How to get new components on the PCB ???

Keld Sørensen wrote:

I have a schematic (A) witch board (B) I want to fit exactly to the

spot of the holes for some components from another schematic -

therefor I have copied the BOARD from this other schematic to my

project and want to use it as the board B.

 

Of cause I have to delete all the wiring and most of the components

but LEAVE the components I want to fit to.

 

Now I have the problem when I switch to board, that the components

from the schematic A is NOT to find at the board (B) - how can I some

kind of "update", so that the components from A is to find on the

board B ?

Eagle cannot do this simply.

How you proceed will depend on the number of objects you wish to place

precisely.

If you wish to replicate the board outline, a few mounting holes and the

accurate placement of a few parts then I would do it manually using Eagle to

deliver the precision.

Right now your schematic(A) and Board(B) are consistent. All your actions

need to retain that consistency.

Proceed, as you have, open a copy of the reference BOARD that has the

positioning you wish to replicate, removing all items that are not required.

Next we can use a ULP to get the details/positioning of the remaining

objects. Unfortunately there is no ULP to do the whole job.

Use the ULP export-board.ulp (download from cadsoft.- caution this is a v4

ULP but we can use it here for our purposes) The Script file that it creates

has all the information you require but you cannot just run that script for

a number of reasons.

If you ran the scr file 'as is' it would draw the board outline and any

mounting holes. It would then attempt to ADD (new)  the parts to the board

and will fail due to naming or library issues.

You need to modify the script to MOVE the equivalent board(B) part (your

part) to the same location

Open up the script file in a text editor.

Change the lines that start ADD

(1) Change ADD to MOVE

(2) Delete all the way up to the "("

So a line like

ADD 'D1' D0204-10@diode R180.000 (0.400 2.650);

becomes

MOVE 'D1' (0.400 2.650);

Next change the part name ('D1' in the above example) to match the part name

on your schematic(A) Board(B) so you move the correct part into position.

Save the script file

Open your project (schematic(A) Board(B))

Delete the default board outline on Board(B)

Run the script file in the Board(B) editor

You should see the board outline, holes and part placement of BOARD

You may have to manually ROTATE a part to get it correct.

You may care to LOCK those elements so you don't inadvertently move them

later.

In future when making daughter boards (Arduino shields are another example)

Start with / prepare a (seed) project you copy  to be your current

project.This has your board outline and connection headers done first.  Then

you continue to develop the schematic. Another approach is to make this

headers/board outline a library part.

HTH

Warren

--

Viewed and responded to from the newsgroup at

news.cadsoft.de

It is easy to create Libraries from Schematic and Board file by using ULP:exp-project-lbr.ulp from ULP folder in the path of EAGLE installation.