How to show In Assembly Drawing??

[chandru.d]

Dear friends,
<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />
I have One Assembly with Door, I need to show that in drawing <B style="mso-bidi-font-weight: normal">closed position[/B] and <B style="mso-bidi-font-weight: normal">Open Position [/B]Also. (I am using ProE Wildfire 2.0)

<B style="mso-bidi-font-weight: normal">How to do that[/B]?

I tried in <B style="mso-bidi-font-weight: normal">explode[/B] View, There I am not able to <B style="mso-bidi-font-weight: normal">rotate[/B] the door (open Position), If anybody knowing this please Guide me..

(Note: I don't want to create new Family table instance)

 

[wsylvester]

snapshot in mechanism perhaps

 

[prohammy]

[url]http://www.mcadcentral.com/proe/forum/forum_posts.asp?TID=33 759&PN=15[/url]


Chandru.d,


The above thread is what you are looking for


Kev

 

[madanprabhu]

Chandru,


One way of doing it would be


1.)to have snapshots of different positions and make them available for drawing.


2.)In drawing you can have two views one with "Open" mode and other with "Close" mode.


3.)Change the display of the views to phantom display thru' View>Drawing display>Component Display.


4.)Now align one view with respect to another..so you have a common view with both positions and one shown in phantom lines...

 

[trgthiyagarajan]

dear chandru


make two different models of same kind, for the first(sayclosed)close one use the model of what u have, the next one(say opened)you change the assembly constraints just its opened, in the drawing keep adding the second model(opened) by drawing model, right click>properties>add model(opened)>setmodel(opened) adn do the need. i think so this will satisfy u.

 

[magneplanar]

Chandru,

an alternate way of doing this involves simplified reports. In your assembly model you place the door in two positions by assembling two parts to the model. You then define a simplified report to be: door open, door closed. On each of those reports you hide the door that is not in the position you want to show. Once you have done that you can call up the simplified report in your 2d drawing view using properties of the view ( or 3d for that matter) to show the two positions. You will have to make sure any BOM on the 2d does not add the additional door to the part quantity total.
This works great to show positions for demonstration. I always make a final assembly that is the production assembled model and remove any extra parts used for demonstration.

It is also possible to drive the assembly dimension from the 2d in the view if the dimension is "shown", but not hand created in the 2d. Be careful if you do that because it will drive the 3d model too.

cheers,

M