How to change libraries after routing

On 29/07/14 17:51, Robert Scott wrote:

That would do it.  But the library I got the part from is an

Eagle-supplied library, and I don't want to get into the maintenance

headache of tracking changes to Eagle libraries.  I would much rather

make a duplicate of the part in a custom library of my own, and then

have the part reference my custom library for updating instead of the

Eagle library.  But I don't know how to do that without disturbing the

routing to the part on the PCB.  It is only the schematic that should

be affected.  Is there any way out of this short of editing the Eagle

library this part came from?

Well, one fairly obvious (and widely recommended) approach is...

Make a copy of (all of) the Eagle libraries. Put them somewhere

editable, either in your user area (if you're a one-man-band) or a

shared project area (if you're part of a team).

Now edit those libraries as you like.

Change the directory settings in Eagle to pick up your customised

libraries before (or instead of) the distribution copies.

Now you can update your design as if you'd edited the Eagle library but

without actually doing so. The design stores only the name of the

library, not the full path.

Hi,

It's possible to change your symbol without risk and it's quite easy.

• Start to create a new library, (or open one of your own library). Usually I name it in a way that It could not be mistaken with Eagle's ones, and I store it in an other directory.
• Then, while your library is open, search in the control panel the device you want to modify. Use a right-click on this device, and select copy to library. This will copy the component into your library (symbol+device+package(s)).
• You can edit your device and change the symbol, rename it etc...
• You save your library.
• You open your schematic (and board) if they don't, and you use the replace tool, to replace the device (from original library) with the device of your new library.
• In that way you keep the eagle's librarys clean, and you limit the risk, since you just edit an 'already good' device.

Be careful:

If you have changed the symbol, but not the names of the pins of the symbol, Eagle will adapt the new symbol, and there will be no change in you board. In the schematic you may re-arrange your wire, because it could look messy (but there will no mix-up in the net list) .

If you changed the pin names of your symbol, Eagle will try to retrieve the pin by their location. So If you want to change the pin names and their position, the best way would be to it in 2 separate steps, first just renames pin, replace your device with the new version. Then edit again you new library, change the symbol, but not the pin names. Then in you project, proceed a library update.

If Eagle can not replace with the new symbol without risk of mix-up, Eagle will display a warning or error.

Good luck.

Quote:

But the library I got the part from is an Eagle-supplied library,

There's the real problem.  Some mistakes can't be fixed after the fact.

This is one of them.

Next time think of this before painting yourself into a corner.  The advice

not to use the Eagle libraries directly is given here often, and should be

obvious from a little thought anyway.

That all said, changing one part is not likely to rip up a lot of the

routing.  If I remeber right, the ripup will only go as far as the next

part or net junction.

--

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

On Tue, 29 Jul 2014 18:06:30 GMT, Guillaume barrey

<noreply-198664@element14.com> wrote:

You open your schematic... and you use the

replace tool, to replace the device (from original library) with the

device of you new library.

How studid of me.  I never noticed that tool before.  Now that I know

that it exists, it is the perfect solution to my question.  Thanks.

Robert Scott

Hopkins, MN

 

That all said, changing one part is not likely to rip up a lot of the

routing.  If I remeber right, the ripup will only go as far as the next

part or net junction.

if we simply replace with the device of the new library and If only the symbol is changed, there will be no ripup at all. But if a wire is no longer connected to the same net, the ripup stop at first junction or part.

On 07/29/2014 02:30 PM, Olin Lathrop wrote:

Quote:

But the library I got the part from is an Eagle-supplied library,

 

There's the real problem.  Some mistakes can't be fixed after the fact.

This is one of them.

 

Next time think of this before painting yourself into a corner.

Robert,

It's not as bad as Olin infers.  There's a way to do this without

disturbing your layout.

Try this:

I couldn't find where Eagle keeps the path to the library stored in the

schematic, but it does keep the name of the library.  Thus, this stands

a good chance of working.  You could copy the eagle library in question

to your own personal lbr directory WITHOUT changing the name.  Make sure

your personal directory occurs before the eagle directory in the library

directory path.  Drop the eagle library from use, and use yours

instead.  Then modify the symbol, save it, and do a library update.

I've done this with the RCL library (and others) with success across

updates and upgrades.

If that doesn't work, try this:

Open your personal library and copy the DEVICE from the eagle library to

yours.  Modify the symbol as needed and save it.  Add this personal

library to your USE list.  Then replace the device on your schematic

with the device in your personal library.

Neither one of these methods should change the board layout, provided of

course, that the package is identical.  No rip-up and reroute should be

required.  That said, do a ratsnest to check for air wires and drc just

to be sure.

HTH,

    - Chuck

EAGLE stores everything in the board and schematic files.  I'd suggest

using the exp-lbrs.ulp to extract the libraries back out from your design

into a local directory, then make your changes and use the "update" command

to pull them back in...

--

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