importing sch and board into project

Jamie Morken schrieb:

Is it possible to import a schematic and board layout from one eagle cad

project into another?  I have a circuit and placed layout that I would

like to maintain the layout of and paste into another schematic/board.

The easiest way is to start the new design from a copy of the old one.

If that is not possible, you must GROUP/CUT/PASTE the schematic and

board parts separately, and for this temporarily close the other editor

window to turn annotation off. After having copied both parts, open the

second editor again and run ERC. Be prepared to fix some (eventually

many) inconsistencies.

Tilmann

Hi,

the help file list the following for the PASTE command:

wrote in message

news:g139gc$nbv$1@cheetah.cadsoft.de...

Jamie Morken schrieb:

 

Is it possible to import a schematic and board layout from one eagle cad

project into another?  I have a circuit and placed layout that I would

like to maintain the layout of and paste into another schematic/board.

 

The easiest way is to start the new design from a copy of the old one.

 

If that is not possible, you must GROUP/CUT/PASTE the schematic and

board parts separately, and for this temporarily close the other editor

window to turn annotation off. After having copied both parts, open the

second editor again and run ERC. Be prepared to fix some (eventually

many) inconsistencies.

 

Tilmann

Hello Tilmann Reh !:

Is it possible to import a schematic and board layout from one eagle cad

project into another?  I have a circuit and placed layout that I would

like to maintain the layout of and paste into another schematic/board.

 

The easiest way is to start the new design from a copy of the old one.

Be careful. If the source design was made by an illegal Eagle copy you

have to expect some serious troubles in the future.

I am not sure but maybe CadSoft willchange this philosophy. At the

moment it is better to be extremely careful.....

regards

--

Grzegorz Zalot

complex ltd.

office tel/fax : +48 32 2505840

mobil : +48 501 301515

Carsten Wille wrote:

Hi,

 

the help file list the following for the PASTE command:

 

<quote>

Function

Copies the contents of the paste buffer to a drawing.

 

Syntax

 

PASTE .

 

Mouse keys

 

Center mirrors the contents of the paste buffer.

Right rotates the contents of the paste buffer.

 

See also CUT, GROUP

 

Using the commands GROUP, CUT, and PASTE, parts of a drawing/library can be

copied to the same or different drawings/libraries. When using the PASTE

command, the following points should be observed:

 

  a.. CUT/PASTE cannot be used in device editing mode.

  b.. Elements and signals on a board can only be copied to a board.

  c.. Elements, buses and nets on a schematic can only be copied to a

schematic.

  d.. Pads and smds can only be copied from package to package.

  e.. Pins can only be copied from symbol to symbol.

  f.. When copying elements, signals, pads, smds and pins, a new name is

allocated if the previous name is already used in the new drawing.

  g.. Buses retain the same names.

  h.. Nets retain the same name as long as one of the net segments has a

label. If no label is present, a new name is generated if the previous name

is already in use.

If there are modified versions of devices or packages in the paste buffer,

an automatic library update will be started to replace the objects in the

schematic or board with the ones from the paste buffer. Note: You should

always run a Design Rule Check (DRC) and an Electrical Rule Check (ERC)

after a library update has been performed!

 

</quote>

 

 

 

As Tilmann wrote, you have to cut and paste separately schematic and board.

But the clue is the last item in the bullet list: Eagle's behavoir of

renaming nets.

 

My way of doubling parts of board and schematic is:

 

step0: Make a backup just in case.

 

step1: Have both, sch and brd open. Use the schematic to edit.

 

step2: Name all signals (and I mean really all) with a net name that ends on

a letter. E.g. N$17 -> N$17A. All copied net name will change from N$17A to

N$17A1 etc.

 

step3: Attach label to all signals you do not want to change in the copy.

(Esp. VCC and GND)

 

step4: Save

I've only really found the  net re-naming to be necessary when I took a

design , deleted a lot of it, to give the section I wanted to copy, and then

went to do the copy /paste routine. As the net names  were not continuous

this threw up a few problems and a lot of inconsitencies crept in...

In most cases with a reasonabley fresh design this stage is not required.

However if you do want to re-name all your nets then have a look at the

ULP's in merge_brd.zip.

One renames all nets by adding a suffix automatically.

The other is a re-name ULP for components that also allows for an offset in

the number to be added. IN many situations renaming the components is

important to ensure you have a clean sequence with no holes in it, which can

throw up some problems occasionally.

I didn't write either of these ULPs- just modified them to meet my own

requirements at the time.

there are a couple of other ulps that look interesting but I've not used them

cheers

David