3
\$\begingroup\$

I made 6 different sensors , unfortunately they are separate designs, and it cots more for production as well.

I tested the prototypes and everything is working perfectly. So i dont want to change the component locations and traces.

Is there any simple way to put all those PCB files to one design as single PCB?

I tried copy and paste tools but didn't worked !

\$\endgroup\$
  • 2
    \$\begingroup\$ Your board fab (board maker) should be able to do this for you, maybe for a small charge. \$\endgroup\$ – Steve G Aug 31 '16 at 9:04
  • 1
    \$\begingroup\$ cant we make it ourselves? \$\endgroup\$ – Sanu - Open Maker Aug 31 '16 at 9:07
  • \$\begingroup\$ When you tried "copy and paste" in what way did it not work? \$\endgroup\$ – Steve G Aug 31 '16 at 9:50
  • \$\begingroup\$ The schematic side is fine.. But doimd the same in pcb shows "can't back annotate this operation. Please do this in schematic \$\endgroup\$ – Sanu - Open Maker Aug 31 '16 at 10:57
  • \$\begingroup\$ Some board makers won't do what you want here- they'll charge a bunch extra if it looks like you've combined multiple designs. Since you don't want to fiddle with the design files at all, you could consider combining the Gerbers using a CAM tool. \$\endgroup\$ – Spehro Pefhany Aug 31 '16 at 11:21
5
\$\begingroup\$

You can combine designs onto a single board.

In the board editor, you can create a new board without an attached schematic -- and then copy all the separate layouts into this combined board. It is not necessary to copy all the schematics into a single schematic file.

One problem that occurs is that EAGLE will change reference designators on the silkscreen as necessary to avoid duplicates. The solution is to follow the same steps you would use to panalize a single board design. Run the panelize ULP (File > Run ULP... or Tools > Panelize) to create "shadow" silkscreen layers that contain the original reference designators before copying. These new layers (125 and 126) will allow duplicate reference designators.

Section Combining Small Circuit Boards on a Common Panel in the EAGLE user manual provides the detailed steps:

Load the board file.

Run panelize.ulp to copy name texts.

DISPLAY all layers.

Use GROUP to select all objects to be copied. To select the whole layout you could also use GROUP ALL.

Click the COPY icon in order to put the group into the clipboard.

Edit a new board file with File/New.

Use PASTE and place the layout as often as wanted. If necessary, it is possible to specify an orientation for the group before fixing it.

Please make sure that the new board has the same set of Design Rules as the original board file has. It is possible to export Design Rules into a file (*.dru) and then import it into another board file (Edit/Design rules menu, File tab).

Save the new board file.

Tell your board house that they have to use layers 125/126 instead of 25/26.

If you are planning to have the board scored or routed (with breakaway tabs) to make the boards easier to separate, those details -- and the overall board outline -- can go on the Dimension layer of the combined board file.

\$\endgroup\$
3
\$\begingroup\$

Export gerbers for the individual boards, then use gerbmerge to generate a combined set of Gerber files.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.