How to repeat the same pattern

Discussion:

Barita Ken

2013-12-06 00:56:54 UTC

I am writing a PCB in which the same pattern is repeated many times.
On EESchema, it is possible to copy/paste the same pattern, but on PCB editor
do I have to allocate the parts each time I put the same pattern?
It is always the same thing and it is uneffcetive to allocate each time.
Even if I copy/paste the pattern, the netlist is connected between the original
and pasted parts.

Is it possible to copy/paste the same pattern effectively?

Arita

c***@public.gmane.org

2013-12-06 09:27:31 UTC

Permalink

----Origineel Bericht----
Van : knbarita-/***@public.gmane.org
Datum : 06/12/2013 01:56
Aan : kicad-users-***@public.gmane.org
Onderwerp : [kicad-users] How to repeat the same pattern

I am writing a PCB in which the same pattern is repeated many times.
On EESchema, it is possible to copy/paste the same pattern, but on PCB editor
do I have to allocate the parts each time I put the same pattern?
It is always the same thing and it is uneffcetive to allocate each time.
Even if I copy/paste the pattern, the netlist is connected between the original
and pasted parts.
Is it possible to copy/paste the same pattern effectively?
Arita

I'm sorry Arita, I have no knowledge of it.
But it would be an awesome feature. I would like to see that you can select a section of your board (complete with components), and then choose copy, paste and annotate. Then for instance have an option to add 10, 100 or 1000 to the original designators. This could then generate new designators and nets. Next, back annotate to the schematic, by using unique identifiers (timestamps?) In the schematic, place the new components next to the schematic, spaced and connected with airwires. Maybe this requires a new flag especially for copy-and-repeat jobs.
Best regards,
Cedric

Bernd Wiebus

2013-12-06 10:14:03 UTC

Permalink

Hello Arita.

Post by Barita Ken
do I have to allocate the parts each time I put the same pattern?
It is always the same thing and it is uneffcetive to allocate each
time.
Is it possible to copy/paste the same pattern effectively?

Yes. Not perfect, but better you do actually.

I assume, you have a correct schematic, which repeats this pattern
already.

Now copy the .brd or .kicad_pcb file and rename it to newboard.
Open the file with pcbnew and delete all objekts with the exception of
the parts and copper pattern you want to use.Then move the residuum to a
corner, were you will get no conflict, if you merge this ne board into
your original one.
Copy this file again and rename it, until you have it so m

Open your original board, and use file > append board to import the new
pcb.

Rename the components syncron to your schematic, and save the board.
The changed board will be in a file newboard-append.kicad_pcb

Again append the newboard . Do NOT mix it up with a file generated by
kicad: newboard-append.kicad_pcb. It is the board you allready merged.

Rename the components syncron to your schematic, and save the board.
Again, The changed board now with to patterns is
newboard-append.kicad_pcb

Do this so often, until you satisfy all your repeated pattern instances.

However, the most work will be renaming and fitting this patterns into
the board.

Alternatively, you can copy and rename the partial pattern pcb so many
times as you use it, rename the components one for one, and append the
single boards one after another into your original board.

With best regards: Bernd Wiebus alias dl1eic

Post by Barita Ken
I am writing a PCB in which the same pattern is repeated many times.
On EESchema, it is possible to copy/paste the same pattern, but on PCB editor
do I have to allocate the parts each time I put the same pattern?
It is always the same thing and it is uneffcetive to allocate each
time.
Even if I copy/paste the pattern, the netlist is connected between the original
and pasted parts.
Is it possible to copy/paste the same pattern effectively?
Arita

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

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://info.yahoo.com/legal/us/yahoo/utos/terms/

Bernd Wiebus

2013-12-06 12:06:27 UTC

Permalink

Post by Bernd Wiebus
Rename the components syncron to your schematic, and save the board.
Again, The changed board now with to patterns is
newboard-append.kicad_pcb

And, of course, remove the old components with the same names. You got
them at the beginning, when you readed the netlist.

And don't forget to reread the netlist. First being carefull and keeping
components.

With best regards: Bernd Wiebus alias dl1eic

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

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://info.yahoo.com/legal/us/yahoo/utos/terms/

Erik Lane

2013-12-14 01:37:20 UTC

Permalink

You can also let your computer do it for you. It took me a while playing
with this before I got it to do just exactly what I wanted, but once you
get it all sorted out, it's like magic!

http://blog.borg.ch/?p=12

Post by Bernd Wiebus

Post by Bernd Wiebus
Rename the components syncron to your schematic, and save the board.
Again, The changed board now with to patterns is
newboard-append.kicad_pcb

Bernd Wiebus

2013-12-14 13:31:22 UTC

Permalink

Hello Erik.

You can also let your computer do it for you. It took me a while playing
with this before I got it to do just exactly what I wanted, but once you
get it all sorted out, it's like magic!

Post by Erik Lane
http://blog.borg.ch/?p=12

Thank you for this tip!

panelize.py is great. But it is for panelizing, which means the same
board repeated on a much greater board just for production. Usually,
these repeated boards have NO electrical connections, if they are ready,
because they are actually different boards, despite they are all equal.

But i think the treatstarter thinks about using the same pattern of
copper on one board, like, as an example, different channels, which are
equal/similar and usually somehow electrically connected to other parts
of the boart, when it is ready, because they are just a part of a bigger
circuitery.

Whith best regards: Bernd Wiebus alias dl1eic

Post by Erik Lane
You can also let your computer do it for you. It took me a while
playing with this before I got it to do just exactly what I wanted,
but once you get it all sorted out, it's like magic!
http://blog.borg.ch/?p=12

Post by Bernd Wiebus
Rename the components syncron to your schematic, and save

the board.

Post by Bernd Wiebus
Again, The changed board now with to patterns is
newboard-append.kicad_pcb

Erik Lane

2013-12-14 23:48:40 UTC

Permalink

Post by Erik Lane
You can also let your computer do it for you. It took me a while playing
with this before I got it to do just exactly what I wanted, but once you
get it all sorted out, it's like magic!

Post by Erik Lane
http://blog.borg.ch/?p=12

Thank you for this tip!
panelize.py is great. But it is for panelizing, which means the same
board repeated on a much greater board just for production. Usually,
these repeated boards have NO electrical connections, if they are ready,
because they are actually different boards, despite they are all equal.
But i think the treatstarter thinks about using the same pattern of
copper on one board, like, as an example, different channels, which are
equal/similar and usually somehow electrically connected to other parts
of the boart, when it is ready, because they are just a part of a bigger
circuitery.
Whith best regards: Bernd Wiebus alias dl1eic

That's not what it sounded like to me. It sounded like the original poster
was complaining that the different netlists were still connected to each
other when they did the copy and paste. It sounded to me like panelize is
what they actually wanted.

But no, if you understood Arita correctly and I did not then panelize
wouldn't work as well for them. You can still edit the nets by hand in the
board file, but that's a pain, especially with a file that big. It doesn't
take too much to do a global find/replace in the file, but you need to do a
bit of digging to find all the relevant lines and make sure you understand
what you're doing.

Thanks,
Erik

k***@public.gmane.org

2013-12-17 16:39:39 UTC

Permalink

Hello.

This is Arita. I am now struggling.

I could insert the pattern by following the way Bernd told me.

I have some questions.

1. If I follow the Bernd's instruction, do I have to change the parts name of the
inserted circuit manually one by one?
2. Even after insertion of the repeated pattern, there still are some thin white lines (rats nest)
that connects the parts between the repeated pattern.

In the original EeSchema circuit, there are not such links. Is it possible to remove them?

3. Can I manually draw lines to connect the parts that are not connected by a thin white line?
I mean is it possible to use the panelize.py and manually connect between them?

Thank you.
Arita

Bernd Wiebus

2013-12-18 07:25:28 UTC

Permalink

Hello Arita.

Post by k***@public.gmane.org
1. If I follow the Bernd's instruction, do I have to change the parts
name of the inserted circuit manually one by one?

Yes. Because after inserting, you will have the parts with the original
names from the original netlist, AND the parts with the names they got
bevore inserting, and this, perhaps, multiple times.
So you have to rename the inserted parts, and to delete the original
parts, to avoid double names, and than rereading the netlist for getting
the right connections..

This may also explain, why it might be preferreable to insert just one
board, rename and delete parts, and then insert the next. You are not so
prone to get confused.

Renaming and deleting is much work to do. Perhabs it might be nice to
have a python skript to do it in a spreadsheet and check for double or
missing parts.

Post by k***@public.gmane.org
2. Even after insertion of the repeated pattern, there still are some
thin white lines (rats nest) that connects the parts between the
repeated pattern.

This is, because you inserted a copper pattern and parts. PCBnew can
link the copper pattern and the parts, but the connection between this
inserted and your existing pattern have done by yourself. Where PCBnew
shall got this information? It is not in your existing board, it is not
in the inserted board, and there is only a hint from the netlist, that
they should be there.
So you have to do it by your own.

Post by k***@public.gmane.org
In the original EeSchema circuit, there are not such links. Is it possible to remove them?

Then i think, there may be double names some where. Your forgot renaming
or forgot deleting some parts.

You will have to reread the Netlist after inserting the board.

Post by k***@public.gmane.org
3. Can I manually draw lines to connect the parts that are not
connected by a thin white line?

After renaming, deleting and rereading the Netlist (and making no
mistakes) there should be white lines (airwires), if there is a
connection in Eeschema. If not, you should make this connection at
Eeschema, export the netlist, and reread them into PCBnew.
Of course, you can simply draw copper at PCBnew, without making the
connections at Eeschema. But than you will run into trouble, if you
somehow need to reread the netlist (because you changed the schematic),
or when you want to make a DRC.

Post by k***@public.gmane.org
I mean is it possible to use the panelize.py and manually connect between them?

I don't investigated in the depth, but i think panelize.py is just what
inserting (appending) a board also does, but much comfortable in a
predefinet pattern for making big repeated structures for production.
So you can use it, too.

But the work with renaming, deleting and rereading the netlist will be
just the same.

With best regards: Bernd Wiebus alias dl1eic

Post by k***@public.gmane.org
Hello.
This is Arita. I am now struggling.
I could insert the pattern by following the way Bernd told me.
I have some questions.
1. If I follow the Bernd's instruction, do I have to change the parts name of the
inserted circuit manually one by one?
2. Even after insertion of the repeated pattern, there still are some
thin white lines (rats nest)
that connects the parts between the repeated pattern.
In the original EeSchema circuit, there are not such links. Is it possible to remove them?
3. Can I manually draw lines to connect the parts that are not
connected by a thin white line?
I mean is it possible to use the panelize.py and manually connect between them?
Thank you.
Arita