EAGLE Central Forums
Where the EAGLE community meets. Sponsored by Stratford Digital.

Home » CadSoft Support Forums » eagle.support.eng » label of supply symbols
label of supply symbols [message #170434] Fri, 12 May 2017 10:17 Go to next message
Marco Trapanese
Messages: 297
Registered: May 2007
Senior Member
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
Re: label of supply symbols [message #170435 is a reply to message #170434] Fri, 12 May 2017 10:52 Go to previous messageGo to next message
rachaelp
Messages: 583
Registered: March 2015
Location: UK
Senior Member
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
Re: label of supply symbols [message #170436 is a reply to message #170435] Fri, 12 May 2017 11:27 Go to previous messageGo to next message
Marco Trapanese
Messages: 297
Registered: May 2007
Senior Member
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...
Re: label of supply symbols [message #170437 is a reply to message #170436] Fri, 12 May 2017 11:33 Go to previous messageGo to next message
rachaelp
Messages: 583
Registered: March 2015
Location: UK
Senior Member
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
Re: label of supply symbols [message #170438 is a reply to message #170437] Fri, 12 May 2017 12:17 Go to previous messageGo to next message
rachaelp
Messages: 583
Registered: March 2015
Location: UK
Senior Member
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


Re: label of supply symbols [message #170447 is a reply to message #170438] Fri, 12 May 2017 17:53 Go to previous messageGo to next message
Jorge Garcia
Messages: 1294
Registered: April 2010
Senior Member
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>
Re: label of supply symbols [message #170448 is a reply to message #170447] Fri, 12 May 2017 18:07 Go to previous messageGo to next message
rachaelp
Messages: 583
Registered: March 2015
Location: UK
Senior Member
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 Smile

Re: label of supply symbols [message #170458 is a reply to message #170447] Sat, 13 May 2017 09:31 Go to previous message
Marco Trapanese
Messages: 297
Registered: May 2007
Senior Member
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
Previous Topic: DesignLink: Getting Started?
Next Topic: Eagle start up from short cut link on my Deck top
Goto Forum:
  


Current Time: Wed Jul 26 12:40:30 GMT 2017