[SOLVED] Netlist repeats part name, making it longer than 31 character

[BusyEng]

Hi,

I am new to Orcad 16.6 (I have been using Orcad 10.5 before) and have difficulty with creating netlist for PCB Editor. I created a simple schematic with few components in it. None of the components' name are longer than 31 characters. However, when I generate netlist I get the following warnings:

#1 WARNING(ORCAP-36006): Part Name "PRINTEDCOIL_PRINTEDCOIL_PRINTEDCOIL" is renamed to "PRINTEDCOIL_PRINTEDCOIL_PRINTED".
#2 WARNING(ORCAP-36006): Part Name "5024300820_5024300820_5024300820" is renamed to "5024300820_5024300820_502430082".
#3 WARNING(ORCAP-36006): Part Name "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM_BT-SPK_L+" is renamed to "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM".
#4 WARNING(ORCAP-36006): Part Name "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM_BT-SPK_L-" is renamed to "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0_1".
#5 WARNING(ORCAP-36006): Part Name "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM_BT-SPK_R+" is renamed to "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0_2".
#6 WARNING(ORCAP-36006): Part Name "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM_BT-SPK_R-" is renamed to "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0_3".
#7 WARNING(ORCAP-36006): Part Name "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM_VBAT" is renamed to "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0_4".
#8 WARNING(ORCAP-36006): Part Name "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM_GND" is renamed to "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0_5".
#9 WARNING(ORCAP-3
6006): Part Name "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM_SW_COM" is renamed to "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0_6".
#10 WARNING(ORCAP-36006): Part Name "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0MM_MIC_GND" is renamed to "PAD_1P5MMX1P0MM_PAD_1P5MMX1P0_7".

For some reason, capture is concatenating each part name three times, making it longer than 31 character, and then truncates them. Because of this renaming, I cannot link the logic to the board (.brd file) as well. Please help as I am stuck here.

Thanks.

 

[SHIVABRS]

Hi,

You can change more than 31 Character just see the below and follow that

Shiva

 

[BusyEng]

I already tried that. For whatever reason, increasing the Name Char Limit has no effect!

 

[BusyEng]

Ok, I think I found a work around for this problem as below:

If you get the ORCAP-36006 warning when trying to generate netlist, you need to open a DOS command window, add the –l 255 switch to the netlist generator command (put it after the –v 3 command) and run it.

For example, if you get the following message in Capture after generating the netlist:

"C:\Cadence\Allegro16.6_InstallationFolder\tools\capture\pstswp.exe" -pst -d "D:\TEMP\SCHEMATICS\TEST2.DSN" -n "D:\TEMP\SCHEMATICS\allegro" -c "C:\Cadence\Allegro16.6_InstallationFolder\tools/capture/allegro.cfg" -v 3 -j "PCB Footprint" -hpath "HPathForCollision" –lite

Then you need to run the following command in the DOS command window:

"C:\Cadence\Allegro16.6_InstallationFolder\tools\capture\pstswp.exe" -pst -d "D:\TEMP\SCHEMATICS\TEST2.DSN" -n "D:\TEMP\SCHEMATICS\allegro" -c "C:\Cadence\Allegro16.6_InstallationFolder\tools/capture/allegro.cfg" -v 3 –l 255 -j "PCB Footprint" -hpath "HPathForCollision" -lite

After doing so, just go to PCB editor and import logic as usual. You are done.