Why do I need to draw the same symbol N times?

On 23.09.2016 06:32, Zoltán Kócsi wrote:

More often than not the same chip is available in different packages,

quite often with different number of pins and the packages with fewer

pins omit some of the lesser used signals.

 

Currently, you need to create a different symbol for every package: if

you have a chip that comes in 5 different packages, with a few pin

differences, you need a symbol drawn for ABC1234-SOIC, ABC1234-BGA,

ABC1234-TSOP and so on. It's the same damn chip, just on some packages

some pins are missing.

 

I wonder if I'm alone with the wish of having just one symbol, with

every possible signal drawn. Then, when it gets placed to the schematic

with a package selected, the not bonded pins grey out and don't allow

wires to be connected to them?

 

You dont need to redraw the symbol. You just create a new component and

add the symbol + all the packages that work with this symbol at the same

component, then connect them correctly. This works, even if some

packages have more gnd/shield pins, cause every package is connected

separately.

Look at the attached sample. I got one symbol and 5 different packages

for the same symbol.

But currently (7.x), if the symbol differs slightly betweeen packages,

you have to copy/make a new symbol, and add/remove pins. Sometimes it

would have been nice if unconnected pins at the symbol were hidden at

the schematics, if they are not user/connected to the chosen package.

Attachments:

Quote:

You dont need to redraw the symbol. You just create a new component

and

add the symbol + all the packages that work with this symbol at the

same

component, then connect them correctly. This works, even if some

packages have more gnd/shield pins, cause every package is connected

separately.

That won't work if one or more of the package variants has less pins than

the symbol.

It would help if the Table of Contents view of the library allowed copying

a symbol, so that you can draw the most extensive symbol for the component,

copy it, delete some pins from the copy (repeat for all variants).

The way I work around this is by drawing the symbol, saving the library and

exiting the library editor, then opening the library in a plain text

editor, find the symbol you just added, then copy/paste it (between ), with a modified name for the copied

symbol. Then reopen the library editor, edit the copied symbol and delete

the pins not used in that variant.

--

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

Rik Steenwinkel schrieb:

It would help if the Table of Contents view of the library allowed copying

a symbol, so that you can draw the most extensive symbol for the component,

copy it, delete some pins from the copy (repeat for all variants).

 

The way I work around this is by drawing the symbol, saving the library and

exiting the library editor, then opening the library in a plain text

editor, find the symbol you just added, then copy/paste it (between <symbol

name="..."> and </symbol name>), with a modified name for the copied

symbol. Then reopen the library editor, edit the copied symbol and delete

the pins not used in that variant.

Why don't you simply use GROUP - CUT - PASTE within the symbol editor?

Tilmann

On 23.09.2016 09:31, Rik Steenwinkel wrote:

Quote:

You dont need to redraw the symbol. You just create a new component

and

add the symbol + all the packages that work with this symbol at the

same

component, then connect them correctly. This works, even if some

packages have more gnd/shield pins, cause every package is connected

separately.

 

That won't work if one or more of the package variants has less pins than

the symbol.

 

It would help if the Table of Contents view of the library allowed copying

a symbol, so that you can draw the most extensive symbol for the component,

copy it, delete some pins from the copy (repeat for all variants).

 

The way I work around this is by drawing the symbol, saving the library and

exiting the library editor, then opening the library in a plain text

editor, find the symbol you just added, then copy/paste it (between <symbol

name="..."> and </symbol name>), with a modified name for the copied

symbol. Then reopen the library editor, edit the copied symbol and delete

the pins not used in that variant.

 

It works for many packages, not for all.

Your symbol should not have the same name over again, like multiple GND

pins. Just draw one and merge all the pins of a package onto the

same symbol pin. This way you can reuse a symbol for same-function packages.

I guess you do know you can use copy/paste to copy a symbol and paste it

onto a new one, then make changes. Just group all , copy group, create a

new symbol and paste.

Or paste these commands into the command line when you got the symbol

you want to copy open:

group all;

copy (>c0 0);

edit newname.sym;

paste (0 0);

All of a sudden you have a copy. (It doesnt copy the description tho)

Quote:

It would help if the Table of Contents view of the library allowed

copying a symbol, so that you can draw the most extensive symbol for the

component, copy it, delete some pins from the copy (repeat for all

variants).

It does... Right click on the symbol you want to copy and select

"Duplicate". It then asks you to enter a new name for the duplicate and

you're done.

--

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

rachaelp wrote on Fri, 23 September 2016 10:45

Stoneshop wrote on Fri, 23 September 2016 08:31

It would help if the Table of Contents view of the library allowed

copying a symbol, so that you can draw the most extensive symbol for

the component, copy it, delete some pins from the copy (repeat for all

variants).

 

It does... Right click on the symbol you want to copy and select

"Duplicate". It then asks you to enter a new name for the duplicate and

you're done.

Not in my version (7.3.0 standard). You can duplicate devices and packages,

but not symbols.

--

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

zoltan wrote on Fri, 23 September 2016 05:29

I wonder if I'm alone with the wish of having just one symbol, with

every possible signal drawn. Then, when it gets placed to the

schematic

with a package selected, the not bonded pins grey out and don't allow

wires to be connected to them?

Morten Leikvoll wrote on Fri, 23 September 2016 07:47

But currently (7.x), if the symbol differs slightly betweeen packages,

 

you have to copy/make a new symbol, and add/remove pins. Sometimes it

would have been nice if unconnected pins at the symbol were hidden at

the schematics, if they are not user/connected to the chosen package.

Yes I think this would be nice. For a lot of cases the existing system

works fine but being able to have a single device which deals with the

entire part in all its variants rather than having to have duplicate parts

with slightly different symbols would be a big benefit in terms of having

much tidier and easier to use libraries. I like the idea of greying out or

hiding unconnected pins but sometimes that might not be enough as a variant

can possibly change a pin function (i.e. it bonds the pin to another

function internally). For this reason I think being able to specify

alternative symbols within the device as well as alternative packages would

be a big benefit too.

Best Regards,

Rachael

--

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

Stoneshop wrote on Fri, 23 September 2016 09:54

Not in my version (7.3.0 standard). You can duplicate devices and

packages, but not symbols.

Yes they added a lot of new features to the library manager throughout the

7.x releases and I can't remember where that was added. If it's an issue

for you at least you have the option of going to a newer release as you

have a v7 license.

Best Regards,

Rachael

--

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

On Fri, 23 Sep 2016 08:47:48 +0200

Morten Leikvoll <mleikvol@yahoo.nospam> wrote:

You dont need to redraw the symbol. You just create a new component

and add the symbol + all the packages that work with this symbol at

the same component, then connect them correctly. This works, even if

some packages have more gnd/shield pins, cause every package is

connected separately.

As Rik Steenwinkel pointed out, that doesn't work with very many chips.

Microcontrollers, FPGAs, power supply chips being ominous examples.

Micros more often than not drop/gain a few port pins between package

variants. FPGAs ditto. Power supply chips often drop rarely used

feature pins. SPI FLASH chips tend to have a 'BUSY' signal on the higher

pincount package, which is dropped if you go to the smallest

pincount/footprint one. So the list is quite long.

In my original post I was specifically talking about packages with

different pin counts and signal pins going missing in the smaller

package.

But currently (7.x), if the symbol differs slightly betweeen

packages, you have to copy/make a new symbol, and add/remove pins.

Exactly. As it has always been the case. Hence my request: I'd like to

draw only one symbol and assign a package, even if the symbol has

more pins than the package. Then the schematics could grey out or even

completely hide the pins that are not available on the package.

In the software world copy-paste-massage-ing code is one of the cardinal

sins, and rightly so, why am I forced to do it with my hardware?

--

Zoltán Kócsi

Bendor Research Pty. Ltd.

zoltan wrote on Sun, 25 September 2016 01:53

Hence my request: I'd like to

draw only one symbol and assign a package, even if the symbol has

more pins than the package. Then the schematics could grey out or even

completely hide the pins that are not available on the package.

By the time you specify which pins should be greyed out, you might as well

have made the minor modifications from the symbol with a little more or

little less pins.  If you're only changing a few pins, there isn't really a

problem to solve here.

You don't want Eagle to just assume that you intentionally used a symbol

with too many pins and not show you the remaining ones.  That would

circumvent useful error checking.  Also, if a different chip has fewer

pins, you most likely want to draw the symbol differently.  You may want to

make it a little smaller, change some of the labeling inside the symbol,

etc.

A good example is a voltage regulator.  The simple 3-pin variety can be

drawn more simply and smaller than one with a shutdown input, for example.

I wouldn't want the simple 3-pin version burdened with a greyed out

shutdown input.  I also wouldn't want it drawn bigger with inexplicable

extra space in the 3-pin usage case.

If the symbols are similar except for a few pins, then there isn't really a

problem here.  Copy and edit works fine.  If the symbols are substantially

different, then you're going to have to do some work for each case one way

or the other.

Quote:

In the software world copy-paste-massage-ing code is one of the

cardinal

sins, and rightly so,

Exactly.  This is the same thing.  Just like with software, you copy and

paste, then make a few minor edits to adapt to details of the situation.

--

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