Orcad to PCB Editor error during Create Netlist

error 102 netlist import

I obtain the following session log error when i tried to create netlist from Orcad Capture to be used by PCB Editor for layout. i don't know what error,who can tell what problem in my project.
CmdLine: netrev.exe -5 -y 1 -i e:\source-work\bcm97455mb_v10\allegro E:\SOURCE-WORK\BCM97455MB_V10\200-115745-0000Gp1.brd C:\Documents and Settings\lance ying\桌面\qq.brd

------ Preparing to read pst files ------

Starting to read e:/source-work/bcm97455mb_v10/allegro/pstchip.dat
Finished reading e:/source-work/bcm97455mb_v10/allegro/pstchip.dat (00:00:00.20)
Starting to read e:/source-work/bcm97455mb_v10/allegro/pstxprt.dat
Finished reading e:/source-work/bcm97455mb_v10/allegro/pstxprt.dat (00:00:00.39)
Starting to read e:/source-work/bcm97455mb_v10/allegro/pstxnet.dat
Finished reading e:/source-work/bcm97455mb_v10/allegro/pstxnet.dat (00:00:00.42)

------ Oversights/Warnings/Errors ------


WARNING: U4101 component device pin number mismatch; cannot replace.

#1 ERROR(302) Device library error detected.

Error with pin number 'AC16' in device 'BCM7401B0_1_BGA676_35X35_050_SK': 'Unable to find pinname in adfncpin.'.

#2 ERROR(302) Device library error detected.

Problems building functions in device 'BCM7401B0_1_BGA676_35X35_050_SK': 'Unable to find pinname in adfncpin.'.

Device 'BCM7401B0_1_BGA676_35X35_050_SK' has library errors. Unable to transfer to Allegro.

WARNING: J2608 component device pin number mismatch; cannot replace.

------ Summary Statistics ------


#3 ERROR(102) Run stopped because errors were detected

netrev run on Dec 24 21:15:56 2007
DESIGN NAME : 'BCM97455MBV10_XX'
PACKAGING ON Jun 17 2005 00:56:10


thank everybody!

adfncpin

your selected footprints are not accurate

recheck them

unable to find pin name in adfncpin

now ,i rebuild my pcb package symbol,and try again.the error is not change.
i don't know why.who can tell me? thank you!!

error 102 allegro

Are you sure about the integrity of the component library symbol, it seems that error refers to the library symbol of the component

generate orcad netlist pcb editor

check ur schematics,if the symbol dont have AC16 pin ,its possible to get the errors while importing.
again the error shows,chek ur library....

orcad error netlist

tahnk everybody,i have know what happed.because in my sch,pin name is to long, cadance is not support.now it is OK. thank !

how to perform netlist check in orcad capture

The schematic Symbol (Orcad Symbol) pin has two properties, one PIN_NAME and another PIN_NUMBER. You might have ended up giving only the PIN_NUMBER property on the schematic symbol and not the PIN_NAME. In your case, the pin number would have been, I guess, AC16 and the PIN_NAME is missing. You can right click on the schematic symbol ---> Edit Part ---> Double Click on AC16 pin and check if the PIN_NUMBER and PIN_NAME property value strings are added. Adding PIN_NAME property value should solve this problem.

In case that does not solve, go the project menu tree. Select the .dsn file. Go to the tool bar and do a CLEAR CACHE and package the schematic and then generate the netlist and try importing it into Allegro.

Also I noticed that the folder name from which you were trying to import the netlist had spaces in between words. Try replacing the spaces with an underscore "_" or hyphen "-".