After upgrading: "Part has inconsistent packages in schematic and board"

[Tbaker25]

Hello all!

I've been running EAGLE 5.x for years. I finally upgraded to 8.x when Autodesk acquired, and started the new subscription pricing. Much more reasonable, and I love Autodesk's approach (Big Fusion360 fan). 

Here's my problem. Every time I load an old 5.x file, I get an error similar to this:

Part U$5 has inconsistent packages in schematic and board (TQFP32-08 from atmel.lbr / TQFP32-08@1 from atmel.lbr)

These are usually custom libraries. It's always a xxx@1 in the board. If I delete the part off both the schematic and board, then place it again, all is right with the world. 

Since I have oodles of 5.x boards, any time I open one to do troubleshooting of an old board, etc, I get this inconsistency which makes trace highlighting to stop working. (Can't highlight a net in the schematic and then see it highlighted on the board)

Not the end of the world, but still annoying. Any ideas how to fix it?

Thanks!

Tom

[rachaelATWH4]

Hi Tom,

My first guess would be update all your libraries to v8 format by opening them in v8 and re-saving them, and then when you open an old v5 design do a 'Library->Udpate all' from the menus to force it to update and I would hope this would fix it.

But... You've been using EAGLE for years and are experienced so I'm guessing it's not going to be this simple.... If this doesn't work then maybe it would be possible to write a ULP which would speed up the process of removing and replacing the affected parts....

Alternatively, if you diff the v8 version of the design file before and after you make the fixes then maybe it would be possible to work out a way to fix the design file quickly with an external command line utility or even just a plain old text editor....

Best Regards,

Rachael

[Tbaker25]

Thanks, Rachael. 

Good ideas. I tried upgrading the library, but it didn't help. 

I'd love to fix the files in-place, but 5.x uses a binary format and 8.x uses XML. Makes it a little more complicated.

Thanks!

Tom

[rachaelATWH4]

---

tbaker wrote:

Good ideas. I tried upgrading the library, but it didn't help. 

---

That's unfortunate. That would have been an easy fix! 

---

@Anonymous wrote:

I'd love to fix the files in-place, but 5.x uses a binary format and 8.x uses XML. Makes it a little more complicated.

---

What I meant here was, open it in v8 and save it in an XML format. Then fix it with the method you used previously by manually replacing the offending parts, save that as a separate copy and finally you can diff the two and see what the changes are. Hopefully that will give some clues about easier ways to fix the issue.

Best Regards,

Rachael

[jorge_garcia]

Hi @Anonymous,

I hope you're doing well. The error you are describing is typical of an old bug in EAGLE that has since been fixed. The easiest solution is to save the designs in the new version of EAGLE.

Open the XML files in at text editor. Try doing a search for TQFP32-08@1 and replace it with TQFP32-08. Sometimes that's all it takes. If the packages internally are different then that can be more difficult.

Not all of your V5 designs will have this issue, it's not a common imperfection.

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

Best Regards,

[Tbaker25]

Thanks Jorge! Will do.
Tom

[Anonymous]

I have a similar problem "board and schematic are not consistent ", many components have some problem with 3d packages.

How to fix that?

[jorge_garcia]

Hello @Anonymous,

What version of EAGLE did you open this file in? If it's prior to V8 it has no clue about the managed libraries and the behavior is not predicatable. Additionally, the LTSpice library has never carried any 3D packages with it so I'm not 100% sure what's going on here.

If you could provide more details I would more than happy to help.

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

Best Regards,

[Anonymous]

Hi, I use latest version of the EAGLE

[rachaelATWH4]

What version of EAGLE were you using prior to updating to the latest version?

Did you do anything to your board or schematic like perform an update to the used libraries? If so were both the board and schematic open so back annotation was working?

Best Regards,

Rachael

[Anonymous]

Hah.  I had a similar problem, with a file saved with v6.x, trying to read in 7.x (yeah, I know, I'm way behind.)

A series of:

Part R1 has inconsistent packages in schematic and board (0207/7 from rcl.lbr / 0207/7 from rcl.lbr)

these were files that I hadn't looked at in a long time, and I was pretty sure I hadn't saved them, either.

Poking around in the XML files, I discovered that the .SCH file had:

<package name="0207/10">
<description>&lt;b&gt;RESISTOR&lt;/b&gt;&lt;p&gt;
type 0207, grid 10 mm</description>
<wire x1="5.08" y1="0" x2="4.064" y2="0" width="0.6096" layer="51"/>

While the .brd file had:

<package name="0207/7">
<description>&lt;b&gt;RESISTOR&lt;</description>
<wire x1="-3.81" y1="0" x2="-3.429" y2="0" width="0.6096" layer="51"/>

Note that the "description" definitions are different.

Manual modification of the .XML so that the descriptions matched fixed the problem.