Actions
Forum Thread Details
  • Replies 7 replies
  • Subscribers 179 subscribers
  • Views 2614 views
  • Users 0 members are here
Related

label of supply symbols

autodeskguest

Hi all,

I wonder if there is a way to automatically label a supply symbol (i.e.

GND) to reflect the actual name of the net it is connected to.

 

In my schematic I have about ten isolated ground nets. I named each one

with different (and meaningful) names, like: GND_MCU, GND_AUDIO,

GND_UART, etc...

 

To improve the readability of the schematic I would like to place a

label close to each ground symbol to show the name of "its" net.

 

Right now I'm able to do so only using the LABEL command, attaching it

to the net. It works, but it would be much easier if the symbols can

show it by itself, using something like >NAME or >VALUE placeholders.

 

Thanks

Marco

 

Parents

  • Hi Marco,

     

    You can create library parts for all your alternative voltages that you

    require and then these will have the right name and automatically set the

    signal name of the signal they are connected to. Manually setting the net

    name to be different from what the symbol implies and adding net labels to

    show the right value runs the risk of missing something and ending up with

    things not connected where you expect.

     

    In the library manager, duplicate the GND device and rename it to for

    example GND_MCU and do the same with the GND symbol. Then open the GND_MCU

    symbol and change the pin name from GND to GND_MCU also. Finally, open the

    GND_MCU device, delete the GND symbol and add in the GND_MCU symbol. Now

    when you place this in your schematics it will work correctly and put the

    correct name on your nets.

     

    IMPORTANT Remember to rename the symbol pin. Failure to remember this

    will result in the original name being placed on the nets which you may not

    see until it's too late, so check, check and check again when you create

    alternative power supply symbols!

     

    Best Regards,

     

    Rachael

    --

    EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

     

Reply

  • Hi Marco,

     

    You can create library parts for all your alternative voltages that you

    require and then these will have the right name and automatically set the

    signal name of the signal they are connected to. Manually setting the net

    name to be different from what the symbol implies and adding net labels to

    show the right value runs the risk of missing something and ending up with

    things not connected where you expect.

     

    In the library manager, duplicate the GND device and rename it to for

    example GND_MCU and do the same with the GND symbol. Then open the GND_MCU

    symbol and change the pin name from GND to GND_MCU also. Finally, open the

    GND_MCU device, delete the GND symbol and add in the GND_MCU symbol. Now

    when you place this in your schematics it will work correctly and put the

    correct name on your nets.

     

    IMPORTANT Remember to rename the symbol pin. Failure to remember this

    will result in the original name being placed on the nets which you may not

    see until it's too late, so check, check and check again when you create

    alternative power supply symbols!

     

    Best Regards,

     

    Rachael

    --

    EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

     

Children
  • in reply to rachaelp

    Il 12/05/2017 12:52, Rachael ha scritto:

     

    You can create library parts for all your alternative voltages that you

    require and then these will have the right name and automatically set the

    signal name of the signal they are connected to. Manually setting the net

    name to be different from what the symbol implies and adding net labels to

    show the right value runs the risk of missing something and ending up with

    things not connected where you expect.

     

     

    Thanks for your answer.

    Yes, this could be a solution. The drawback is I will end up with a list

    of symbols some of them used only in one project...

     

     

    In the library manager, duplicate the GND device and rename it to for

    example GND_MCU and do the same with the GND symbol. Then open the GND_MCU

    symbol and change the pin name from GND to GND_MCU also. Finally, open the

    GND_MCU device, delete the GND symbol and add in the GND_MCU symbol. Now

    when you place this in your schematics it will work correctly and put the

    correct name on your nets.

     

    IMPORTANT Remember to rename the symbol pin. Failure to remember this

    will result in the original name being placed on the nets which you may not

    see until it's too late, so check, check and check again when you create

    alternative power supply symbols!

     

     

    Yeah, I'm aware of this.

    Do you think it would possible to write an ulp to do all this stuff? It

    needs several actions and it's error prone if you have to make dozens of

    such a device...

     

     

     

  • in reply to autodeskguest

    Marco Trapanese wrote on Fri, 12 May 2017 12:27

    Il 12/05/2017 12:52, Rachael ha scritto:

     

    You can create library parts for all your alternative voltages

    that you

    require and then these will have the right name and automatically

    set the

    signal name of the signal they are connected to. Manually setting

    the net

    name to be different from what the symbol implies and adding net

    labels to

    show the right value runs the risk of missing something and ending

    up with

    things not connected where you expect.

     

    Thanks for your answer.

    Yes, this could be a solution. The drawback is I will end up with a

    list

    of symbols some of them used only in one project...

     

    In this case, how about copying the symbols to a project specific lbr file

    which you keep with the sch/brd files so you don't clutter up your main

    library?

     

    Marco Trapanese wrote on Fri, 12 May 2017 12:27

    In the library manager, duplicate the GND device and rename it to

    for

    example GND_MCU and do the same with the GND symbol. Then open the

    GND_MCU

    symbol and change the pin name from GND to GND_MCU also. Finally,

    open the

    GND_MCU device, delete the GND symbol and add in the GND_MCU

    symbol. Now

    when you place this in your schematics it will work correctly and

    put the

    correct name on your nets.

     

    IMPORTANT Remember to rename the symbol pin. Failure to remember

    this

    will result in the original name being placed on the nets which

    you may not

    see until it's too late, so check, check and check again when you

    create

    alternative power supply symbols!

     

    Yeah, I'm aware of this.

    Do you think it would possible to write an ulp to do all this stuff? It

     

    needs several actions and it's error prone if you have to make dozens

    of

    such a device...

     

    Yes I think so, i'd imagine it would be quite straightforward but I'd need

    to have a bit more of a look to be sure. It would be quite a useful tool

    for creating such devices for project specific use I think.

     

    Best Regards,

     

    Rachael

     

    --

    EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

     

  • in reply to rachaelp

    rachaelp wrote on Fri, 12 May 2017 12:33

    Marco Trapanese wrote on Fri, 12 May 2017 12:27

    Do you think it would possible to write an ulp to do all this

    stuff? It

    needs several actions and it's error prone if you have to make

    dozens of

    such a device...

     

    Yes I think so, i'd imagine it would be quite straightforward but I'd

    need to have a bit more of a look to be sure. It would be quite a useful

    tool for creating such devices for project specific use I think.

     

    Best Regards,

     

    Rachael

     

     

    Just a quick follow-up, I had a quick look and I think writing a ULP to do

    this is relatively simple. The command line commands to run from the

    library are easy to build up and If I have a spare 30 minutes later on I

    will have a go at putting something together in ULP to automate it a little

    better. For now here is the command I just used on my library to test it:

     

    copy 0V.dev@ 0V_TEST;copy 0V.sym@ 0V_TEST;name 0V 0V_TEST;edit

    0V_TEST.dev;del (0 0);add 0V_TEST (0 0); edit;

     

    Note that all my power devices have the symbol nicely placed at the origin

    hence the above works. If they were placed in an ad-hoc way it wont and

    will require a little ULP to get the right location.

     

    Best Regards,

     

    Rachael

     

     

     

    --

    EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

     

  • in reply to rachaelp

    On 5/12/2017 8:17 AM, Rachael wrote:

    rachaelp wrote on Fri, 12 May 2017 12:33

    Marco Trapanese wrote on Fri, 12 May 2017 12:27

    Do you think it would possible to write an ulp to do all this

    stuff? It > needs several actions and it's error prone if you have

    to make

    dozens of > such a device...

     

    Yes I think so, i'd imagine it would be quite straightforward but I'd

    need to have a bit more of a look to be sure. It would be quite a useful

    tool for creating such devices for project specific use I think.

     

    Best Regards,

     

    Rachael

     

    Just a quick follow-up, I had a quick look and I think writing a ULP to do

    this is relatively simple. The command line commands to run from the

    library are easy to build up and If I have a spare 30 minutes later on I

    will have a go at putting something together in ULP to automate it a little

    better. For now here is the command I just used on my library to test it:

    copy 0V.dev@ 0V_TEST;copy 0V.sym@ 0V_TEST;name 0V 0V_TEST;edit

    0V_TEST.dev;del (0 0);add 0V_TEST (0 0); edit;

     

    Note that all my power devices have the symbol nicely placed at the origin

    hence the above works. If they were placed in an ad-hoc way it wont and

    will require a little ULP to get the right location.

     

    Best Regards,

     

    Rachael

     

     

     

     

    Hi All,

     

    There are already is a ULP for making supply symbols. You can grab it

    from here:

    http://eagle.autodesk.com/eagle/ulp?utf8=%E2%9C%93&q%5Btitle_or_author_or_description_cont%5D=supply&button=

     

    Pick make-supplysym-dev.zip.

     

    Please let me know if there's anything else I can do for you.

     

    Best Regards,

    Jorge Garcia

     

    --

    We have a new forum here <http://forums.autodesk.com>

     

  • in reply to autodeskguest

    Jorge Garcia wrote on Fri, 12 May 2017 18:53

    Hi All,

     

    There are already is a ULP for making supply symbols. You can grab it

    from here:

     

    http://eagle.autodesk.com/eagle/ulp?utf8=%E2%9C%93&q%5Btitle_or_author_

    or_description_cont%5D=supply&button=

     

    Pick make-supplysym-dev.zip.

     

    Please let me know if there's anything else I can do for you.

     

    Best Regards,

    Jorge Garcia

     

    --

    We have a new forum here <http://forums.autodesk.com>

     

     

    Thanks Jorge, this is very useful! I'd taken the approach of copying and

    modifying an existing symbol programmatically but this is much neater image

     

     

    --

    EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

     

  • in reply to autodeskguest

    Il 12/05/2017 19:53, Jorge Garcia ha scritto:

     

    There are already is a ULP for making supply symbols. You can grab it

    from here:

    http://eagle.autodesk.com/eagle/ulp?utf8=%E2%9C%93&q%5Btitle_or_author_or_description_cont%5D=supply&button=

     

    Pick make-supplysym-dev.zip.

     

     

    Very useful!

    Thanks!

    Marco