Orcad to PCB Editor error during Create Netlist

[yzb1658]

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!

 

[ehsanelahimirza]

adfncpin

your selected footprints are not accurate

recheck them

 

[yzb1658]

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!!

 

[raminzk]

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

 

[ansari6682]

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....

 

[yzb1658]

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 !

 

[pvskt]

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 "-".