I've looked at several forms/user guides/help documents and I'm unable to find the answers I'm looking for. I'm using orcad capture 16.2. I do *not* have CIS :'(
1. Is there a straightforward way to keep schematic compenonts off of the BOM. e.g. a PCB pad, fiducials, etc. EDIT: I'm aware there is a BOM_IGNORE property, but does this work on orcad captures BOM tool. Does it also affect the pcb editor properties? (BOM report,Component placement report...)
2. Is there a way to mark components as do not stuff so that when generating the BOM it will mark those components as such.
3. What is the preferred method for adding parts to the BOM that do not exist in the circuits but are part of the PCB assembly? e.g. heatsink. I read somewhere that making a library part with no pins is the way to go.
I'm looking for a way for the Bill of Materials tool to automate these for me. I want the BOM to output the "Item" "Qty" "Reference" "Part" and "Companies Part Number" fields such that I do not have to manually edit them whatsoever. Then I can add any other info from my own database such as RoHS status, description manufactures alternates etc.
BOM_IGNORE was not supported in the 16.2 release for the Capture BOMs, you can add and set a PSpiceOnly property to TRUE and these parts will make neither the netlist nor the BOM, otherwise you will need a user property and use this for later processing.
BOM Variants are supported by Capture CIS, otherwise you will need a user property to flag this and post process the BOM
You can add parts with no Pins for mechanical parts, these will make the BOM but not the netlist.
The Capture BOM is not going to automate this for you, you will need to make a BOM with all the properties and then post process that data for the final BOM.
In reply to oldmouldy:
Thanks for the answer mostly what I was looking for except.....
I can clearly see a "BOM_IGNORE" property in my property editor for parts. Are you certain it does nothing?
Also, if in case it does work, does it affect the Capture BOM , the PCB Editor Reports, or both.
I tried setting it to several different values (TRUE,1,YES, YEP) to see if anything would work and so far it looks like nothing. What are acceptable values? Didn't see that in the help documentation either...
In reply to cobcra:
Of course you can, that's in the Cadence-Allegro proerty filter and, if you set the value to TRUE and pass the netlist to PCB Editor, there is a chance that the PCB Editor BOM will respect it when it reports the BOM but it's not supported for the Capture BOM at 16.2. In 16.6, BOM_IGNORE set to TRUE does get the part with the property set removed from the Capture BOM.