Parameter change within drawings

[andysuth]

I'm combining office and ProE at the moment and need to change drawing scale within the ProE drawing environment.


I know there's a parameter, scale, to control this that can be controlled by the pretty standard formats and boarders, but I don't know how to change this through a relations editor as it appears WF3 doesn't let you have relations on a drawing, only on its parts or assemblies.





Any ideas?





I'd like to do something like:


ps=300


scale:0 =ps / MB_SPAN:4


Where ps is approx sheet width and MB_SPAN is a parameter from the assembly model.





Thanks,





-AS

 

[andysuth]

I've still not worked this out, if any one has any clues?

 

[vlad1979]

I think you may be able to do this with Pro-program to have some sort of relation: if the part length is too big then the drawing view to be scaled down.....justa thought...

 

[vlad1979]

I searched PTC site for this and found :


Additional Information
<DIV =indent10>


Description
-----------------
How to parametrically set the scale of a view based on a relation parameter.

1) Create a relation in the model like the following example:
if part_length >= 10
view_scale = 0.5
else
view_scale = 1.00
endif
</PRE>
2) In the drawing, select #Modify, #Value, and pick on the current scale view value. Instead of entering a number, enter 'view_scale' (without the quotes). Pro/ENGINEER will prompt: "Do you want to save this expression: view_scale ?" Select #Yes. As the value of the paramter part_length is modified the view scale will dynamically change upon model Regneration.


See if it's working</DIV>

 

[andysuth]

I'll try this with ceil and floor instead of this optional stuff.





I'll keep you posted.





-AS

 

[andysuth]

I searched PTC site for this and found :


Additional Information
<DIV ="indent10">2) In the drawing, select #Modify, #Value, and pick on the current scale view value. Instead of entering a number, enter 'view_scale' (without the quotes). Pro/ENGINEER will prompt: "Do you want to save this expression: view_scale ?" Select #Yes. As the value of the paramter part_length is modified the view scale will dynamically change upon model Regneration.


See if it's working</DIV>

Vlad,





I've used this relation in the main assembly:


/* RELATIONS (EXTRACT)


HALFSHEET = 290


SPAN_LENGTH = 15000
MAINVIEWSCALE = 5 * Floor(HALFSHEET / (SPAN_LENGTH * 5),3)


/* RELATIONS (END)


But can't see how to do the second half of the suggested solution.





I've tried double-clicking the scale value in the boarder (which allows numerical alterations) and accepts when I type MAINVIEWSCALE but doesn't even alter the value to MAINVIEWSCALE when it's acepted it.


Not sure where the MODIFY menu option is.


Is it allowed on WF3?





Cheers,





-AS

 

[andysuth]

I found a way to do this on the auxilary views, which aren't the mainview or projections, but not on the main view.





To do on auxilary view: left mouse button on the numerical value.


right mouse click, select from menu "Edit Value", change to the parameter name


(This I changed to mainviewscale:1 for the example relations above)


Press enter and confirm the change to the equation.





Change the length parameter.


Update.


the Drawing view scales should also update.


I've not got this to work for the main view or it's projected views, only auxliary views.


As a result, I now go into the primary general view and change from sheet scale to custom scale and then write "mainviewscale:1" (or just any old numerical value and then exit properties and right click on the scale numerals and "Edit Value" to mainviewscale:1)


This refers the sheet to a parameter value in the model/assembly directly referenced by the drawing (~:2 or ~:3 would refer to a model part within an assembly referenced by the drawing etc. etc. etc.)


Shove this in your Assembly relations (or top level part):


/* RELATIONS (EXTRACT)


HALFSHEET = 290


SPAN_LENGTH = 15000
MAINVIEWSCALE = 5 * Floor(HALFSHEET / (SPAN_LENGTH * 5),3)


/* RELATIONS (END)


If you're really swish (which I ain't!) you can use a little Pythagoras to so it isn't just dependant on the length but also the width of the part.


You may also want to remove the "halfsheet=290" and "span_length=15000" bits AFTER VERIFYING the relations: when you verify these will be added as parameters and so it'll be better if you remove them from the relations as you can then control the parameters e.g. from a drawing view.


Cheers for your help,


-AS
Edited by: andysuth