cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

SOLVED
Newbie

Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Hello

 

I am trying to show the surface of a part in a note .

To do so i tried to calculate the mass properties by going in to < File > <Prepare> <Model properties> and calculate the mass properties there.

Then in relations i defined a term "Surface_Area=PRO_MP_AREA"

After this in drawing i placed a note "&Surface_Area"

So i got the surface are of the part.

But now if i edit my part, the surface area in the note doesn't change accordingly in this method.

 

So please suggest a method by which if i edit my model, my values for surface area should also be changes automatically.

 

Thank You

Sumeet

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

I think that your problem is that, by default, the built in PRO_MP_XXX parameters do not auto-update after regeneration.

You have to go into File->Prepare->Model Properties->Mass Properties (change)->Calculate... (or Generate Report...)

However, you can calculate the mass properties upon regeneration if you set the config.pro option:

mass_property_calculate automatic

(other options available, check configuration editor)

---

2nd point: you shouldn't have to make another parameter and equate it's value to that of PRO_MP_AREA.

Just use &PRO_MP_AREA directly in your note.

----

3rd point:

Since the behavior of your model's usage will vary depending on end-user's config.pro state,

I suggest you might want to utilize the measurement tool to create an area analysis feature and then display its calculated AREA parameter in your notes:

surface_area_in_a_note.png

Notes:

1) the syntax to display the parameter AREA which belongs to a feature called OVERALL_SURFACE AREA is &AREA:FID_OVERALL_SURFACE_AREA

2) [.1] is a modification code to round the display of this parameter to 1 decimal place;

3) you'll notice that when you edit this note afterwards, the OVERALL_SURFACE_AREA will have been replaced by the feature id number.

View solution in original post

10 REPLIES 10

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Are you regenerating the model after the edit?

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Yes i have tried it.

I aslo went to 

File-->Prepare-->Model Prooerties and re calculated the mass properties

And after calculating i regenerated the model too

But in the drawing also i updated the sheet, but still not working

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Hi,

if you defined Initial relation then you have to regenerate your model twice.

Please upload your model and drawing for testing purposes, if it is possible. Use How to Attach a File to a Discussion Reply procedure.

MH


Martin Hanák

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Can the relation be moved to the footer?

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Hello,

Sorry, in my last reply i was wrong about:

"Even after recalculating and regenerating, the values won't update"

Actually they do get updated after recalculating and regenerating.

But i wanted to ask, is it possible to updated the value without having to recalculate every time i update my models.

Because my model comes with the family table with 9 instances, and i have to go to each instance and recalculate the mass prop. to update my values.

So is there any relation that we could define or any other method.

Thank you

Sumeet

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

I think that your problem is that, by default, the built in PRO_MP_XXX parameters do not auto-update after regeneration.

You have to go into File->Prepare->Model Properties->Mass Properties (change)->Calculate... (or Generate Report...)

However, you can calculate the mass properties upon regeneration if you set the config.pro option:

mass_property_calculate automatic

(other options available, check configuration editor)

---

2nd point: you shouldn't have to make another parameter and equate it's value to that of PRO_MP_AREA.

Just use &PRO_MP_AREA directly in your note.

----

3rd point:

Since the behavior of your model's usage will vary depending on end-user's config.pro state,

I suggest you might want to utilize the measurement tool to create an area analysis feature and then display its calculated AREA parameter in your notes:

surface_area_in_a_note.png

Notes:

1) the syntax to display the parameter AREA which belongs to a feature called OVERALL_SURFACE AREA is &AREA:FID_OVERALL_SURFACE_AREA

2) [.1] is a modification code to round the display of this parameter to 1 decimal place;

3) you'll notice that when you edit this note afterwards, the OVERALL_SURFACE_AREA will have been replaced by the feature id number.

View solution in original post

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Hi,

you can define Post Regeneration relation instead of Initial.

postregen.png

MH


Martin Hanák

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Thank You everyone for your ideas and inputs

Sumeet

Re: Placing parametric note for Surface Area/Volume/Mass in Drawing (Creo 2.0)

Hi,

maybe the following info will help...

1.]

If you modify model containing family table, then you must run Verify command and then save the model.

2.]

Attached part contains family table with W column. The value in W column is computed via Post Regeneration relation w=pro_mp_mass.

I guess you can use similar procedure for model surface area.

3.]

My config.pro contains following option ... mass_property_calculate AUTOMATIC

MH


Martin Hanák