation' then delete 'parameter' then add the same 'relation' again.
but again in drawing I get Wt. *** Lbs.So I am having to delete that note and add the same again.(&mass Lbs.).
Is there any way that this can happen automatically for me.
Because its just not related to that part.I am having to repeat the same procedure for any assembly that has this part.
Please help.

 

[ASTALAVISTA]

Oh I guess I can add
'&pro_mp_mass' instead of '&mass" I guess in that drawing cell..
correct me if I am wrong.
Also you are reading so might as well answer one more question if you happen to know the answer..
How can I add volume in drawing or in BOM?
Edited by: ASTALAVISTA

 

[dgs]

I think that you should be able to use &pro_mp_mass directly.

On the relations, Pro/E evaluates the relations first, prior to regenerating the model. That way all dimensions and parameters are set properly. Unfortunately, for parameters driven by mass/props, those will be evaluated based on the old model geometry.

There are two solutions for this:

1 - Regenerate the model twice. First regen updates the geometry, the second sets the mass/props parameters. Not ideal, but it works.

2 - The better way is to place your mass/props regen in the 'post regen' section of the relations dialog. Open your relations and look in the lower right corner. You should see a drop down that gives a choice between 'Initial' and 'post regen'. Click on 'Post regen' and place your 'mass=pro_mp_mass' relation there. Now it won't be evaluated until after the model has been regenerated.

 

[ASTALAVISTA]

Thanks Doug.
I tried both your methods on a test part.
Apparently '&mass' or "&pro_mp_mass' doesnt make any difference.
If I edit any part I need to
1.Generate report
2.and then regenerate the part and it changes the value in drawing as well
be that relation 'initial' or 'post regen'
may be I am not understanding it right.

 

[kdem]

You may alsowant to change the value for mass_property_calculate in your config.pro.

 

[kenppy]

To an earlier question about the BOM and part weights.
View attachment 4961

 

[anand_m_s]

Create a parameter called weight and use the following relation:

weight=mp_mass("")
Use this parameter in the repeat region to get the weight of part or assembly in the drawing.

 

[ASTALAVISTA]

got it guys....appreciate all your efforts...