3 PCBs, 1 design

Discussion:

3 PCBs, 1 design

jimofc300

2010-05-10 05:22:47 UTC

Hi,

Still new to KiCAD.

I hope there's a simple solution to my rather simple problem, since it must be very common. I haven't been able to find one in the docs or by poking at KiCAD. Can someone help?

I have a design that will have three PCBs within a lot of other hand wiring, such as switches, panel connectors, a power module, and so on. I've created a hierarchical schematic that leads to each eventual PCB as a separate schematic sheet. I want to convert each of these three schematics to PCBs, one-by-one. KiCAD, however, seems to think that I want a PCB of the entire mess, not just the single sheet schematic. It compains that component numbers haven't been assigned to the higher items in the hierarchy (they haven't).

So far, all I've figured out is to copy the schematic to another file and make a PCB from it. While this works, it's sloppy and automatic back-annotation seems impossble.

Is there any way to force KiCAD to make a PCB of a single schematic sheet, even when buried within a larger hierarchical design?

Thanks,
Jim

------------------------------------

Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/kicad-users/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/kicad-users/join
(Yahoo! ID required)

<*> To change settings via email:
kicad-users-digest-***@public.gmane.org
kicad-users-fullfeatured-***@public.gmane.org

<*> To unsubscribe from this group, send an email to:
kicad-users-unsubscribe-***@public.gmane.org

<*> Your use of Yahoo! Groups is subject to:
http://docs.yahoo.com/info/terms/

Cat C

2010-05-10 14:45:03 UTC

Permalink

You might want to have connectors for wires/cables between those boards.

So if the schematics show connectors instead of connections you might get what you want.

Even if you won't populate connectors, you can still put some headers where you'll solder the wires.

Cat

Date: Mon, 10 May 2010 05:22:47 +0000
Subject: [kicad-users] 3 PCBs, 1 design
Hi,
Still new to KiCAD.
I hope there's a simple solution to my rather simple problem, since it must be very common. I haven't been able to find one in the docs or by poking at KiCAD. Can someone help?
I have a design that will have three PCBs within a lot of other hand wiring, such as switches, panel connectors, a power module, and so on. I've created a hierarchical schematic that leads to each eventual PCB as a separate schematic sheet. I want to convert each of these three schematics to PCBs, one-by-one. KiCAD, however, seems to think that I want a PCB of the entire mess, not just the single sheet schematic. It compains that component numbers haven't been assigned to the higher items in the hierarchy (they haven't).
So far, all I've figured out is to copy the schematic to another file and make a PCB from it. While this works, it's sloppy and automatic back-annotation seems impossble.
Is there any way to force KiCAD to make a PCB of a single schematic sheet, even when buried within a larger hierarchical design?
Thanks,
Jim
------------------------------------
Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links

Lorenzo

2010-05-12 12:59:25 UTC

Permalink

Post by jimofc300
Is there any way to force KiCAD to make a PCB of a single schematic sheet, even when buried within a larger hierarchical design?

I had a similar issue with a sandwitch-board (i.e. two pcb mounted with risers).

The trick is to use a single pcb file with all your boards drawn into it and declare the joining points (connectors, risers, whatever) as modules (like the CONN_ parts). Of course you have to manage manually the pinouts of these connectors to make them match!

It is actually easier to build them later since you only have to submit *one* gerber/PnP set instead of three! You could also ask the manufacturer about how he would like the board aligned to ease panelisation and where to put scoring/rat-bites indications (but, anyway, they will have no trouble separating three boards from the same gerber set).

------------------------------------

Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/kicad-users/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/kicad-users/join
(Yahoo! ID required)

<*> To change settings via email:
kicad-users-digest-***@public.gmane.org
kicad-users-fullfeatured-***@public.gmane.org

<*> To unsubscribe from this group, send an email to:
kicad-users-unsubscribe-***@public.gmane.org

<*> Your use of Yahoo! Groups is subject to:
http://docs.yahoo.com/info/terms/

andrewdwork

2010-08-02 08:06:40 UTC

Permalink

Hi Jim,

I am struggling with hierarchical schematics too, but the idea is to make a single board from many sub-sheets, not seperate PCBs from each sub-sheet.

Suppose you were building an audio amplifier.

Maybe the circuit is complex and to make it more readable you would break it into sections such as PSU, pre-amp, power amp, protection circuit etc.

The final result will still be one PCB.

If, say, the the front panel was a seperate PCB, you would still have to do a seperate circuit.

You could use hierarchical schematic for the overview of the unit, but not for the individual PCBs, as I understand it anyway.

My problem is trying to resolve ERC errors with power flags / Global labels, but that's another story.

Post by jimofc300
Hi,
Still new to KiCAD.
I hope there's a simple solution to my rather simple problem, since it must be very common. I haven't been able to find one in the docs or by poking at KiCAD. Can someone help?
I have a design that will have three PCBs within a lot of other hand wiring, such as switches, panel connectors, a power module, and so on. I've created a hierarchical schematic that leads to each eventual PCB as a separate schematic sheet. I want to convert each of these three schematics to PCBs, one-by-one. KiCAD, however, seems to think that I want a PCB of the entire mess, not just the single sheet schematic. It compains that component numbers haven't been assigned to the higher items in the hierarchy (they haven't).
So far, all I've figured out is to copy the schematic to another file and make a PCB from it. While this works, it's sloppy and automatic back-annotation seems impossble.
Is there any way to force KiCAD to make a PCB of a single schematic sheet, even when buried within a larger hierarchical design?
Thanks,
Jim

------------------------------------

Please read the Kicad FAQ in the group files section before posting your question.
Please post your bug reports here. They will be picked up by the creator of Kicad.
Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library.
For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/kicad-users/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/kicad-users/join
(Yahoo! ID required)

<*> To change settings via email:
kicad-users-digest-***@public.gmane.org
kicad-users-fullfeatured-***@public.gmane.org

<*> To unsubscribe from this group, send an email to:
kicad-users-unsubscribe-***@public.gmane.org

<*> Your use of Yahoo! Groups is subject to:
http://docs.yahoo.com/info/terms/

Andy Eskelson

2010-08-02 12:36:33 UTC

Permalink

The hierarchical circuit system is there to help you split up a circuit
into manageable sections. it is NOT a method to make separate PCBs as
such.

It is possible to make separate PCBs, but you will have to be
careful regarding interconnections, and you would have to accept that.
ALL the PCB's would be produced at once initially. You will also have to
do some manual adjustments as well.

If your design uses several PCBs DO NOT interconnect them on the circuit.

Terminate the interconnection points as connectors or pins of whatever.
This will keep each circuit module isolated.

You can then continue with PCBnew in the normal way, When you place the
components you will find that each circuit module will be isolated from
the next. You can define several board outlines and place the components
on them, (this can be tedious if the design uses many components)

You may have to accept a few DRC type errors if the power arrangements
get a bit messy. Once you have done with the layout you can then either
plot all at once, or delete the unwanted layouts and just print the one
that is left.

Another option that I have seen suggested, is that you can open the sub
sheet as a separate project and work on that, but that can cause it's own
issues. (I've never tried this)

A better method and the one that I prefer is to
treat each PCB as it's own design, and then the problems generally go
away. i.e. in a project I will have a PSU circuit, a processor circuit, a
relay driver circuit and so on. Each with their own netlists, PCBnew
files and so on. So the general rule is, if the final result is to be one
PCB, then everything goes into one circuit, using sub sheets as required.

If the end result is several different PCB's, then each PCB should have
it's own circuit. (Which is what andrew suggests below)

Power flags are not that hard once the penny drops.

In the case of a design with an external power unit....

The circuit will only have a connector or a pin where the power will come
into the circuit. It will NOT have any on board power. So in order for
the ERC to work, you have to tell the system that a particular line is
providing power. That is the function of a power flag.

So if you have a design that needs 5V to power it, you would have a
ground and 5V pin somewhere on it. Usually at this point on the circuit
you would place a couple of power flags. One on the 5V pin and one on the
ground pin. Then the ERC will be happy. (It seems a bit odd at first, but
ground or 0V is treated as a POWER IN type pin)

Of course there are gotchas that can trip you up. The ERC does it's
checks by looking at the pin types on the various parts. For power it
looks at pin types of POWER IN and POWER OUT. It's quite simple, in that
every power IN must be connected to a POWER OUT somewhere. So on most
devices say a 7400 chip, there will be a 0V and +5V on the part, and
these will be defined as POWER IN types. You have to connect these to a
POWER OUT source. A power flag is effectively creates a POWER OUT
device.

Some devices can have a pin defined as a POWER OUT. Typically this is on
regulators such as a 78xx types, where the output pin is often defined as
a POWER OUT type. In this case you don't need the power flag on that
line, if you add one it will confuse things.

Andy

On Mon, 02 Aug 2010 08:06:40 -0000

Post by andrewdwork
Hi Jim,
I am struggling with hierarchical schematics too, but the idea is to make a single board from many sub-sheets, not seperate PCBs from each sub-sheet.
Suppose you were building an audio amplifier.
Maybe the circuit is complex and to make it more readable you would break it into sections such as PSU, pre-amp, power amp, protection circuit etc.
The final result will still be one PCB.
If, say, the the front panel was a seperate PCB, you would still have to do a seperate circuit.
You could use hierarchical schematic for the overview of the unit, but not for the individual PCBs, as I understand it anyway.
My problem is trying to resolve ERC errors with power flags / Global labels, but that's another story.