Eagle 5.1.1 wires/lines not editable

Robert Pearce wrote:

On Wed, 20 Jun 2012, Warren Brayshaw wrote to us saying :

>> The board may not get changed after a library modifircation for a

>> number of reasons

 

There's another one, I think, at least on V4.16 (it may have changed)

 

When you run exp-project-lbr it creates a library. When you have

"USE"d this library and updated all, even with the directory order

and unique names sorted, this does not cause any existing components

to be taken from the new library. So, for example, all the resistors

are still associated with the RCL library.

 

I don't know if that's a real problem for a component that originally

came from a library that you don't have.

--

Rob Pearce                       http://www.bdt-home.demon.co.uk

This, I think, is a caused by one of the conditions I mentioned.

exp-project-lbr  can export to multiple or a single library.

Exporting to multiple libraries

The parts on your board still refer to a library called RCL and will only

update from a library called RCL

With this in mind, to have them update, they have to find the new library

named RCL before finding the old RCL

This means the path to the new libraries, created with the export, has to be

in the directory path before the path to the old RCL. If not the old RCL

will provide the detaile for the update.

Exporting to a single library

Here you generate a single library with a new name.

An update all will not look into it as the board components never know of

this library.

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

On Wed, 20 Jun 2012, Warren Brayshaw wrote to us saying :

>The board may not get changed after a library modifircation for a number of

>reasons

There's another one, I think, at least on V4.16 (it may have changed)

When you run exp-project-lbr it creates a library. When you have "USE"d

this library and updated all, even with the directory order and unique

names sorted, this does not cause any existing components to be taken

from the new library. So, for example, all the resistors are still

associated with the RCL library.

I don't know if that's a real problem for a component that originally

came from a library that you don't have.

--

Rob Pearce                       http://www.bdt-home.demon.co.uk

The contents of     | All power corrupts, but we need electricity.

this message are    |

purely my opinion.  |

Don't believe a     |

word.               |

Guoliang Zhang wrote:

Now actually I can run a ULP called exp-project-lbr.ulp to generate a

library which does contains the mechanical only part that represents

the board. but still after i modified the library, use the library,

update the board layout, the board does not get changed. even worse,

if I add this as part from the schematic, a few extra board outlines

are added to the layout and I cannot delete them. what kind of 'part'

this is? how can I move or delete or edit it properly?

You add the part to the schematic and the board outlines appear in the board

editor, that is good. To delete them you need to delete the device in the

schematic editor.

If you run exp-project-lbr.ulp  in the board editor you only get packages.

Run it in the schematic editor and you get the full device.

The board may not get changed after a library modifircation for a number of

reasons

You must USE the library ( Ensure the Green dot is on. Sometimes it turns

off when modifying a library)

You should perform "Library update all " in the library and in the schematic

or board

If your new library has the same name as another. Only the fiirst folder

found, matching the library name, in a valid path will be searched for the

device.

The path of your library is not known to Eagle ( Options > Directory paths)

HTH

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

Am 20.06.2012 00:30, schrieb Guoliang Zhang:

Now actually I can run a ULP called exp-project-lbr.ulp to generate a library which does contains the mechanical only part that represents the board. but still after i modified the library, use the library, update the board layout, the board does not get changed. even worse, if I add this as part from the schematic, a few extra board outlines are added to the layout and I cannot delete them. what kind of 'part' this is? how can I move or delete or edit it properly?

 

I agree with the other guys that it must be a library part.

If you cannot find that part by switching off layers, exporting

(exp-project-lbr.ulp)a library amd scan that,then the "final" method of

destroying is needed.

Make a copy of that board!!! Here you select half of the board and

delete it. If that part is gone hit the restore button and delete a

different area. This way you can work forward until a few things are

left only. Exporting this "project" library should then point to the

library and part name.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

Now actually I can run a ULP called exp-project-lbr.ulp to generate a library which does contains the mechanical only part that represents the board. but still after i modified the library, use the library, update the board layout, the board does not get changed. even worse, if I add this as part from the schematic, a few extra board outlines are added to the layout and I cannot delete them. what kind of 'part' this is? how can I move or delete or edit it properly?

If that is the case, when I generate a part list from the File/Export... option, do I see the library from which this board is residing? I did just that and could not find the board listed in any place of that list. Is there a way to tell where the board library is or what name it is? The brd file is binary, I have no way to figure out the hierachy.

Thanks

GZ

Guoliang Zhang wrote:

Hi, forum,

 

I inherited a project from someone who left the company a while back.

when i tried to do some modifications to the dimention and keepout

layer, i have the trouble not being able to edit any of the lines.

these are visible boarders/fills/polygons but no way to click through

or get high-lighted, just as if they do not exist. Any obvious reason

that can cause such lock down?

 

Thanks

GZ

Maybe the bare board was built as a library part and potentially it is

"Locked" . If you cannot get an Information dialog to display for the

dimension wire then this is likely.

HTH

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de