Input Netlists

Owned by Bill OLeary
Last updated: Jan 19, 2022
3 min read

This section discusses the Input Netlist Formats and the CSETS that modify the behavior of NetBom when processing them.




BOM SpreadSheets

NetBom added support to read Generic BOM Spreadsheets In Version 21.12.1 

A BOM SpreadSheet can be compared to another BOM Spreadsheet, a Netlist, or an Orcad .DSN File

Allegro HDL (and Orcad) pstxnet.dat, pstxprt.dat and pstchips.dat files

When working with AllegroHDL Netlists, the Input files are usually contained in the design_top_level/worklib/packaged directories 

Until Version 19.7.1, NetBom only read the pstxnet.dat file to extract NetList data and the pstxprt.dat file to extract PartList (BOM) data

Starting in Version 19.7.1 NetBom is able to merge the part properties from the pstchips.dat file (where all the AllegroHDL Injected part properties are added on a per part basis). This enables a much more detailed comparison of part properties, and allows improved PartList generation since NetBom has access to more part properties (like Description, Mfg, Mfg PartNumber....)

In either case, the User only selects the pstxnet.dat file as the input Netlist and NetBom will locate the companion files

Orcad DSN Inputs

Version 19.8.1 of NetBom added the capability to directly read and compare Orcad DSN files

NetBom uses the installed Orcad tool's pstswp utility to convert the DSN file to the 3 Allegro NetList Files (pstxnet.dat, pstxprt.dat and pstchips.dat) so Its required that orcad is installed on the computer you are executing NetBom from.

Orcad DSN Specific CSETS

There is a special group of CSETS that tells orcad which properties to export from Capture to the Allegro NetList.

Use the search for config setting and enter 'D2N' in the match field to find them.

NetBom uses the CSETS to modify the Allegro.cfg file for the user (it copies the existing one and then makes the changes before running the pstswp utility)

The most important one is the ORCAD_D2N_ACFG_COMPDEF_LIST 

This is the CSET you will use to tell Orcad what component properties to copy to the resulting AllegroHDL Netlist files (and most of the properties will show up in the pstchips.dat file) 

Finding Orcad Properties to Transfer to Allegro


If the user does not know what Orcad Properties exist in the design, They can examine the existing Orcad DSN to determine which properties are available to transfer across. 


A powerful tool to examine the existing properties is the Orcad PartProperty Editor...

Select all the parts on a page, and use Ctrl-E to open the Parts Property Editor

Be sure that the Filter is set to Filter by: <Current properties> (which is not the default)

The Gui will show something like this where all the avialable properties for all selected parts can be seen:

Once  the user  has determined the available properties, they can add properties that they would like to use in the NetBom comparison to the ORCAD_D2N_ACFG_COMPDEF_LIST CSET,

Separating Each Property Name with a comma. 

For Example:

ORCAD_D2N_ACFG_COMPDEF_LIST=Manufacturer,Description,PWR,Current,DATASHEET,Manufacturer PN,PCB FootPrint,Fit Rate,DNI

Orcad Part Property Names Containing Spaces

NetBom will gracefully handle Property Names that contain spaces like "PCB Footprint".

The user should keep the spaces in the CSET. NetBom will tell Orcad to replace all spaces with an '_'.

If the user would like to use the Property in the NetBom comparisons (using the KEY_PROP_LIST CSET)  or Ignore the property using KEY_PROP_IGNORE_LIST, They will need to use the PropertyName with the '_'

Like: PCB_FootPrint,Fit_Rate

Illegal Orcad Property Values

The pstswp utility will fail if the Property Value contains an illegal character (for instance a space or NewLine at the end of the property) 

In this case, the user will either need to fix the Property Value in the design or they will have to remove that property from the ORCAD_D2N_ACFG_COMPDEF_LIST

CadEnhance has requested that Cadence provide a workaround for this issue, but the Error exists in 17.2-2016 S054 

EDIF Netlists

NetBom can read EDIF Netlists produced by Orcad, Mentor (Pads Professional, and Pads Logic) and Altium Tools 

Mentor nets.fwd, parts.fwd, pins.fwd

When working with Mentor DxDesigner NetLists, the nets.fwd,parts.fwd and pins.fwd files are read by NetBom

the User selects the nets.fwd file and NetBom automatically locates the other 2 companion files

KeyIn KYN Netlists

NetBom supports the KeyIn NetList Format, but they do not typically provide good property information to extend the value of the NetList/PartList comparison