Entering in a netlist after manual parts placement and routing

[davepcb]

Tom,
This forum is excellent. Thank you for all of your advice.
I have a similar problem as the guy that was trying to import a netlist after he manually made some connections in Pads.

My situation is that I had to manually place some parts and make some connections and then make routes (many differential) to and from an 896 pin BGA. The routes took a long time to do. Now I would like to import the netlist from Orcad and somehow not affect the hard work that I already did.

In summary, I placed a couple of parts from the PADS library, manually routed all of the differential signals then went back to the schematic and made the same connections there. I have to bring in a netlist but I think that it will wipe out all of the routes that I did already!

I'm not good at putting things in words.

Dave

[randychase]

I think you are right, that entering in the new netlist is a bad idea.

Your best bet is to output the netlist from the board and run a netcheck tool against it vs the one from Orcad. This will create an ECO file that you can read in and it will make *only* the changes.

You also can manually create the ECO file using the PowerPCB ASCII format.....or manually enter the changes. But use netcheck or netcomp to verify the netlists are compatible.

You can download the netcheck from http://www.cadprosystems.com and they offer a free 30 day trial.

[Tom]

Dave,

I have to agree with Randy that the best way to get a clean netlist into PowerPCB using OrCAD as your Schematic Tool is by using "Netcheck Tools" as a 3rd party ECO generator. This is how it works....

You can manually bring parts into a design using the ECO Tool box.
You can manually place the parts.
You can use the ECO Tool box (route ICON) to route traces (differential pairs in your case) to unconnected pins. This will create a netlist with net names like $$$1, $$$2, etc.
You can create a PowerPCB netlist using File/Report/PowerPCB V3.0 Netlist
You can Export the OrCAD Netlist using the PowerPCB V3 or V4 Netlister DLL file.
You can then compare the two netlists in Netcheck Tools and it will create an ECO file. When you File/Import the ECO file, it will modify the PowerPCB database to match the OrCAD netlist.
Netcheck Tools will perform the following features:
1. It will automatically rename your original PowerPCB netnames from $$$1, $$$2, etc. to the OrCAD netname.
2. It will Import any parts that you did not manually place.
It will update every decal to the decal name that is assigned in the OrCAD Symbol.
3. It will completely update the PowerPCB netlist, leaving the entire manual routing in place (if the two netlists match pin for pin).
4. It will delete any part that is in the design but not in the schematic. So if you put Mounting Holes to GND you have to add the Mounting Holes to your schematic. Fiducials will not be deleted because they are not a netlist item.
5. The great thing is that Netcheck Tools produces a Human Readable Report and an ECO file so you can check the differences prior to importing your netlist.
6. Netcheck Tools will retain the paths of both your netlists in the program so you can run the program over and over again within seconds.
7. It also works as a netlist translator so you can compare 25 different format netlists. Actually any netlist format in the world. Including FutureNet (can you believe that!). You can actually translate any netlist format to any other netlist format.
8. It also works as a netlist comparison tool for final netlist verification match.
We use Netcheck Tools every day, sometimes several times a day. It's a safe product that will not destroy the hard work that you manually performed.
When you contact CADPRO Systems - 858.695.9900 ask for the free 30 day Netcheck Tools evaluation. They will require an e-mail address to send you the download URL and the "Password" to turn on the 30-day trial. I like to test drive the product before I lay down the bucks.
Buy it once (there's no need for yearly maintenance, ours has worked forever) and use it a thousand times. That's a good ROI.