Re: Jumpers and zero-ohm resistors

开云体育

Bernd,

Thank you to point this aspect. I didn't even think to the fuse.
I save your message it will probably be helpful in the future.

Just one question (it makes a while I didn't design a board) : for example 0-Ohm resistor with a power Input connected to gnd power line and a power output with a power flag connected to the Gnd pin of the IC. Shouldn't there be a net name conflict with the IC gnd and the resistor's output ? And, with a fuse and the same rationale, wouldn't the ERC cry a bit ?

Regards

On 21.09.24 21:05, Bernd Wiebus via groups.io wrote:

Show quoted text

-----BEGIN PGP SIGNED MESSAGE-----
Hash: SHA512

Hello Pierre-Raymond

Mandatory for power lines.

Same Problem as for fuses. It is not the problem, that you use two nets
(numbers will be enough) but for the ERC-Testing, because you end a
power line, and the other end of the device is no power line. So the
ERC-Test will throw errormessages.

Cure for this seems for zero ohm resistors the same as for fuses:
Define one pin as power input, so you can connect it to a symbol
with power flag, and the outher as power output, so you can
connect it to passive pins. Then the ERC will be satisfied.

Of course, as for small designs, you can easyly ignore the error
messages, as far as you not get confused with real errors.

Be aware, there sometimes is a confusion with names. The pin, where
the fuse or zero ohm resistor is tied to a pin with power flag

Other aspect: Keeping the zero ohm resistor in the schematic will make
the DRC at the board run smooth. And if you forgot the resistor
accidentially, you will got an error message. :O)

With best regards: Bernd Wiebus alias dl1eic



Am Sat, 21 Sep 2024 19:14:54 +0200
schrieb "Pierre-Raymond Rondelle via groups.io"
<pierreraymondrondelle@...>:

John, Robert,

Zero Ohms resistors have the drawback to create two nets.

I had similar issue some years ago with Kicad 5.20, it didn't have
any practical solution for that. So, I cheated, creating symbol and
models for keeping the same net name on both sides of the jumper.
Mandatory for power lines. My computer being too old, I didn't
migrate to newer kicad versions. Consequently, didn't test the trick
on post 5.20. But since you're asking the jumper question I assume
that this hasn't been solved.

Instead, I made a specific component using 3 pads with the same net
name, whichever the pad number is. In the middle a square one (thin
and long, this is the "jumper wire"), of course not drilled and two
round ones at the ends. The 3 pads were? overlapping, establishing a
connection in between the ends.

For the schematics,I created a dedicated symbol with one terminal, (I
named it "lnk"), and filled the attribute table for the BOM. I placed
it on a convenient place on the net the jumper is installed, I
numbered it. That's all.

Refer to the annexed files. Remember it's ver 5.20. You may have to
modify it regarding the new version rules. My application was to
route a number of different single side PCBs where power lines were
routed on component side via jumper wires. Refer to: "Strap
footprint.png" & "Strap footprints in use.png" In schema, the symbol
was: "Strap symbol for eeschema.png", represented by "Strap Symbols
attached to the drawing.png" in the electrical drawing.
"My_Straps.pretty.rar" is the strap library model for 3.81 to 22.86
mm long jumpers. And for the PCB I also provide an example
"strap_test.rar" (not functional, for decorating your bedroom only !
). Have fun



On 20.09.24 18:49, Tony Casey via groups.io wrote:
If you want to use headers and links, I have schematic symbols for
those. Perhaps KiCad even has them in one of its extensive library, I
don't know.

Alternatively, use zero Ohm resistors, and add a text note to say
what they are for. Do that, as well for links. If they are multiple
position links, add a truth table.

I try to put everything on the schematic. That way, nothing gets
missed.

--
Regards,
Tony?

On 20 Sep 2024 17:17, John Woodgate <jmw@...> wrote:

Thanks, Robert. I suppose they have to be placed in the schematic
exactly where they are needed in the layout, which can make the
schematic look very odd. On 2024-09-20 16:35, Robert via groups.io
wrote: They are normally in the schematic as zero ohm resistors.
In the

layout they can be whatever you like, eg pukkka zero ohm resistors
(wire-ended or surface mount), hand-cut wire links, blobs of
solder, etc.

Regards,

Robert

* Plain text email - safe, readable, inclusive. *


--
This email has been checked for viruses by Avast antivirus
software. 





--

OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.www.avg.com

View All 27 Messages

#24222

Join [email protected] to automatically receive all group messages.