开云体育

How are jumpers? included in a board design? Do they appear in the schematic or only in the PCB layout? Are they to be treated as zero-ohm resistors, perhaps?

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

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.
www.avast.com

开云体育

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.

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

开云体育

Hello,
??? Instead of jumper, I offen use so called in French "coffee bean". Just put a drop of solder to make the connection.

开云体育

Thanks, Jean-Paul, but I want to jump over a track on a 2-layer through-hole board. A zero-ohm resistor works.

Hello,
??? Instead of jumper, I offen use so called in French "coffee bean". Just put a drop of solder to make the connection.

???

??? Regards, Jean-Paul

****
Site :

Le 2024-09-20 à 17:30, John Woodgate a écrit?:

How are jumpers? included in a board design? Do they appear in the schematic or only in the PCB layout? Are they to be treated as zero-ohm resistors, perhaps?

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

开云体育

Thanks, Tony. My need is very simple, to allow one track on a layer to cross another. I can put zero ohm resistors on the schematic, but (inevitably, I suppose) that restricts the routing of the jumpered track. In other words, without the jumper I could join point C to either point A? or point B, but if a jumper is needed between B and C, point C can only be joined to point B.

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.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Given what you are trying to achieve, John, you could create a custom
schematic symbol that looks like a wire segment. You could even hide
all the text fields. Basically it would just be two back-back pins, so
once connected up it would just be a straight line on the schematic
(albeit brown, which will help you find it again :)).

Regards,

Robert.

开云体育

Thank you, Robert.

Given what you are trying to achieve, John, you could create a custom
schematic symbol that looks like a wire segment.?? You could even hide
all the text fields.?? Basically it would just be two back-back pins, so
once connected up it would just be a straight line on the schematic
(albeit brown, which will help you find it again :)).

Regards,

Robert.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

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

Hello John.

I suppose they have to be placed in the schematic
exactly where they are needed in the layout,

Exactly. A schematic is used to document and describe your circuit, an
despite this zero ohm resistor has nothing to do with the principal
function of the circuit, it has a fundamental function at this board.

So you have to show it in the schematic, but of course, with a comment.

which can make the
schematic look very odd.

Not if you mention the following:

For creating the board, you will need this jumper as a real material
device. So for planning your materials, it should be noticed at the
BOM, which can easily done by software, if this device is mentioned at
the schematic.

Also a jumper can be a nice place for measuring or injecting signals
for trobleschooting. Another reason to show it at the schematic.

Maybe even for orientating at schematic/board. Jumpers can be good
landmarks.

There are other types of jumpers, which are not made as zero ohm
resistors for crossing, but by sockets and short circuit plugs or with
(special) solder pads and solder blobs. Of course, also by pads and
zero ohm resistors.

This Type of jumpers are by function at reality switches, and so, they
should be shown at the schematic as switches.

With best regards Bernd Wiebus alias dl1eic






Am Fri, 20 Sep 2024 17:17:59 +0100
schrieb "John Woodgate via groups.io" <jmw@...>:

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.
www.avast.com

-----BEGIN PGP SIGNATURE-----

iQEzBAEBCgAdFiEEceydlAu1Ov6Z3ILE6D4maolCoowFAmbtyxcACgkQ6D4maolC
oozmeggAgeo+MgVW5uDCTnHzMXq1WWsryHkTSy50JZGRKHbC/nhdlvwq4dyQlkYC
vYbByLjxQcR18LekhlXWIsNrV9EogGAtLsDNulEfqk7Z5U8Qxx4PFRim6nCT/7Lr
4E1Sa3UBfo52VvmtSGqdy8YmF/4IT90fZFHERHsJM1PU2US8P4aktPOcsIsoEgtb
DmnC7wQPmfdQWH90TPmqdz0Fcs29Y8QmjJvwt+//MRtchICeUm5TihEs+91mkzSD
zAKsmXW1FG+97Rgs/Si1Fgkkbqg5+5lfA6PJfr7V54k9fALpxQUAOYIAde9A8Ktr
ehAy1MVU5l6NcYv0M5LnSzOqRGy97Q==
=R7/h
-----END PGP SIGNATURE-----

开云体育

Thank you, Bernd.

On 2024-09-20 20:20, Bernd Wiebus via groups.io wrote:

Hello John.

> I suppose they have to be placed in the schematic
> exactly where they are needed in the layout,

Exactly. A schematic is used to document and describe your circuit, an
despite this zero ohm resistor has nothing to do with the principal
function of the circuit, it has a fundamental function at this board.

So you have to show it in the schematic, but of course, with a comment.

> which can make the
> schematic look very odd.

Not if you mention the following:

For creating the board, you will need this jumper as a real material
device. So for planning your materials, it should be noticed at the
BOM, which can easily done by software, if this device is mentioned at
the schematic.

Also a jumper can be a nice place for measuring or injecting signals
for trobleschooting. Another reason to show it at the schematic.

Maybe even for orientating at schematic/board. Jumpers can be good
landmarks.

There are other types of jumpers, which are not made as zero ohm
resistors for crossing, but by sockets and short circuit plugs or with
(special) solder pads and solder blobs. Of course, also by pads and
zero ohm resistors.

This Type of jumpers are by function at reality switches, and so, they
should be shown at the schematic as switches.

With best regards Bernd Wiebus alias dl1eic

?




Am Fri, 20 Sep 2024 17:17:59 +0100
schrieb "John Woodgate via groups.io" <jmw@...>:



> 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

开云体育

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

开云体育

Thank you very much.

I just want one trace on a through-hole board to permanently 'hop over' another on the same layer. But 'Mandatory for power lines.' worries me, because I do want to put a hop-over in a power line (+ supply to an opamp).? Why is it mandatory and what are the bad effects if it's not done?

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.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

-----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. www.avast.com





--

OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.www.avg.com

-----BEGIN PGP SIGNATURE-----

iQEzBAEBCgAdFiEEceydlAu1Ov6Z3ILE6D4maolCoowFAmbvGRUACgkQ6D4maolC
ooxFawf/ZCK6AojJIW478kwpa8gX/cbkjyt3oA6NyJ48Rj9IDjbwqeQUTrQotBTN
yx8SHMpRnkuygMU+Eq102g4wsNMfugsk9ASioa9EQ55LtcCkAqtKG7ukRDW8CeZq
5hA/umxrNPBa5A3cEUmXLn79OPz6RHKF+guB1wu9IPYxwZUnhMuHl3FGqJIQagvO
b4pyLd+H0d4/E6XOZkkrx70TBrWk2LlnRaLv5gMVVb9seiZX349j68qqpxSed0uH
HL9k/5eoB1hV/sL9Hd7cL/5RPlMx8JxyY2ssgT/H786WwUhV/D5qkf0dkJll4ehw
HsSlCyL+dNBP0CPojy+B0UNq6U3dgQ==
=tKEO
-----END PGP SIGNATURE-----

开云体育

Excuse me John, I had not been clear at all. My mistake. Mandatory is in my applications because power lines are the ones that pose me most of the problems in logic boards. My boards are dense, all of them are routed on component side. And I said mandatory because of the net name change between one side and the other of a 0-Ohm strap. In this case if I have to route a line between an IC gnd to the gnd, jumping? over other lines, and use a jumper, the IC side of a the jumper must not change its gnd name and THIS IS a real problem causing conflicts. You may ignore some of the errors but that's quite messy for me.

Instead of naming this part as "lnk" or "strap" or "jumper", I probably had to name it "net transfer component".

The purposes of this special part were to keep the net name, include this component in the BOM and make the error check happy. In addition it's identified on the electrical drawing.

Just for my information, when you have tested it, please tell me if it still play a helpful role in the last version of Kicad or if it's redundant with a new function that I don't yet know. Thks.

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

开云体育

Thank you, Pierre-Raymond. I will try to answer your question, but it may be long delayed.

Excuse me John, I had not been clear at all. My mistake. Mandatory is in my applications because power lines are the ones that pose me most of the problems in logic boards. My boards are dense, all of them are routed on component side. And I said mandatory because of the net name change between one side and the other of a 0-Ohm strap. In this case if I have to route a line between an IC gnd to the gnd, jumping? over other lines, and use a jumper, the IC side of a the jumper must not change its gnd name and THIS IS a real problem causing conflicts. You may ignore some of the errors but that's quite messy for me.

Instead of naming this part as "lnk" or "strap" or "jumper", I probably had to name it "net transfer component".

The purposes of this special part were to keep the net name, include this component in the BOM and make the error check happy. In addition it's identified on the electrical drawing.

Just for my information, when you have tested it, please tell me if it still play a helpful role in the last version of Kicad or if it's redundant with a new function that I don't yet know. Thks.

On 21.09.24 19:24, John Woodgate via groups.io wrote:

Thank you very much.

I just want one trace on a through-hole board to permanently 'hop over' another on the same layer. But 'Mandatory for power lines.' worries me, because I do want to put a hop-over in a power line (+ supply to an opamp).? Why is it mandatory and what are the bad effects if it's not done?

On 2024-09-21 18:14, Pierre-Raymond Rondelle via groups.io wrote:

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.

--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.

-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

开云体育

No matter John! This is to provide more accurate information next time the question emerges.

Don't miss Bernd's message, this another way to solve your issue.