G$1 next to reference designator, how to get rid of this?

How many gates (symbols) are there in your device and what are their add

levels?

Zoran wrote:

How many gates (symbols) are there in your device and what are their add

levels?

There are three:

A Schmitt inverter, add level "Next"

A power symbol, add level "Can"

A no-connect symbol, add level "Can"

I have set the add levels to other entries, no luck, that darn G$1

always shows up.

--

Regards, Joerg

http://www.analogconsultants.com/

Try changing a power symbol and no-connect symbol add level to 'request'

and leave the inverter at 'next'. When adding the part to the schematic,

only the inverter gate will be added and you will have to invoke the

other two if you want them placed.

'G$#' is an automatic gate name that Eagle sets when adding a symbol to

a device, where # is the gate number. When having multiple 'next' or

'can' gates of the same device in a schematic, a gate name is appended

to the part name, that's why you are getting 'U6G$1'.

You might also want to rename the gate from an automatic 'G$1' to

something more meaningful, e.g. '-#'; that way you would have something

like that when adding several 'next' or 'can' gates from one device:

'U6-1', 'U6-2', 'U6-3', and so on.

I hope this helps.

Zoran

Zoran wrote:

Try changing a power symbol and no-connect symbol add level to 'request'

and leave the inverter at 'next'. When adding the part to the schematic,

only the inverter gate will be added and you will have to invoke the

other two if you want them placed.

 

'G$#' is an automatic gate name that Eagle sets when adding a symbol to

a device, where # is the gate number. When having multiple 'next' or

'can' gates of the same device in a schematic, a gate name is appended

to the part name, that's why you are getting 'U6G$1'.

 

Thank you, Zoran, that did the trick! Strange thing is, I've looked in

other libraries for clues and there are cases where it's the same, main

symbol with "next" and the power with "can", and it works. But, main

thing is, the G$1 is gone.

You might also want to rename the gate from an automatic 'G$1' to

something more meaningful, e.g. '-#'; that way you would have something

like that when adding several 'next' or 'can' gates from one device:

'U6-1', 'U6-2', 'U6-3', and so on.

 

Usually with multipart symbols I use A, B, C, and so on.

I hope this helps.

 

It sure did

--

Regards, Joerg

http://www.analogconsultants.com/

Strange thing is, I've looked in

other libraries for clues and there are cases where it's the same, main

symbol with "next" and the power with "can", and it works.

That's strange because 'next' and 'can' are essentially the same except

for the fact that 'next' is added automatically with ADD command and

'can' can only be added with INVOKE. Gate numbers should be there. Or

maybe I must brush up on this a little

But, main thing is, the G$1 is gone.

Good Just remember to invoke and connect the power pins if they are

not already implicitly connected to the supply.

Zoran

Zoran wrote:

>> Strange thing is, I've looked in

>> other libraries for clues and there are cases where it's the same, main

>> symbol with "next" and the power with "can", and it works.

 

That's strange because 'next' and 'can' are essentially the same except

for the fact that 'next' is added automatically with ADD command and

'can' can only be added with INVOKE. Gate numbers should be there. Or

maybe I must brush up on this a little

 

>> But, main thing is, the G$1 is gone.

 

Good Just remember to invoke and connect the power pins if they are

not already implicitly connected to the supply.

 

Since I do analog stuff I have to almost always invoke the power pins.

But there Eagle has a bug, at least 4.16 does: When you invoke power

pins they show up with the refdes U6P (or U6G$2 if nothing was edited).

Very ugly when you scoot it over the device symbol. You can smash, move

and delete but this does not "stick", then the U6P pops right back up.

Entering a blank for the power pins in the library editor doesn't work,

it requires that something is entered.

--

Regards, Joerg

http://www.analogconsultants.com/

Joerg wrote:

Zoran wrote:

>>> Strange thing is, I've looked in

>>> other libraries for clues and there are cases where it's the same,

>>> main symbol with "next" and the power with "can", and it works.

>>

>> That's strange because 'next' and 'can' are essentially the same

>> except for the fact that 'next' is added automatically with ADD

>> command and 'can' can only be added with INVOKE. Gate numbers should

>> be there. Or maybe I must brush up on this a little

>>

>>> But, main thing is, the G$1 is gone.

>>

>> Good Just remember to invoke and connect the power pins if they

>> are not already implicitly connected to the supply.

>>

>

Since I do analog stuff I have to almost always invoke the power pins.

But there Eagle has a bug, at least 4.16 does: When you invoke power

pins they show up with the refdes U6P (or U6G$2 if nothing was

edited). Very ugly when you scoot it over the device symbol. You can

smash, move and delete but this does not "stick", then the U6P pops

right back up. Entering a blank for the power pins in the library

editor doesn't work, it requires that something is entered.

 

--

Regards, Joerg

 

http://www.analogconsultants.com/

Your answer may lay in a similar question I asked in this post.

http://www.eaglecentral.ca/forums/index.php/m/131169/c6b26c5fc772ccae538bde44e40f0b15/#page_top

Or search for the topic in eagle.suggest.eng

Enhancement to ADDLEVEL to prevent gate name being appended

It would be good to have the ability to prevent the gate name being

appended

to the gate, and thus reduce schematic clutter.

...

Klaus replied

Just use the ">PART" placeholder in your symbol instead of ">NAME".

HTH

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

But there Eagle has a bug, at least 4.16 does: When you invoke power

pins they show up with the refdes U6P (or U6G$2 if nothing was edited).

Power pins that are part of a device are also symbols like any other

gate. If a symbol contains a text variable e.g. >NAME or >VALUE, it will

be displayed in the schematic. So if you don't want these texts

displayed, you have 2 options:

- smash each part in the schematic and delete the texts, or...

- remove the texts in the symbol if you don't need them anywhere at all.

Name and value will get back if you unsmash (shift+smash) the part.

That's how it works in 6.2, I can't tell for the 4.16, that was some

time ago...

The only thing you can't smash is a pin / pad name, but you can choose

to display the pin name, the pad name, both, or none (off).

Entering a blank for the power pins in the library editor doesn't work,

it requires that something is entered.

Each gate must have a name, just the same as any part in the schematic /

board, and spaces are not allowed.

You however don't have to display these names with >NAME text variable

if you don't want to.

Just use the ">PART" placeholder in your symbol instead of ">NAME".

This one I didn't know. Thanks!

@Joerg:

Just check Help->Editor Commands->TEXT where variables are explained.

Zoran

Zoran wrote:

>> Just use the ">PART" placeholder in your symbol instead of ">NAME".

 

This one I didn't know. Thanks!

 

@Joerg:

Just check Help->Editor Commands->TEXT where variables are explained.

 

Also search for >PART in the pdf Manual (found in the DOCS folder) where

examples of the use of  >PART and >GATE are shown.

--

Viewed / responded via the newsgroup at

news.cadsoft.de