How to add 0R 1206 Resistor as Jumper t o Board Layout

farabiahmed wrote on Wed, 09 June 2010 11:06

But I can't find how to do it by Eagle without adding to schematic.

Good, because such things should be in the schematic.  You can make a

jumper device and have it use your 0 Ohm resistor footprint if you like.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

[quote

Good, because such things should be in the schematic.  You can make a

jumper device and have it use your 0 Ohm resistor footprint if you

like.

Thanks, but how can I tell Eagle, this jumper device's pins are same?

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

"Ahmed" <farabiahmed@gmail.com> wrote in message

news:hupu51$gqe$1@cheetah.cadsoft.de...

[quote Good, because

such things should be in the schematic.  You can make a

jumper device and have it use your 0 Ohm resistor footprint if you

like.

>

Thanks, but how can I tell Eagle, this jumper device's pins are same?

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the

CadSoft EAGLE community meets.

if the "jumper device's pins are same", what's the scope of the componnent?!

I think you need to reconsider your way of thinking PCB's!

Olin Wrote...

[quote

Good, because such things should be in the schematic.  You can make a

jumper device and have it use your 0 Ohm resistor footprint if you

like.

>

"Ahmed" wrote in reply

Thanks, but how can I tell Eagle, this jumper device's pins are same?

--

Ahmed

Don't think of this as two items. Olin is talking of one device here.

Search the libraries for a "Solder Jumper". That will give you a picture of

what you are aiming for. A 'symbol to appear in the  schematic  and a

footprint (package)  to appear on the board.

When these are logically joined you have a device. This is what Olin

suggests you make. That way you get the correct look for your schematic and

it will have a 1206 footprint on the board.

Warren

On 6/9/2010 2:39 PM, Olin Lathrop wrote:

farabiahmed wrote on Wed, 09 June 2010 11:06

>> But I can't find how to do it by Eagle without adding to schematic.

>

Good, because such things should be in the schematic. You can make a

jumper device and have it use your 0 Ohm resistor footprint if you like.

Just curious, what is the rationale to have such in the schematic? I

could understand if it is a jumper in the sense of selecting a

particular option. And of course, it needs to be in the BOM no matter what.

But what if the board has a significant jumper layer and there are many

0R jumpers that are just part of the circuitry, not selecting anything.

Why would I want to see these on the schematic? How does EAGLE know that

the net name should be the same on both sides of the jumper?

Is it more expensive to move up from a 2 layer to 4 layer board or just

add 10 0R jumpers? Looking at real circuit boards from disk drives and

the like, I see many examples of 2 layer + jumper construction...

Gary Gofstein schrieb:

Is it more expensive to move up from a 2 layer to 4 layer board or just

add 10 0R jumpers? Looking at real circuit boards from disk drives and

the like, I see many examples of 2 layer + jumper construction...

In most cases, a four layer board is significantly more expensive than a

two layer board with /many/ additional jumpers (depends on board size,

of course).

Tilmann

On Thu, 10 Jun 2010, Gary Gofstein wrote to us saying :

>But what if the board has a significant jumper layer and there are many

>0R jumpers that are just part of the circuitry, not selecting anything.

>Why would I want to see these on the schematic? How does EAGLE know

>that the net name should be the same on both sides of the jumper?

Ask yourself why the jumpers are there. Remember, the schematic is the

master definition, the board is merely an implementation. If the jumper

has to be there for the system to work then it MUST appear in the

schematic. This includes the case where a ground track needs to be taken

from a particular point, such as a star-earth design. If you're doing

star earthing, you MUST show that on the schematic, and Eagle needs to

know the two (or more) sides of the star are different nets.

If there are 0R jumpers, they must be there for a reason. I cannot think

of any possible reason to employ one that doesn't imply some

significance that really MUST be shown on the schematic. If you don't

need to show it on the schematic then you don't really need it there,

and a better board layout is the answer you actually want.

So that leaves only the possibility that you are hand-making a PCB and

don't want to go to double-sided (or from 2-layer to 4-layer), and

therefore intend to fit a few short wires to make up the missing bits of

track. In that case, I would suggest that your best bet is to design a

double-sided (or 4-layer) board with as little as physically possible on

the extra layers, then ignore those layers when making the PCB. The

layers that are not physically implemented on the PCB then show where

the wire links need to be added.

>Is it more expensive to move up from a 2 layer to 4 layer board or just

>add 10 0R jumpers? Looking at real circuit boards from disk drives and

>the like, I see many examples of 2 layer + jumper construction...

I've not often seen a professionally built high-density board that used

0R0s purely to avoid extra layers. I've seen lots where there were 0R0s

liberally scattered for build option selection reasons (disk drives

often do that) so that one PCB can be built for several different

products (e.g. different drive capacities, different motor types). I

have seen a few audio amplifiers where the PCB is single-sided and

various signals are carried on heavy gauge bus bars instead of tracks; I

don't know what the schematics for them look like.

--

Rob Pearce                       http://www.bdt-home.demon.co.uk

The contents of this | Windows NT crashed.

message are purely   | I am the Blue Screen of Death.

my opinion. Don't    | No one hears your screams.

believe a word.      |

On 6/11/2010 9:43 AM, Robert Pearce wrote:

>

Ask yourself why the jumpers are there.

They're there because a 4 layer board is more expensive than a 2 layer

board with jumpers.

track. In that case, I would suggest that your best bet is to design a

double-sided (or 4-layer) board with as little as physically possible on

the extra layers, then ignore those layers when making the PCB. The

layers that are not physically implemented on the PCB then show where

the wire links need to be added.

That works for wire links, but they must be cut and stripped and

probably installed by hand, does not work for 0R0 jumpers.

>

I've not often seen a professionally built high-density board that used

0R0s purely to avoid extra layers.

Maybe because the EDA tools like EAGLE don't handle it very gracefully.

I've seen lots where there were 0R0s

liberally scattered for build option selection reasons (disk drives

often do that) so that one PCB can be built for several different

products (e.g. different drive capacities, different motor types). I

These were clearly a jumper layer. If it results in a more reliable (2

layer), more manufacturable, lower cost board and is electrically

equivalent - why wouldn't someone use them?

If it sounds like I'm preaching, I'm not; but I have asked this question

many times and I have never gotten a satisfactory answer. Is there

something wrong with using a jumper layer that I don't know about? Or is

it just that it is too time consuming or impossible to make one on most

EDA tools?

On 6/11/2010 3:22 PM, Gary Gofstein wrote:

On 6/11/2010 9:43 AM, Robert Pearce wrote:

>>

>> Ask yourself why the jumpers are there.

>

They're there because a 4 layer board is more expensive than a 2 layer

board with jumpers.

>

>> track. In that case, I would suggest that your best bet is to design a

>> double-sided (or 4-layer) board with as little as physically possible on

>> the extra layers, then ignore those layers when making the PCB. The

>> layers that are not physically implemented on the PCB then show where

>> the wire links need to be added.

>

That works for wire links, but they must be cut and stripped and

probably installed by hand, does not work for 0R0 jumpers.

>>

>> I've not often seen a professionally built high-density board that used

>> 0R0s purely to avoid extra layers.

>

Maybe because the EDA tools like EAGLE don't handle it very gracefully.

>

I've seen lots where there were 0R0s

>> liberally scattered for build option selection reasons (disk drives

>> often do that) so that one PCB can be built for several different

>> products (e.g. different drive capacities, different motor types). I

>

These were clearly a jumper layer. If it results in a more reliable (2

layer), more manufacturable, lower cost board and is electrically

equivalent - why wouldn't someone use them?

>

If it sounds like I'm preaching, I'm not; but I have asked this question

many times and I have never gotten a satisfactory answer. Is there

something wrong with using a jumper layer that I don't know about? Or is

it just that it is too time consuming or impossible to make one on most

EDA tools?

From reading this thread I think the main problem is we don't actually

understand what you are trying to achieve with these jumpers.

I have seen 0R SMT jumpers used on a few prototypes and they where used

for this reason:

The company has in house board manufacturing but only for 2-4layers and

during development the board was too complex for a 4layer routing and

they used SMT jumpers that looked like resistors but where just wire

bridges in a standard SMT package. They where not on the schematic as

the guy who routed the board just added them to get those last few

airwires routed. This worked but if I saw a commercial product with that

I would stay away as they where obviously cutting corners or cheap.

The second reason to use 0R jumpers is the acceptable reason. If you

look on things like hard drive logic boards, digital oscilloscopes, or

mp3 players that have a 2/4/8 gig option to buy they use 0R jumpers to

specify which model the device is. For example I had a sandisk mp3

player years ago with 2GB memory and if you replace it with a 4GB chip

the player still only uses 2GB. After you clear and set some bridges it

work with the full 4gb. We do that as most boards are not programmed

after full assembly and its easier to have one firmware and use 0R

jumpers to select features in the last phase of mfg.

Don't know if that's what you where talking about or now but if you try

and word your question with a specific example where the sch has no

jumpers and the pcb does we can find out why.

I've just come up against this problem recently.

I'm using single sided & 1206.

I wanted to have something that would 'bridge' over another track (to save

using a bit of wire), so I just used a 0R 1206 resistor - I slighly

modified the package 'gap' between pads (on account I needed more space

since I want to run a fine track in  between the the resistor pads.

Once I created the the new library part, I simply added it to the schematic

at more or less the same point where I wanted to be on my board file.

It all works well,

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.