-
Is there a truly integrated schematic and board design package?
Posted by Agent86 on 31 Jan, 2017 00:28 -
Is there an EDA package that combines both schematic and board on the screen at the same time?
Traditionally, we capture the schematic first, then do some manipulation to convert it to a board. With packages like KiCad and gEDA, if you want to change something about the design, you start from the beginning of the pipeline, edit the schematic, then update the board after the modification. With a package like EAGLE, there is an annotation connection, so you can change some things in the board and they will propagate back to the schematic, as long as you have both schematic and board open at the same time.
Seems as it might be a good thing to really embrace the idea and have both schematic and board open at the same time, all the time, and have all changes anywhere propagate throughout both schematic and board.
Am I missing something? -
Probably not what you meant, but meets the word of your question:
Altium's work area can be split into multiple windows (or windows dragged off into a new main window), so you can work on the schematic and PCB at the same time.
Object highlighting (select part on SCH, highlight footprint on PCB; but not the other way around) is nice, but properties aren't updated until you send the ECO ("update changes"). Also, the info panels swap activity in a somewhat ponderous manner when alternating focus between SCH and PCB, which slows things down.
There are probably desirable reasons to keep things neat and ECO'd -- like if corporate procedure requires change logs throughout the design process. And it's not at all uncommon for the SCH and PCB designers to be completely different people with little overlap, and only little back-annotation or changes requested; an instant sync (which could be enabled via network connectivity, give or take ping!) could be absolutely irritating.
I would imagine it not being terribly hard to keep things instantly in sync (perhaps a script could even implement this in most EDA systems?), but it may be more burden than help. Often you'll make considerable changes in the schematic, and they'll resolve themselves on the PCB without trouble; or, other times, you'll have broken links between SCH symbols and PCB footprints, and everything ends up discombobulated (a problem which could've been alleviated with incremental updates -- if you had remembered/considered to update the PCB as you went, maybe the carnage wouldn't have been so bad? But you were really concentrated on those changes!).
So I don't know offhand if there are any that are real-time synced, but there may be. A lot do it through some sort of ECO process, which ranges from horrible (e.g., obscure and irritating workflows like OrCAD + PADS) to relatively painless (as with Altium).
Tim -
I used diptrace for the first time a few weeks ago and the extra two (or is it three) clicks to import the schematic changes into the board didn't bother me.
If nothing else it made me stop and think If I am really done and ready to change the board after making changes to the schematic.
What changes do you make to the board that you expect to make it back into the schematic ?
Ot to put it another way, why would you want the PCB layout person to screw around with your schematic?
-
Is there an EDA package that combines both schematic and board on the screen at the same time?
PCB Elegance has a schematic and layout editor that can talk to each other. Turn on active schematic select and the components selected on the schematic are also selected on the PCB. It makes it easy to group the PCB geometries (footprints) when starting a layout for the first time. You can also change the change the geometries in the layout editor and send the changes back to the schematic. It doesn't have a way to automatically highlight the nets like the probe (?) feature of Eagle though.
Actually, I think quite a few PCB packages have similar features, just look around. I know Altium can do this properly. -
What changes do you make to the board that you expect to make it back into the schematic ?
Or to put it another way, why would you want the PCB layout person to screw around with your schematic?- Say I have a quad opamp. I randomly choose one of the four for my design. When I work on the board, I realize that I should have chosen one on the *other* side of the chip. I can go back to the schematic and swap gates, but why not just let me do it on the board?
- I scan one of my old home-etched pcbs and show it in the background of my board editor. Then I start placing components and tracing the traces, building the schematic as I go.
- Say I'm working on my new Gizmotronic 9000 and I realize that I need to split the pcb to fit in the case that I decided to use. I think it would be easier to group the physical parts on the board and move them, rather than try to figure out where everything is on the schematic.
-
Say I have a quad opamp. I randomly choose one of the four for my design. When I work on the board, I realize that I should have chosen one on the *other* side of the chip. I can go back to the schematic and swap gates, but why not just let me do it on the board?
Many packages do gate and pin swapping. Though the setup can be awkward. (Altium has a swapping editor in the SCH Library view, that's kind of tedious.) Swaps usually show up in the back-annotation ECO, and can be implemented without too much trouble, though sometimes it will just give up (Altium tends to be useless with SCH updates in general; Multisim-Ultiboard can miss linked components and, since it /does/ know how to resolve schematic import, actually: it can throw in all the parts you were missing, and do you the favor of deleting the old parts that clearly aren't placed correctly!
).QuoteI scan one of my old home-etched pcbs and show it in the background of my board editor. Then I start placing components and tracing the traces, building the schematic as I go.
Most packages have the means for PCB drawing only, though it's not always useful. I think the old Traxmaker was good for that? Doing it in Altium is annoying, because editing nets is tedious. You'd probably want to trace the schematic first, and then reconstruct the PCB.
It's not a common use-case, I think. Similar problems can arise with gerber import, though -- often the nets don't work at all, or *everything* gets netted, including no-net shapes and NC pads.QuoteSay I'm working on my new Gizmotronic 9000 and I realize that I need to split the pcb to fit in the case that I decided to use. I think it would be easier to group the physical parts on the board and move them, rather than try to figure out where everything is on the schematic.
This might be easier in some packages -- Altium supports rigid/flex board construction, and can even show you how a flex assembly bends up in 3D, if you're using it for an assembly like that.
Most times, completely splitting a board (adding connectors to pass nets between, and all that) is an early design step, and a huge oversight to realize later in the build. But if you need to do it, it's probably going to be a pain no matter how (and in what) you do it.
Tim -
I used diptrace for the first time a few weeks ago and the extra two (or is it three) clicks to import the schematic changes into the board didn't bother me.
If nothing else it made me stop and think If I am really done and ready to change the board after making changes to the schematic.
What changes do you make to the board that you expect to make it back into the schematic ?
Ot to put it another way, why would you want the PCB layout person to screw around with your schematic?
DipTrace can backport changes from PCB to Schematic. Also, there's a default hotkey for renewing your PCB for a related schematic (Shift-Alt-K I think; it tells you in the menu). -
Most software can back annotate PCB changes to the schematic, but would you always want it to do that automatically?
It's not unheard of for someone to make errors, have little accidents in the pcb, such as deleting components, nets etc. that are still selected while also deleting something else
and then just clicking through the confirmation screens.
Auto updating then makes it so that the scm is the same as the PCB - accidental errors included.
However, if back or forward annotation is actually a task that requires user interaction then they can see and confirm if something untoward has happened.
Me - I prefer to have to click a couple of times while I confirm an ECO update than have the pcb auto updated to the schematic.
Matt.