> On Nov 22, 2019, at 12:42 PM, Brian <[email protected]> wrote:
>
>>> On 22 Nov 2019, at 19:29, Brian <[email protected]
>>> <mailto:[email protected]>> wrote:
>>>
>>> From the peanut gallery:
>>>
>>> Can someone tell me an example use-case for a single schematic symbol
>>> corresponding to multiple board entities within a single project?
>>>
>>> As perhaps a rather naïve PCB designer, it seems like mostly a bad idea to
>>> me to have anything other than 1:1.
>>>
>>> Thanks,
>>> -Brian Henning
>> On 11/22/19 2:37 PM, Jeff Young wrote:
>>> Hi Brian,
>>>
>>> Imagine you’re doing an audio amplifier. Your main schematic sheet has 4
>>> subsheets: PSU, control logic, left channel and right channel. Both left
>>> channel and right channel point to the same sub-page. So there’s a single
>>> schematic symbol for each part in the left & right channel, which gets
>>> annotated as two different references (ie: Q101 and Q201), and attached to
>>> two different footprints.
>>>
>>> Cheers,
>>> Jeff.
>>>
> Hi Jeff,
>
> Thanks for helping me understand this. So how would someone looking at the
> schematic know that this one symbol represents both Q101 and Q201? For that
> matter, if there's some instructions or a tutorial about creating a situation
> like this (one schematic drawing representing multiple instances of the
> subcircuit on the pcb), I'd be interested to learn it. I have a couple
> projects in the pipeline where I might find this feature useful; in the past,
> I've manually copy/pasted sections of a schematic to repeat subcircuits.
>
> Thanks,
> -Brian
When I first read Brian H’s message, “multiple board entities” stood out — I
thought he was talking about having more than one physical PCB in the project!
Now I understand his concern.
Brian — when you have a design which uses multiple instantiations of the same
sub-sheet, when you look at that design in the schematic editor (are we still
calling it EESChema?) you can navigate through the sub-sheets using the
Hierarchical Navigator. In each instance of a sub-sheet, you will see that each
component has been assigned unique reference designators.
So do a simple test. Create a project. In the project’s main sheet, choose
Create Hierarchical sheet from the right-hand menu. Give it a reasonable file
name (like subsheet.sch) and give it a reasonable Sheet Name. (Sheet name is
basically a reference designator for a sub-sheet.) Enter that sheet, add some
parts. keep it simple, like a single inverting op-amp circuit, so an op-amp
symbol and two resistors. Add two power symbols for the op-amp power. Add
hierarchical labels for the input and output. Don’t worry about annotation yet.
Save the sheet.
Navigate back to the top. Right-click on the sub-sheet symbol and choose
“Import sheet pins.” You need to do this once for each hierarchical label you
added. This is how you bring nets up to a higher level. Now select that
sub-sheet symbol by left-clicking/holding and drawing a rectangle around it.
Right-click and choose “duplicate block.” Now you have a new instance of that
same sub-sheet. Place it. Then right-click on it, choose “Edit …” (or just hit
E) and give it a better sheet name. Now you have two unique instances of that
sub-sheet. Choose Tools -> Annotate Schematic. When that’s done, enter each of
the sub-sheets — you will see that they each have unique reference designators
for the same symbols. Also, the non-hierarchical (local) nets in each sub-sheet
will have unique net labels! So when you export the netlist for PCB it’ll work
as you expect.
Oh, yeah, when you print out the schematic, you will get as many sheets as you
have instances of the sub-sheets. So the simple example here, with a top-level
sheet and two instances of a single sub-sheet will give you three printed pages.
Try it!
-a
_______________________________________________
Mailing list: https://launchpad.net/~kicad-developers
Post to : [email protected]
Unsubscribe : https://launchpad.net/~kicad-developers
More help : https://help.launchpad.net/ListHelp
