[PCB_FORUM] Re: IDF file??

If you are generating files for ProE you need
to select PTC as your output choice.

In ProE have the ME do this procedure. (Wildfire version)
File/Open file.emn
Open as a PART ONLY.
Select OK or Done to any popup menus.
When board outline and holes are displayed do a SAVE.
Next, create a blank assembly.
Insert component/assemble.
Add the part created previously. Again, select OK or Done to any popup
menus.
Then do an insert Shared data/ from file. Select the .emn file.
(Yes, I know you used this file but the system needs it again.)
Then a popup will popup, ha ha, looking for the .emp file.
Select this file.
The system then goes about making all the parts, components, on the
board.
When it is done do a save. Only at this point are all the parts,
components,
actually saved on disk.

Many, many ProE engineers have tried, and failed, to import these files
by skipping
straight to the assembly. ProE has these instructions in their help
menu.

Good Luck!


Jerry

-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mike Finczak
Sent: Wednesday, August 16, 2006 10:18 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: IDF file??

Eileen,
        
        1) From the Allegro menu use -----> File
                                         -----> Export
                                             -----> IDF

           This will generate two files in your working directory
           with the extensions "LDF" and "BDF". Send both


        2) Try generating in IDF version 2.0. Also make sure that 
           the board outline is a continuous shape, and that it has
           a physical thickness in the board stackup. They may also
           be looking for a different file extensions, ask them.


        3) To view the height for a component, display the Place_Bound
           layer, and then select -----> Edit
                                     -----> Properties
                                         -----> Pick the Place_Bound
Box.
                                   (select only shapes in the find
filter)


                Shape at -6600.10,5698.71 on subclass PLACE_BOUND_TOP
                PACKAGE_HEIGHT_MAX = 364.17 MIL


        4) Not sure if reporting all heights is possible. Someone else
on 
           the forum may have a better answer.


Regards,
       Mike Finczak
       CopperCAD Design
       www.CopperCAD.com
       905-488-8958 



-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Eileen Ong
Sent: Wednesday, August 16, 2006 3:05 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] IDF file??


Hi all,
I'm trying to generate a 3D file (with component height) for the
Mechanical to verify.
 
1) Is this function export IDF? If not IDF then what file format should
I generate for them.
2) I have generated an IDF file and send to Mechanical, but they claim
that they can't read 
   in the file. They are using ProE. Can some one pls advise?
3) I have received the Brd file from customer, from layout, how do I
check the height of the
   component on board? (by attributes). 
4) Is there a way to generate a report on the component height?
 
Best regards,
Eileen
 

-----------------------------------------------------------
To subscribe/unsubscribe: 
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe

To view the archives of this list go to
http://www.freelists.org/archives/icu-pcb-forum/

Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
To subscribe/unsubscribe: 
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe

To view the archives of this list go to 
http://www.freelists.org/archives/icu-pcb-forum/

Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------

Other related posts: