Netlisting in 16.5

Not really, if you have a single license for PCB Editor. A license for PCB Editor will be taken if PCB Editor is running, you won't be able to start another PCB Editor session after the netlist is generated unless you have multiple licenses, equally, if you could open two copies of essentially the same board, it might be all too easy to edit the "wrong" one. Also, if the "input" board is open, PCB Editor won't be able to get past the "file lock" to change it.

The name of the input and output boards will be saved in Capture.

The previous "board revision" behaviour was great if that is what you wanted, a real pain if you didn't. You can enable versioning of items in PCB Editor from Setup>User Preferences, File_management, Versioning, ads_boardrevs controls the number of board revisions kept, the default is 1, you can increase this, set the "input" and "output" to be the same in Capture and PCB Editor will look after the file versions when the board re-opens.

Thanks OM. I wasn't looking at having two files open at once as that could become a real issue. I had a designer working for me a few years back that used to do that with 15.7 (I didn't know he was doing it that way) and it got us into a big mess when he renamed components and backannotated the wrong board. But that is a story for another day..........

Being a creature of habit (over 25 years of 16.2 and older use), when I come across something like this, I try to see if I can get it to function the way I'm used to doing it (ie, 16.2 and before). If I can't get it to work that way, then I "conform" and learn the new method. In this case there is no longer an "autoECO" feature like what I was used to in 16.2. So I will close PCB editor, generate the netlist and let Capture open editor back up.

As for the versioning, I'll dig through the info you provided and see what makes sense for me.

Thanks,

Tom

16.5 introduced file locking so if you editing a board in the PCB editor, the netlist process will report an error since that board is in use. 

While file locking can be disabled; it should be considered a good thing because it prevents the loss of edits.

 You can change your use model when you know an ECO is available from Capture either by:

1. Save your board, invoke an empty design so the lock is released and then open the original design after the Capture user completes the ECO update.
2. Have the Capture user export just the pst files. When it is convient do you can do File->Import->Logic to update your design.

I like option 2.

Thanks for the tips. The majority of the time, I am the Capture user and Editor user. I usually have Capture on one monitor and the PCB on another. I like being able to volley changes back and forth easily. With 16.5 being the new beast that it is, I just need to learn some new tricks.

Tom

PS: Go Phils!

Tom Perhaps this may be an easier way for you.

When your first cut of the schematic is ready to go, in the netlister enter your Imput board file, I usualy use a pre-caned Template with a board outline that has all the layers and colors configured.

Choose your output board name and this will be based on the above template. Run the netlister and package your board. By default I leave the capture option "Do not open Board file" checked as I open Allegro manually.

On your next pass of schematic changes Leave Allegro open but when you go to do the netlist change your input board to your output board name and leave the output board as it is. Check that "Do not open Board file" is enabled and then hit ok to create that updated netlist.

Pop over to allegro and select  File "Import Logic" in that window at the bottom choose your import directory to be where your board is packaged then click import logic.

This should update your board for you. From that point on you can go back to capture do a new netlist to update, pop back over to allegro and just hit import logic again to do the updates.

The above works good for me but it is not even close to being as streamlined as the older capture Layout combination. Reminds me of the old PCAD days : )

Thanks Scott.