[PCB_FORUM] Re: Importing orCAD schematics
- From: "Edwards, Keith" <keith.edwards@xxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Fri, 5 May 2006 10:18:19 -0700
Gary,
The device file creation can be simplified by the file I sent over in my
last mail (not sure if you received it yet).
Also, to get the PST files, just follow my instructions in my previous
email. I did forget to give you one step so here it is again.
Open the schematic
Click on the .dsn
From the pull-down menu, select edit, browse parts and select all parts
From the pull-down menu, select edit, properties
You will now see a column for PCB footprints. You will have to give each
part the correct Allegro symbol name
Assuming the schematic is correct and you have pin names/numbers, you
should be able to package using the Allegro tab to create PST files.
You will not need device files using this method. You can just import
the PST files by pointing to that folder when inside Allegro.
One other hint in Orcad, to copy and paste, use the following
shortcuts...
Copy = Ctrl + Insert
Paste = Shift + Insert
-Keith
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Gary MacIndoe
Sent: Friday, May 05, 2006 10:06 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Importing orCAD schematics
Thanks Patrick, I was hoping that if I needed to create device files,
that they could be simplified.
So Donna from Comcast says that if it is orCAD v10, the schematics can
output netlist files specifically for Allegro, it creates the needed
pst*.dat files, and separate device files are not needed. Sound right
to you?
So then the only thing I can see that would need to be done is for the
orCAD schematics to be pointing to the same files that Concept points to
in order to get the Allegro symbol information.
Thanks for helping out!
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 westfeldt
Sent: Friday, May 05, 2006 10:07 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Importing orCAD schematics
You are right, your netlist will probably not have anything like
functions, etc. In general, you don' tneed anything except package,
class and pincount, but if your numbering is alpha you need pinorder,
pinuse and function for allegro, and the pin names cannot be duplicated
unless they are listed separately as power. Look at the two very simple
attached examples.
Patrick Westfeldt, Jr.
720-406-0887
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Gary MacIndoe
Sent: Friday, May 05, 2006 9:43 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Importing orCAD schematics
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:
