[PCB_FORUM] Re: Importing orCAD schematics
- From: "Edwards, Keith" <keith.edwards@xxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Fri, 5 May 2006 09:15:28 -0700
Gary,
Since you mentioned that it is a small design, you would probably
benefit from exporting the Allegro (PST) netlist. This allows a better
check between the logic and physical data (it syncs up the pin count
better between the logic/physical parts and could catch errors). There
are some things that must be done such as pin number AND names must
exist for each logic symbol. You also have to add the PCB footprint
names in the schematic symbol. This is easy for small schematics. Just
click on your .dsn in Orcad, from the pulldown menu select
Edit-Properties then type the names into the PCB footprint field. You
will now be able to create the PST files assuming the schematic packages
correctly.
If you choose to do the 3rd party netlist, you will have to edit the
package section of the netlist. You will also need device files for
each part type. You could generate them using the attached file which
will dump libraries (dra, psm, bsm, pad, txt, etc) from any BRD file
that is in the folder which you run the file. Just rename it to a .bat
file and you should be good to go.
Just incase the attachment does not make it, here are the contents of
the batch file.
::dumps info from all cadence brd files in a folder where the batch
folder is ran
FOR /F "usebackq delims==" %%v IN (`dir /od /b *.brd`) DO
%CDSROOT%\tools\pcb\bin\dump_libraries.exe -pdamsflcx %%v
-Keith
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of
ryan.donna@xxxxxxxxxxx
Sent: Friday, May 05, 2006 8:50 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Importing orCAD schematics
Gary,
If you are using v10 of orcad you do not need the device files at all if
they output the netlist in the allegro formatted files (3 pst*.dat files
just like concept). If they gave you these 3 files, import logic ->
select "cadence" tab -> select "design entry CIS" and "Import Cadence".
If they did not give you these 3 files, ask them to output the netlist
from orcad by running Tools -> Create Netlist -> select the "allegro"
tab -> check box for "Create Allegro PCB Editor Netlist". This will
output the 3 pst*.dat files.
Donna
-------------- Original message --------------
From: "Gary MacIndoe" <gary.macindoe@xxxxxxx>
Patrick,
Thanks for the response. I found out that the schematics are
orCAD v10, but I doubt that they are pointing to my Allegro symbols.
So, if this is the case, I have to create a device file for each
different part (i.e. 0603, sot23, tsop24 etc.), right?
I did a library dump on a design I'm working on now, and here is
the device file for a 60 pin BGA:
(DEVICE FILE: DDR2DRAMX8_60-60)
PACKAGE BGA60_8X12MM_0P8MM
CLASS IC
PINCOUNT 60
PINORDER 'DDR2DRAMX8_60-60' A0 A1 A10 A11 A12 A13 A14 A15 A2 A3
A4 A5 A6 A7 A8 A9 BA0 BA1 BA2 CAS_L,
CKE CK_DH CK_DL CS_L DM DQ0 DQ1 DQ2 DQ3 DQ4 DQ5 DQ6 DQ7
DQS_DH DQS_DL NC0 ODT RAS_L VDD0 VDD1,
VDD2 VDD3 VDDL VDDQ0 VDDQ1 VDDQ2 VDDQ3 VDDQ4 VREF VSS0
VSS1 VSS2 VSS3 VSSDL VSSQ0 VSSQ1 VSSQ2,
VSSQ3 VSSQ4 WE_L
PINUSE 'DDR2DRAMX8_60-60' IN IN IN IN IN IN IN IN IN IN IN IN IN
IN IN IN IN IN IN IN IN IN IN IN IN,
BI BI BI BI BI BI BI BI BI BI NC IN IN POWER POWER POWER
POWER POWER POWER POWER POWER POWER,
POWER UNSPEC GROUND GROUND GROUND GROUND GROUND GROUND
GROUND GROUND GROUND GROUND IN
FUNCTION G1 'DDR2DRAMX8_60-60' H8 H3 H2 K7 L2 L8 L3 L7 H7 J2 J8
J3 J7 K2 K8 K3 G2 G3 G1 G7 F2 E8 F8,
G8 B3 C8 C2 D7 D3 D1 D9 B1 B9 B7 A8 A2 F9 F7 A1 E9 H9 L1
E1 A9 C1 C3 C7 C9 E2 A3 E3 J1 K9 E7,
A7 B2 B8 D2 D8 F3
PACKAGEPROP DEVICE_LABEL 'X8 SSTL2'
PACKAGEPROP HEIGHT '0.xxx'
PACKAGEPROP PARENT_PART_TYPE DDR2DRAMX8_60
PACKAGEPROP PARENT_PPT DDR2DRAMX8
PACKAGEPROP PARENT_PPT_PART 'DDR2DRAMX8_60-60'
PACKAGEPROP PART_NAME DDR2DRAMX8
END
Do I really need all of this in the device files (obviously a
0603 device file would be much simpler!), or are there just a few basic
things needed?
Could I do a library dump on a very large Concept -> Allegro
design that uses many different symbols, then use the device files for
the orCAD design?
Sounds like it could be quite a job creating all of the device
files for a pretty good size design!!
Thank for the help Patrick!
Gary E. MacIndoe
PCB Design Engineer
Advanced Micro Devices
Longmont, Colorado
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of westfeldt
Sent: Thursday, May 04, 2006 4:50 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Importing orCAD schematics
If your customer has v10 or higher, and has your footprint names
in the schematic, then you should have him put out the special allegro
netlist set. Otherwise, there is a fair amount of 3rd party setup you
have to do, including creation of simple device files.
Patrick Westfeldt, Jr.
720-406-0887
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Gary MacIndoe
Sent: Thursday, May 04, 2006 4:37 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Importing orCAD schematics
Hey guys,
Sorry if this has been covered lately.
I have been asked to do a small design for Marketing (!?!), and
they, for some reason, use orCAD for schematic capture. It has been
years since I imported anything but Concept HDL.
So in the Import Logic window, Other tab, do you just point to
the orCAD netlist (?) in the "Import netlist:" field? Anything else or
is just that simple?
Thanks for any help!
Gary E. MacIndoe
PCB Design Engineer
Advanced Micro Devices
Longmont, Colorado
::dumps info from all cadence brd files in a folder where the batch folder is
ran
FOR /F "usebackq delims==" %%v IN (`dir /od /b *.brd`) DO
%CDSROOT%\tools\pcb\bin\dump_libraries.exe -pdamsflcx %%v
pause
Other related posts:
