Don't Connect/Route Power Pin

Thanks for your reply!

For the solution, I will do as you say and change the names or manual route.

Thanks for all.

autodeskguest  wrote:

Really? You have two pins that you have explicitly placed ON THE SAME

NET in the schematic, thus telling Eagle that they need to be connected,

and you're complaining that it tries to connect them?

 

If they shouldn't be connected then they can't be the same signal and

you need to not have them connected on the schematic.

 

If they are the same signal and should be connected then you WANT the

autorouter to connect them.

 

If the power header and ICSP header both have pins for the 5V supply,

and it's the same 5V supply, then both pins need to be connected to the

5V supply and thus to each other for the board to be correct.

 

If you don't like the particular route that the autorouter lays out then

do that routing by hand. Just don't blame the tool for doing what you

tell it to.

I am aware this is an old thread but I think the subject needs additional explanation.

The problem is when using a device describing some additional PCB that could be placed onto the PCB that is being designed. For example, I've made a device for Arduino Pro Mini 18x32 mm board which can be placed into the schematics as any other component (e.g. resistor or transistor). The problem which original poster is reffering to is the following:

In the described case where the component placed into desigh has multiple pins connected internally, there are multiple situationy when we do not want or even must not to connect these pins once again with PCB traces. For example Pro Mini board has RAW input which goes to the voltage regulator and it has two Vcc ouputs to power some other 5 V device with the same voltage as the µC. However, these pins can be used as inputs as well. If we do not connect voltage to the RAW input (we do not use the voltage regulator) then we can connect 5 V to Vcc pin to power the µC directly. Furthermore, I have a design where the µC is powering the light sensor via output pin (to conserve the battery during sleep) and in that case we don not want anything at all to be connected to Vcc pins. We do not want to connect both internally connected Vcc pins with the traces which will prevent efficien routing of other traces we need.

The second Vcc on that board is just so it is more convenient to connect the programing cable, the secong Vcc pin is not because of the same reason µC itself has more supply pins!! µC has more power supply pins because of the current cosideriations but Mini Pro board has 2 Vcc and 5 GND pins just because of the convenience to connect more devices. When we solder such a board to our PCB we don't care to which of the Vcc of GND pins will some trace be connected. But we do care if Eagle insists that we draw the traces to connect the internally already connected pins once again - and to ruin our routing!! The traces between multiple Vcc and multiple GND pins are already routed on our board that is soldered onto the design, we do not want to connect those traces again because in our design.

The original poster was right when he was annoyed by Eagle's insisting to connect already connected traces once again. That is (was?) well known Eagle's problem of which the authors were aware - so they even implemented the solution.

giova013  wrote:

For the solution, I will do as you say and change the names or manual route.

Changing the names of pins in library is not a good idea. That way you will have to change schematics every time you change your mind and decide to route the trace towards some of the alternative pins. For example, let's say you have Arduino which is powered with 9V via RAW input so you get 5V at several pins. If every 5V pin (which you will use to power some sensor or something) will have a different name then you will have to decide from where (from which exactly of the several possible 5V pins) you are going to route the trace in advance - during drawing schematics. If you later after switching to board view decide there is a better solution to draw the traces if you use another 5V pin, then you will have to go back to the schematics and change the connections to be able to route the trace from other 5V pin.

Similarly, if you placed Arduino board on your PCB and you are using one of the Arduino's 5V pins to directly power the board with 5V then you will have the same problem - you will have to decide which of the several 5V pins will be used to power the Arduino in advance - before having the chance to route the traces. Later when you notice it might be better to power the Arduino through one of the other 5V pins, you will have to go back to the schematics and change the connections.

On 28/10/17 10:28, Ch Ch wrote:

  wrote:

For the solution, I will do as you say and change the names or manual route.

 

Changing the names of pins in library is not a good idea. That way you will have to change schematics every time you change your mind and decide to route the trace towards some of the alternative pins. For example, let's say you have Arduino which is powered with 9V via RAW input so you get 5V at several pins. If every 5V will have a different name then you will have to decade where you are going to route the trace in advance - during drawing schematics. If you later after switching to board view decide there is a better solution to draw the traces if you use another 5V pin, then you will have to go back to the schematics and change the connections to be able to route the trace to other pin.

 

Similarly, if you placed Arduino board on your PCB and you are using one of the Arduino's 5V pins to directly power the board with 5V then you will have the same problem - you will have to decide which of the severay 5V pins will be used to power the Arduino in advance - before having the chance to route the traces. Later when you notice it might be better to power the Arduino through one of the other 5V pins, you will have to go back to the schematisc and change the connections.

 

I'm struggling to make head or tail of what you're trying to say here

but it sounds like utter tosh.

If the daughter board is being powered by 9V and the 5V pins on it are

powering other parts of the main board, it's acting like a regulator,

and all its 5V pins are outputs with parallel function. It's fine to

connect them all.

If they're all connected together and can be used to "route through"

then that's a separate issue, which was addressed, but it's not usually

good practice to do so. In any case, if you are routing through a

part, deliberately, then it's definitely good practice to SHOW THAT ON

THE SCHEMATIC, otherwise your test technician is going to be seriously

confused when debugging. Which puts us firmly in the

decide-in-advance-and-use-different-nets scenario.

autodeskguest  wrote:

I'm struggling to make head or tail of what you're trying to say here

but it sounds like utter tosh.

 

If the daughter board is being powered by 9V and the 5V pins on it are

powering other parts of the main board, it's acting like a regulator,

and all its 5V pins are outputs with parallel function. It's fine to

connect them all.

 

If they're all connected together and can be used to "route through"

then that's a separate issue, which was addressed, but it's not usually

good practice to do so. In any case, if you are routing through a

part, deliberately, then it's definitely good practice to SHOW THAT ON

THE SCHEMATIC, otherwise your test technician is going to be seriously

confused when debugging. Which puts us firmly in the

decide-in-advance-and-use-different-nets scenario.

I am saying this:

https://electronics.stackexchange.com/questions/110585/eagle-how-to-make-the-router-ignore-internally-connected-pins-in-…

English is not my native language so it might worth reading various posts regarding the same problem written by native speakers that could be found on internet.

Yes, if the daughterboard is powering other parts of the main board, it might be fine to connect all pins together. Consider this 'daughterboard', it has 5 GND pins and 2 Vcc pins. Vcc pins can be used to power the 'daughterboard' or to power something else with the 'daughterboard'.

1. If the 'daugterboard' is powered via RAW pin (going to voltage regulator) then +5V is present on both Vcc pins, ready to be used for powering some other device. The output of a voltage regulator is connected to Vcc pins.

2. If the main board already has +5V rail, then the 'daughterboard' can be powered directly through one of the Vcc pins. In that case RAW input of the 'daughterboard' is not used and daughterboard's voltage regulator is out of use. It is up to the PCB designer to decide whether to connect +5V to all of the Vcc pins or just to one of them which might be more suitable regarding the traces.

3. If the 'daughterboard' is powered via RAW pin and designer decided to power up some device using I/O pin of the microcontroller then PCB designer might decide to leave Vcc pins unconnected. For example, I have a design where I am using a voltage divider formed by a resistor and a LDR. The voltage divider is not powered from +5V but is powered from one of the I/O pins. That way I can cut the power to the voltage divider in software before putting µC to sleep so the voltage divider does not consume power during the sleep intervals.

4. There are 5 GND pins on the 'daughterboard'. GND pins near RX and TX pins are because so it is easier to connect USB --> UART converter which has very short reach of the connectors. Additional Vcc and GND pins are made for the use case when the 'daughterboard' is used as a standalone board. When that board is used as a 'daughterboard' then it is not necessary to use all of them, it is enough to use just one of the Vcc pins and just one of the GND pins. These pins are VCC@1, VCC@2, GND@1, GND@2, GND@3, GND@4 and GND@5. It is up to PCB designer to decide which one will be used and which one will not be used. Similarly there are two pairs of RS232 pins, RXI@1, RXI@2, TXO@1 and TXO@2. It is up to PCB designer to decide which RX and which TX pin is he going to use. When we use the board as a standalone then we do not connect both RX pins together on the outside of the board, we use just one of the RX pins. When we use the board as a standalone then we do not use all of the Vcc pins to power the board with +5V, we use just one of the Vcc pins to power the board and we might decide to do the same in the case the board is used as a 'daughterboard'.

Yes, it is a good practice to 'show that on the schematics' but it is up to PCB designer to decide whether he is going to use one or more pins to power the 'daughterboard'. Internally connected pins in case of the board I mentioned are interchangeable, that is - you might use just one of them or you could connect all of them even on the outside of the 'daughterboard'. If you do not want to increase the complexity of the main PCB's traces, then you will use just one of the daughterboard's Vcc pins and just one of the RX/TX pins and just one of the exposed GND pins. In that case you will have to leave some unrouted traces meaning some airwires will remain in the design. Alternatively, you might route these unwanted connections (which are forced by Eagle) in the layer which will not be sent to the manufactory. It is not up to the software to decide if you want to use one or more of the 'same' pins. Pins named as name@1, name@2, name@3, name@4, ... are already connected together and connecting the trace to any of these will connect all of them to the same net.

When the 'daugtherboard' is used as a standalone, do you connect +5V to all of the Vcc pins? No, you connect +5V to just one of them, the one which is the most suitable considering physical locations of the multiple Vcc pins. The same is for powering the 'daugterboard' or when the 'daughterboard' is powering other devices.

BTW, I cannot find this thread by browsing the forum!? I can find it only with google.

giova013  wrote:

 

Hi everyone!

I'm making an Arduino Due Shield, and at the Main Board there are Output Power Pins (+5V, +3V3), which I use in my Shield.

The problem is that those pins are being connect one to each other (Output to Output) and not only to what is being used in my Shield (as Input).

Those Output Power Pins are in a simple Header.

Is there someway to tell the program to don't connect them?

 

Thanks!

To summarize everything in just a few sentences:

1. What you were asking can be easily done with Eagle 7 as described in the attached picture.

2. What you can do as a workaround in Eagle 6, I have described in my previous post. I am sure there are other workarounds too.

Attachments:

jw0752  wrote:

 

Hi Giovanni,

The 3V3 and the 5 volt power taps on the header of the Arduino should not be connected to one another.

<snip>

John

Just for the clarification, because this thread is full of misunderstandings or wrong interpretations of what someone said:

When original poster said: 'The problem is that those pins are being connect one to each other', he didn't want to say that 5V and 3V3 pins are connected together - he wanted to say that multiple 5V pins are connected together (by airwires) and multiple 3V3 pins are connected together forcing him to route the traces which he does not need or want to route.

I have here described the solution. What original poster asked is legitimate demand and it seems the option of doing exactly what was asked was finally added as a new option in Eagle 7. No doubt Eagle developers added that option after realizing it was missing.

Thank you for your clarification of what the original poster said 2 years ago. I had forgotten my response. I usually avoid replying on the CadSoft questions as they are usually more about CadSoft's protocols and not so much about the actual electronics. Here on the E14 site we see the CadSoft forum as but one of many streams. Based on the phrasing of the original question I stand by my answer but I can also see where I could have misunderstood the poster.

John

jw0752  wrote:

 

Thank you for your clarification of what the original poster said 2 years ago. I had forgotten my response. I usually avoid replying on the CadSoft questions as they are usually more about CadSoft's protocols and not so much about the actual electronics. Here on the E14 site we see the CadSoft forum as but one of many streams. Based on the phrasing of the original question I stand by my answer but I can also see where I could have misunderstood the poster.

 

John

You are welcome. I think these old threads are a valuable source of informations for someone who will search for the solution to the same problem in the future. This thread might save someone hours of time. Especially because this thread is the very first result when searching google with the string:

cadsoft eagle how to route not connected pins

In fact I registered just to answer this question. Otherwise I use news client for accessing news.cadsoft.de server to read the topics but this thread did't show among the posts and I am not able to find it using any combination of the links starting from www.element14.com

Regards