[PCB_FORUM] Re: IDF file??

Eileen,
 
    I replied yesterday with complete instructions.
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 

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Eileen Ong
Sent: Wednesday, August 16, 2006 11:14 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: IDF file??



Hi all,

I have successfully generated the .emp and emn files.

 

But the problem is the mechanical guys can only open the .emn file but
can't open the .emp

Any one familiar with ProE and know how to get these 2 files imported?

 

Also, the Mechanical is asking for .prt or .stp file format, anyone
knows if it's possible to generate this 2 type of format for mechanical.

 

Thanks

 

Best regards,
Eileen 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Andrew Noonan
(annoonan)
Sent: Thursday, August 17, 2006 12:16 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: IDF file??

 

Hi Eileen,

Mike gave you some good advice. I think I can add a little to what he
said. 

 

1. IDF is the right general format. When you click File>Export>IDF, make
sure you click on the drop-down box currently set to "IDF" and select
"PTC" (Parametric Technologies Corp., the company that makes Pro/E). The
contents of the two file formats are practically identical, just the
files extensions are different. 

 

2. Once you have generated both these files (*.emn, *.emp), your
mechanical folks should not have a problem. Either format (IDF 2.0 or
IDF 3.0) should work. 

 

3. What Mike said.

 

4. The reports function allows you to create custom reports. You would
need to do some reading and experimentation, but I'm sure it can be
done. Make sure to include the PACKAGE_HEIGHT_MAX and PACKAGE_HEIGHT_MIN
properties.

 

Hope this helps,

Andrew

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Eileen Ong
Sent: Wednesday, August 16, 2006 12:05 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

Other related posts: