Back Annotate from Allegro to bring in component location and board side using "pickdata" broken on 17.4

If you are using OrCAD schematic and OrCAD PCB (aka Allegro) then the "Layout" backannotation is the incorrect method despite your claim.  It has *always* been through the PCB Editor mode.  The Layout tab was there to support other tools only which have been removed.

All of your data can still be injected into your schematic if you use OrCAD schematic via PCB Editor backanno.  It just requires setting up the config file to import/export user defined properties.

Hi Red.

In the pcb editor the mirrored status of a symbol/footprint shows up under "Component Report", the header for the report shows "SYM_MIRROR" if the symbol is mirrored on the bottom side of the board.

How to get this Mirrored status back to the schematic so a BOM can be generated & show that mirrored status ?

You mentioned the Allegro.cfg file so testing a few things here I added SYM_MIRROR=YES to the [ComponentInstanceProps] section to see if BackAnno would work. This is probably the wrong method as I could not get it to work.

Any Clues on how to do it ?

BTW the bom out of Allegro is pretty good and have used this alot, more curious than anything on how to pass that SYM_MIRROR info back to capture. Not a got to have for me :)

Thanks..

The title of the column is "SYM_MIRROR" but that is not an actual component property.  You can only pass properties attached to components, nets, etc back to OrCAD.

So what to do?  

You can add a property to the component and pass it back  Call it SYM_MIRROR and pass it back.  I just did that and it works great.

You can write some SKILL code that digs down to the component property for mirrored side and then pass that back via an attached component property.

You can use the logic rename tool and add a character such as "T" or "B" to the component based on its placement side then that will tell you which side.

You can use the OrCAD property import tool and add it after adjusting the old SKILL tool file out there which I think you're using...

But out of curiosity, why do you need to do this?  I've been doing this my whole career and never had to separate these on the schematic side; just in the placement data. I did use to add 500 to the bottom components to quickly identify top from bottom but the BOM was always the same (all identical parts on the same line).   I'd like to learn why you do this and hopefully someone more experienced will chime in on an even better method.

Hi Red

So on this a couple of things. Over the years I have see this on BOM's sometimes called out as a line item header called "Location". The idea is so that at a glance a assy house can look at the BOM and see what side of the board components are on. This would be kind of a value add and is useful in particular for SMD builds that may have components on the bottom side of the board.

For rework techs it is also handy in conjunction with the schematic.

In Allegro/Orcad PCB Editor you can generate a BOM fairly easily that can include the "Mirror" info. No need to modify footprints/symbols to do this. This would be the method I use.

It seems to me that there should be an easier method to get this info back to the schematic. Doing Skill files or bit twiddling on Orcad Symbols just to generate a BOM out of capture is a bit of a heavy lift. It is kind of like this. When you purchase Capture it comes with a massive amount of symbols which is great. Though those symbols are pretty useless for a real design. The symbols do not contain attributes which are used so that Orcad Capture can generate a viable BOM. Things like MFR/PN, Manufacturer etc or basically any property that one would see on a typical BOM.

CIS does address and makes things a bit easier. I dunno if it is possible to convey the PCB Sym_Mirror info back to CIS.

As I mentioned earlier it's not a got to have for me. But I can see that if a company was actively structured so that their BOM's needed to have this info it may well present a road-block for them from the schematic generation level if they do indeed use the schematic to generate a viable BOM.

Thanks. 

I've worked here almost 10 years, we've always created BOMs that have the components grouped by internal part numbers but split by top and bottom, so for example part number 12345.1 has reference designators C1, C2, C3, C4 with a quantity of 4 on top and 12345.1 is on another line with ref des C5 and quantity of 1 for the bottom.  Our ERP system has top and bottom in separate machine steps so that's they only way we can do an automatic upload of BOMs from CSV into our system. Allegro doesn't output a grouped BOM that I'm aware of and with the changed back annotate option we lost the ability to use the skill file we were using to generate a swap file containing board side information. 

The property tool sounds like the easiest option out of those 3, I'll have to look into it.