At 12:38 PM 12/1/98 -0800, Donna Perry wrote:
>Yipes, I just wrote over my finished board file !!
>What software is available to convert PADS .pho
>files BACK into a database file???? Is there any
>help out there? (I am using good 'ole
>PADS-Perform.)
There used to be a product called GerbIn which would translate (or assist
translation) of Gerber data back into various CAD systems. It sold in 1993
for $1000, and the CAD modules were variously priced. PADS-PCB was $500 and
PADS-2000 was $750. GerbIn has been replaced by GerbCAM, and, when I asked
the company that sells it here, they were a little vague as to what it
would do. I didn't get their present name, but their better known product
is Unicam. Their phone number is 603-431-9411. GerbCAM is on special now
till the end of the year for $2500, and it *may* include numerous CAD
interfaces.
My guess is that these prices may be a bit much to pay for a single
translation job. So below is a generic method. It's a bit tedious, but
probably better than redesigning the board! Unless someone has appropriate
software and is willing to do the translation for cheap.
Presumably PADS-Perform has a facility for importing Gerber to a layer.
Hopefully, the original plots were done with flashes where possible rather
than draws. Let us pray....
Also copper pour will make things more complex....
Assuming flashes for pads and no copper pour, the basic idea is to import
the Gerber plots to the appropriate layers, note where pin 1 (or other
reference location) is for all components, delete the flashed pads and
replace the components with the original library parts. In some CAD
systems, it may be possible to place the components over the existing pads
and then delete the free pads afterwards, which will be faster. If one is
so lucky as to have generated a pick-and-place file, then component
placement might even be automatic, though it would require massaging the
data some to make a pick-and-place file into a component placement file or
macro.
Again, in some systems, it will be easy to convert all the flashed via pads
into true vias with holes.
The free lines making up text on the board will be replaced with actual
text....
Once one has a board file which *looks* like the original CAD file (it will
generate the same photoplots, presumably), then the original net list
should be imported. Again, most CAD systems can do this and automatically
assign nets to the pads, traces, and vias on the board according to their
connectivity. And then the board can be DRC'd. If it passes DRC, presumably
it is the same as the original design or close enough....
If the original net list is unavailable (which should not be the case),
again, most CAD systems can generate a net list from the board.
I used to do Gerber imports with Tango for DOS, using the above procedure,
except that these were Gerber files from a foreign (to me) CAD system, so I
needed to make the library parts as well. I wrote utilities to assist in
the translation, most particularly, a utility that would read a drill file
and convert the surface pads (which is what you usually get from Gerber)
into through holes with the appropriate hole size. I could then create
library parts, after numbering the pads, since Tango allowed the conversion
of free primitives into library parts.
[log in to unmask]
Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433
################################################################
DesignerCouncil E-Mail Forum provided as a free service by IPC using LISTSERV 1.8c
################################################################
To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body:
To subscribe: SUBSCRIBE DesignerCouncil <your full name>
To unsubscribe: SIGNOFF DesignerCouncil
################################################################
Please visit IPC's web site (http://www.ipc.org) "On-Line Services" section for additional information.
For technical support contact Hugo Scaramuzza at [log in to unmask] or 847-509-9700 ext.312
################################################################
|
