Device unlinked from library, how to detect?

On 5/6/2014 7:11 AM, Morten Leikvoll wrote:

This problem is very old. Sometimes I upgrade my libraries and give

devices a new name. Sometimes I delete buggy devices.

 

When I from a project use the "library->update all" funcion, I get no

notifications of the placed components that doesn't exist in library

anymore. That is scary.

This would be an interesting point to discuss. In EAGLE, once a part is

brought into a design it is completely independent of its parent

library. The only thing linking them at that point is basically the

library name.

What is scary about this behaviour? No data can be lost since as long as

you have the part in a design you can always recover part into a library.

 

When I (from the v6 contect menu) choose "open device" I get the error:

"Package variant 'xxx' of deviceset yyyy does not exist in current

library <library filename>. Please adjust the library path or export the

drawing libraries first!"

I do not want to do this for every part present on my brd/sch. It is

possible to write an ULP to find them, but I think it should be part of

the library update function.

It's important to remember that Update all checks only libraries that

are in the paths specified in the Control Panel -> Options ->

Directories. If you're library is stored outside of those directories

you'll get the same error.

hth,

Jorge Garcia

Jorge Garcia wrote on Tue, 06 May 2014 16:01

On 5/6/2014 7:11 AM, Morten Leikvoll wrote:

This problem is very old. Sometimes I upgrade my libraries and

give

devices a new name. Sometimes I delete buggy devices.

 

When I from a project use the "library->update all" funcion, I get

no

notifications of the placed components that doesn't exist in

library

anymore. That is scary.

This would be an interesting point to discuss. In EAGLE, once a part is

 

brought into a design it is completely independent of its parent

library. The only thing linking them at that point is basically the

library name.

 

What is scary about this behaviour? No data can be lost since as long

as

you have the part in a design you can always recover part into a

library.

 

When I (from the v6 contect menu) choose "open device" I get the

error:

"Package variant 'xxx' of deviceset yyyy does not exist in current

library <library filename>. Please adjust the library path or

export the

drawing libraries first!"

I do not want to do this for every part present on my brd/sch. It

is

possible to write an ULP to find them, but I think it should be

part of

the library update function.

It's important to remember that Update all checks only libraries that

are in the paths specified in the Control Panel -> Options ->

Directories. If you're library is stored outside of those directories

you'll get the same error.

Jorge,

What is scary ?  How is that all not considered very scary?  For anyone who

had designed boards this is a nightmare because you lose control over being

able to deterministically understand what is happening to your design

during a library update.

I've posted about this many times.  The library update needs to provide a

full report.  That should include at least:

what parts were found and identical (and therefore didn't change)

what parts were not found in the library

what source libraries were not found

what parts were updated and what the changes were

I've had boards come back not functional because a device name was changed

in the library after it was added to the schematic.  After that, the

library update will quietly ignore that part but won't tell you about.  So

you can make changes to the device in the library (the master copy) but it

won't make it into your current design.  So the board comes back wrong if

you don't catch it.

Now I should have checked and caught that.  In that case a lot of things

had changed and I had checked all the other library changes but forgot to

check that one.  But isn't the tool supposed to be help in exactly these

cases where the task can be automated.

So please CadSoft, don't blow this request off.  This is a real issue that

happens in the real world and it would be so easy to address.

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

Take advantage of v7 License Promotion right now at

http://www.eaglecentral.ca

--

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

"James Morrison"  skrev i nyhetsmeldingen: lkbtsa$4q0$1@cheetah.cadsoft.de

...

What is scary ?  How is that all not considered very scary?

Thanks for the support. We agree on the severity of this issue, but I dont

have same requirement for documentation, especially if there is no change

(but it would be a nice option).

Mainly I need to know wich ones are not present in a used library anymore.

It could show the replace dialogue if one is missing (like if the

package/symbol has changed), with a "continue(dont update this device)"

button.

I guess undo will work, so the need for an action list for every device

before executing the changes is not something I miss, but would be nice.

Regards,

Hi,

Am 07.05.2014 10:11, schrieb Morten Leikvoll:

Mainly I need to know wich ones are not present in a used library

anymore.

This one is already in EAGLE since >= 6.5.2, from UPDATE_en.txt:

"Library update: Information to the user about devicesets that are used

in schematic but can't be found in the corresponding update library."

James is absolutely right when requesting a full report. I'm missing

that as well. At least, they took the very first step. Hopefully we get

V6.6 some day...

Rene

"René König"  skrev i nyhetsmeldingen: lkcrgi$kpj$1@cheetah.cadsoft.de ...

Am 07.05.2014 10:11, schrieb Morten Leikvoll:

Mainly I need to know wich ones are not present in a used library

anymore.

This one is already in EAGLE since >= 6.5.2, from UPDATE_en.txt:

"Library update: Information to the user about devicesets that are used

in schematic but can't be found in the corresponding update library."

Cool! I guess I have to update to 6.5.2 beta. Thanks

Regards,

"Morten Leikvoll"  skrev i nyhetsmeldingen: lkcush$7ce$1@cheetah.cadsoft.de

...

"René König"  skrev i nyhetsmeldingen: lkcrgi$kpj$1@cheetah.cadsoft.de ...

Am 07.05.2014 10:11, schrieb Morten Leikvoll:

Mainly I need to know wich ones are not present in a used library

anymore.

This one is already in EAGLE since >= 6.5.2, from UPDATE_en.txt:

"Library update: Information to the user about devicesets that are used

in schematic but can't be found in the corresponding update library."

Just tried it but something looks bugged.

I got a mismatch on a FPGA:

quote

Following devicesets are used in schematic but have not been found in the

corresponding update library:

Altera.lbr 4SGX180_F1152

If this is not intended, adjust the library paths or library deviceset names

and update again.

unquote

I tried replacing it, and even change package, but I still get same mismatch

after update all.

Also tried the same after renaming the altera.lbr to altera2.lbr. Still

mismatch.

Also tried dropping libs and using them again.. Still mismatch..

The Altera.lbr contains the device 4SGX180_F1152 with package name

4SGX_F1152, and a pile of symbols with different names wich I believe are

unchanged.

Any ideas?

Regards,

For the interested, Walter found the cause of this issue.

At "update all", v6.5.4 Beta scans the entire library paths for the library

name (even those not in use). In my case it saw the same library name in a

different folder, and compared it with that.

I suspect this will be fixed in a future version.

On 9/05/2014 7:03 p.m., Morten Leikvoll wrote:

For the interested, Walter found the cause of this issue.

 

At "update all", v6.5.4 Beta scans the entire library paths for the

library name (even those not in use). In my case it saw the same library

name in a different folder, and compared it with that.

 

I suspect this will be fixed in a future version.

 

This has been mentioned before, by me, only 4 weeks ago.

Same part name in another library folder on another path in your

directory options and you get the update from the first one that matches.

The libraries are searched in the order they are specified in the

directories settings.

What should be changed for an 'Update all' is the matching should

continue to the end of all libraries and the user advised if there is a

second match and not perform update until you advise which one you want.

Of course, you should manage your libraries so there are no duplicates

of library name and part but novices will often so this when they are

unaware of the trap.

Warren

"warrenbrayshaw"  skrev i nyhetsmeldingen: lki0aa$lun$1@cheetah.cadsoft.de

...

This has been mentioned before, by me, only 4 weeks ago.

Same part name in another library folder on another path in your directory

options and you get the update from the first one that matches.

Sorry for not catching it.

The libraries are searched in the order they are specified in the

directories settings.

What should be changed for an 'Update all' is the matching should continue

to the end of all libraries and the user advised if there is a second match

and not perform update until you advise which one you want.

Of course, you should manage your libraries so there are no duplicates of

library name and part but novices will often so this when they are unaware

of the trap.

My suggestion is simply to only scan libraries in use and report if several

of the projects devices come from a library that is not in use.

Your suggestion seems to open the door for a lot more bugs, and require a

lot more work, so maybe for a future version?

[quote title=Morten Leikvoll wrote on Fri, 09 May 2014

03:43]"warrenbrayshaw"  skrev i nyhetsmeldingen:

lki0aa$lun$mailto:1@cheetah.cadsoft.de

...

This has been mentioned before, by me, only 4 weeks ago.

Same part name in another library folder on another path in your directory

options and you get the update from the first one that matches.

Sorry for not catching it.

Isn't that how it is supposed to work?  The directories in the Control Path

-> Directories settings are in order of priority from left to right.  As

soon as EAGLE finds a file that matches it stops looking.  This is true for

running scripts and ULP's as well as updating.

I agree, you should generally not have 2 libraries with the same name, but

if you do that is what the priority takes care of.  However, if you don't

know then I guess that could cause confusion.

If there was a full report at least you'd see what was updated and where it

came from.  Then it wouldn't be hidden at least.

Quote:

>The libraries are searched in the order they are specified in the

>directories settings.

>What should be changed for an 'Update all' is the matching should

continue

>to the end of all libraries and the user advised if there is a second

match

>and not perform update until you advise which one you want.

>Of course, you should manage your libraries so there are no duplicates

of

>library name and part but novices will often so this when they are

unaware

>of the trap.

 

My suggestion is simply to only scan libraries in use and report if

several

of the projects devices come from a library that is not in use.

Your suggestion seems to open the door for a lot more bugs, and require

a

lot more work, so maybe for a future version?

I don't think the libraries "in use" should be the qualification for what

is searched.  The "use" command really only tells EAGLE which libraries to

consider when adding parts.  But I could easily (and often do) "use" a

library to add a couple parts and then remove it from "use" because I know

I don't want any more parts from that library.  And the more libraries are

in use, the longer it takes for the Add Device dialog to appear.  So I

would often have devices in my designs that are not part of libraries that

are in use at the time of the update.

I think EAGLE should, for each device in the design, look for that device

in all of the libraries that can be found in the EAGLE Library Directories

(as specified in Control Panel).  If it finds a match for device name and

library (that matches the library reference in the device itself) then it

goes ahead and tries to update.  Anything else should not be updated.

And of course a full report should be created of what happened during the

update for EVERY device in the design.  The idea is that the designer

should have full knowledge of exactly what happened during the update and

exact HOW each device changed or why it did not change.

There are two things that the "update all" command needs to look for:

device and library (that is referenced by the device).  Only if it finds

both should it replace the part.  If it actually looking into other

libraries that is not correct and should be fixed immediately.

CadSoft, please think like a designer about this.  I have designs with

close to 1000 parts and when I do "update all" there is no possible way I

can ensure currently that one specific change I made was included in the

update.  And as I stated, even as a veteran designer and EAGLE user, I

still had a board come back non-functional about 6 months ago because of

this issue.

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

Take advantage of v7 License Promotion right now at

http://www.eaglecentral.ca

--

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