extreme positions in drawing 1

[luckym]

Hi.
Is there any possibility to show in drawing views extreme (boundary) positions of parts or assemeblies?
For Example: other position of lever.

Thank You for help.....
michal

 

[im4cad]

If I understood correctly your question, in your case you can create a view of your lever, create a snapshot of it (make it a 2D view, not related anymore with the part), create a group including all 2D items included in that snapshot, and move it in the right place. After that (to have your 2D items follow the view in case you move it) use View --> Relate View -->Add Items --> Select your view --> Pick Many --> Select your 2D items --> Done
You can change the line style (for example “Phantom”), to show that that’s not a real part, it’s just another position for that part).


im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[luckym]

OK thanks.....
If I understand..... I'll turn lever to other position, create part of view with "use edge" and then "relate view".
But it is lot of work.... if that view is complicated.
Is there any other way to do this and keep dependency?

thanks
michal

 

[im4cad]

There is no need to use edge.
Just create a view of your lever in the desired position, make a snapshot from it, group all the 2D items from your snapshot, move it to the right place, and relate view. It takes 3-5 minutes
If you want to keep the dependency, you may add your lever again in your assembly, to show the other position.

im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[Hora]

Michal,

You can use also Pro/Mechanism or Pro/Process or family tables to keep the dependency between the solid and the drawing.

-Hora

 

[luckym]

To Hora:>
Will You explain me it more closely?....thanks
for example how to use family tables for it?


To IM4CAD:> What is SnapShot?

luckym

 

[Hora]

Michal,

It's easy to use family tables. Assemble your lever in a position. If you need to rotate it, use datum planes or coordinate systems. In that way, you can rotate it to the position you want. Then choose FAMILY TAB->choose to insert a dimension, click an the lever and select the assembly dimension. Then create a new instance name and change the value for the dimension added in table.

Good luck

 

[im4cad]

Michal,

A snapshot is when you need a 2D view in Pro/E not related any longer with the 3D part, or assembly. The view looks just the same, but now you can edit the line type, color, etc.
Try for yourself as an exercise:
View --> Modify View --> Snapshot

im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[luckym]

To im4cad:>> thank You ..... I understand now ) I have never used this "Snapshot" ..... Thanks

To Hora:>> Well. I know use family tables but I don't know how to apply this tables in drawing .....
I mean it like this: I have created two instances of assembly in FT. (Different possition of lever)
Then I add 1st view to drawing (view of 1st instance)
and then, 2nd view (next instance) and finaly I align this two views and modify line styles ..... Have You thought it like that?

And what about PRO/mechanism an Pro/Process?
I can work with PRO/mechanism but I haven't any IDEA how to use it on that.

 

[Hora]

Michal,

If you only need to show the lever posision only and not the entire assembly then why don't you add a simplified representation to remove the unnecessary parts for instance B?

Or, to avoid family tables, you can add in your assembly once again the lever in a new position and then create two simplified reps (one for lever in position A and the other for lever in position B, while master rep will keep both levers). This can give you a little bit of work in BOM (due to qty of 2 for levers), but you can fix this in relations.

Mechanism -> you need a licence for this -> can snaphot positions for levers and then insert them in drawing.

Pro/Process -> you also need a license for this and is a little bit more complicated -> you need to create a new assembly an choose process as subtype-> then create the assembly process plan where you can put your lever in position A and B.

-Hora

 

[Hayden]

I'm with Hora's last suggestion here. Assemble the lever in it's 2 different positions.
-Create a family table with the generic showing the lever only once, in it's home position.
-Create an instance (inst A) where the lever appears in both positions.
-Create a view in you drawing of inst A. Use View/disp mode to make the extra lever phantom.
-Change drawing model to the generic and create your main views of the assembly.
-Make sure this is the active model when you create your BOM.
I'm not 100% sure on this as I'm not currently working on Pro E (Wish I was!!) but I am 99%.

Cheers

Hayden

 

[luckym]

OK thanks You All

 

[prakashshan]

hai luckym,
To place the family table instances in the drawing ,use addmodel option.ie.,first create the no of instances in the model then prepare drawing,when you entered in the drawing menu automatically pro/e will ask you that which instances you want to create the drawing,select generic first then use add model option and select the instance then repeat the same for no of instances,
hope this will helps,
regrds,
prakash