view represent simplify in Pro/E wildfire?

[wiebe]

I need to remove machined holes from a flat pattern so I can create a DXF for laser cutting. In previous Pro/E versions I used view, represent, simplify. Menu mapper doesn't map this function, does anyone know how to do this with Pro/E Wildfire?

 

[peppinu]

Maybe not exactly what you are looking for. What we do, is we first "snapshot" the view (views, modify view, in 2001). This will turn the 3d view in 2d entities which you can delete after, we even go a step further by translating the profile's datum to the lower left corner (0,0) so that on the machine the profile to be cut would come at the proper datum.

Joe Borg

http://www.methode-eur.com

 

[wiebe]

I'm a little confused with the "snapshot" method. What type of file (.dxf?) do you end up sending to the cutter? What I am used to is creating a new sheet for the flat pattern to be cut, blank the format, set scale = 1, view represent simplify out any holes not to be cut by laser (this step I can't duplicate in Wildfire),set view to no disp tan / no hidden and finally save as a .dxf. This file is what goes to the laser cutter who imports it into his local machines program / software.

 

[Moroso]

What Joe is saying is instead of doing View Represent do a Snapshot of the view, that will turn it into a 2D unassociated view, from there you can delete the holes you do not want cut and then translate the rest to the 0.0 lower left corner.

HTH

Brian

 

[wiebe]

OK, I found the "snapshot" command, this will work in a pinch. I am a little hesitant to implement this method considering the view is not parametric after being converted to draft entities.

Thankyou both very much.

 

[peppinu]

Wiebe
You are right about the view not being parametric any more. You can do a "save as" on the drawing and keep it for records, besides you can delete the model from the drawing to end up with just a draft stable proe drawing. After all a .dxf is not in any way associated. I suggest that you do not save the original drawing with snapshot views.

Joe Borg

http://www.methode-eur.com

 

[Guest0527211403]

Would it be possible in your situation to create a family table instance of the part without the holes? You can create a drawing of this instance which will remain associated to the original model.

Another option is to use View-->Drawing Display-->Edge Display and use "Erase line" to get rid of what you don't want.

Hope it helps
Mark

 

[Guest0527211403]

I just ran across this page (

http://www.synthx.com/tom/sy_tip_0502.htm),

which answers your question directly.

Mark