[PCB_FORUM] Re: Importing orCAD schematics
- From: "Gary MacIndoe" <gary.macindoe@xxxxxxx>
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Fri, 5 May 2006 11:29:02 -0600
Thanks Keith, sounds like it's not going to be easy, even with the orCAD
schematics being created with v10.
Regards,
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 Edwards, Keith
Sent: Friday, May 05, 2006 10:15 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Importing orCAD schematics
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
Other related posts:
