combine two designs into one project

If all you want is the schematic copied into an exsting design, then that's fairly easy.

Draw a 'group' around all the parts you want and hit the 'cut' button (which does not 'cut' but instead 'copies' the group to the paste buffer) then right-click on any part of the group and select 'cut group'.

Now close that schematic and open the destination schematic and press the 'paste' button. Voila. done.

If you need to copy the schematic AND the layout, then it becomes a bit more tricky. You must first of all make sure that all the components on both schematics have unique names. There must be NO names existing on both schematics before the copy. Then do the same as above, to copy the schematic. The close the schematic and do the same cut-and-paste with the board.

I hope this helps.

"Kenny Millar" <communitymanager@premierfarnell.com> wrote in message

news:117449697.20671282859075727.JavaMail.jive@flcspu-csapp-01.premierfarnell.com...

If you need to copy the schematic AND the layout, then it becomes a bit

more tricky. You must first of all make sure that all the components on

both schematics have unique names. There must be NO names existing on both

schematics before the copy. Then do the same as above, to copy the

schematic. The close the schematic and do the same cut-and-paste with the

board.

And then fix by hand, one by one, ERC errors, since in 99% of cases the new

full schematic will not be consistent with the new full board, due to

different names added by defaults to components and nets.

It's faster to start from scratch, if there are more than 10 components to

move.

"Mike Wilson" <mail4mikew@gmail.com> wrote in message

news:i56ium$mfl$1@cheetah.cadsoft.de...

Hello!

>

I'm sure that there is probably an easy way to take the contents of one

design and copy them into another... I haven't a clue how though. I am

currently looking through the ULP's @ cadsoft. Can anyone point me in the

right direction?

>

Mike

"merging_v21.zip" is specifically for that. (Eagle Homepage --> Download -->

Ulps)

Read carefully the instructions.

Maurice

Ha ha, I was just writing a reply on my experience with

"merging_v21.zip"! I'll have it up in a few minutes - Thanks BTW, it

works nice.

Mike

On 8/27/2010 8:54 AM, Maurice wrote:

"Mike Wilson"<mail4mikew@gmail.com>  wrote in message

news:i56ium$mfl$1@cheetah.cadsoft.de...

>> Hello!

>>

>> I'm sure that there is probably an easy way to take the contents of one

>> design and copy them into another... I haven't a clue how though. I am

>> currently looking through the ULP's @ cadsoft. Can anyone point me in the

>> right direction?

>>

>> Mike

>

"merging_v21.zip" is specifically for that. (Eagle Homepage -->  Download -->

Ulps)

Read carefully the instructions.

>

Maurice

>

>

>

On 8/26/2010 1:31 PM, Mike Wilson wrote:

Hello!

>

I'm sure that there is probably an easy way to take the contents of one

design and copy them into another... I haven't a clue how though. I am

currently looking through the ULP's @ cadsoft. Can anyone point me in

the right direction?

>

Mike

I had a design (Rev A), that I needed 2nd prototypes for (the design

includes 3 boards, joined with break-aways), but only one board. So I

separated out the one board (Rev B). However, the customer desires that

all three boards be togther, so I needed to import the changes of Rev B

back (with other changes), to create Rev C.

I ended up removing the (old) Rev B contents from Rev A, and then using

merging_v21.zip from (Eagle Homepage --> Download -->

Ulps --BIG THANKS TO MAURICE!) to merge Rev B back into Rev C. The

process is described in the notes in the .zip, and it isn't very

cumbersome at all. Took me about 5 minutes to do it - the first time...

I had to go through the process a few times to have decent success. It

came down to what others have mentioned:

1.) Get all of the components to have unique identifiers, or,

merging_v21 can create new identifiers.

2.) Get the nets to have unique names from the destination design,

unless you want the imported nets to connect with the destination design.

3.) Evaluate the libraries - If you are not sure if the libraries used

in the two designs are the same (mine were not), then do this (there are

probably better ways, this worked for me, but maybe it just happened to

work):

- export the parts from the source design to a new library, in it's own

directory (using exp-project-lbr.ulp, create a single library).

- point the eagle directory for libraries on the destination project to

the directory with the new library.

4.) Save the destination project, and back it up. If there are any

problems, you can alway exit without saving, I did this 3 or 4 times

until I had a good transfer the way I liked it.

5.) NOW export/import the design changes according to the instructions

in merging_v21.

I had a few problems with GND nets, and power supply nets, there were a

number of warnings when merging to the destination, but once I

understood what they were about, they were no big deal other than

clicking through the warnings.

merging_v21 had a bug? that caused some warnings/errors when it created

library parts (needed to identify what parts of the original to copy),

but they seems to have no negative effect on the output. Unfortunately I

did not record these errors.

The other issue I had was that the silkscreen labels changed sizes in

the transition, and were no longer smashed in the destination. I had

well over 30 parts, and a complicated routing with curved traces and

such, and REALLY did not want to lose that work, this was a real time

savior for me.

Thanks again Maurice, that worked well.

Mike

I have been using the merge ULP and scripts for many years...now in 4.11 I have issues, everything but the device itself is imported.

I wish that I was a programmer so that I could fix this, but what I have seemed to have found is that the ADD command syntax has changed.  I just cannot believe this, but the error that I get on a line like this (copied from the .scr file):

add 'ACT00' CHIPLED_0805@led R0.000000 (11.136000 11.012000) value 'AMBER' (11.136000 11.012000)

is

Package not found: ACT00

if I remove the 'ACT00' from the add command line, I get:

add CHIPLED_0805@led R0.000000 (11.136000 11.012000) value 'AMBER' (11.136000 11.012000)

and the error is:

Invalid parameter: AMBER

so I make the line

add 'ACT00' CHIPLED_0805@led R0.000000 (11.136000 11.012000)

and I get a part, but of course it is not named ACT00 and it does not have the value AMBER.

Anyone know what happened to the merging scripts?  Or what happened to the Eagle ADD command syntax from when this worked last (4.10???)

ANY help here would be good help!  Thanks!

Jim

Found the issue.  Not sure where this went sour, but the merging ULP generate the add command out of correct syntax for Eagle 4.11...have not gone back to 4.10 to see if this is the same problem, but I do remember using the merging scripts often...

OLD:

add 'ACT00' CHIPLED_0805@led R0.000000 (11.136000 11.012000)

NEW:

add CHIPLED_0805@led  'ACT00' R0.000000 (11.136000 11.012000)

All that was done was to swap the first and second data arguments (fields) in the add command.  Here are the two lines in the UPS for board and schematic that fix this:

export_board_v3.ulp line 80:

         printf("add %s@%s '%s%s' %s%sR%f (%f %f) \n",

         E.package.name,E.package.library, E.name,suffix,

         spin[E.spin],mirror[E.mirror],E.angle,xx1,yy1);

export_schematic_v3.ulp line 67:

               if(!first) printf("add %s@%s '%s%s' '%s' %sR%f (%f %f) \n",

                  P.device.name,P.device.library,P.name,suffix,

                  I.gate.name,mirror[I.mirror],ang,xx1,yy1);

And I was wrong, this is not part of the "add" line, this is a separate command that adds the VALUE property to the added device so that the netlist is correct between board and schematic.

THIS IS GOOD:

value 'AMBER' (11.136000 11.012000)

Hope this helps someone else!

Jim