"Block Copy" in Eagle PCB Layout

Question

Hi all, how does one do a "block copy" in Eagle Cad PCB Layout? I want to preserve/match the two circuits physical layout. Much appreciated, PietT

Richard_H · Answer

Am 19.07.2011 14:28, schrieb Pieter Swanevelder:

Hi all,

how does one do a "block copy" in Eagle Cad PCB Layout? I want to preserve/match the two circuits physical layout.

Much appreciated,

PietT

Frequently asked in the forum. Some quotes from previous postings:

==================

This can be done with the help of the commands GROUP, CUT, and PASTE.

Assumed you have consistent pair of schematic and board and you

would like to use one of your existing designs (also a consistent pair

of sch and brd) in the current project you could begin, for example,

with the schematic:

Open the schematic you want to use in your project and use the

commands GROUP and CUT to copy it into the clipboard

Now open the schematic of your current project. You will notice

that the layout editor opens the consistent layout file, too.

BUT YOU HAVE TO CLOSE IT AGAIN!

Now use the PASTE command in the schematic and place the

previously selected group.

That's it for the schematic.

Now the same procedure for the layout:

Open the board you want to put into the clipboard and use

DISPLAY ALL first to activate all layers.

Now: GROUP, CUT. Open the "target" layout and PASTE.

Now you have to run the ERC which compares schematic and layout.

This is necessary because it might happen that the names of parts or

nets are renamed while pasting them into the existing project.

ERC can check whether the new numbering in SCH and BRD is all the

same. In the case there are differences ERC reports this and you have

to adjust this manually. Until ERC reports consistency again.

=================

news://news.cadsoft.de:119/fn617k$j6$1@cheetah.cadsoft.de

eagle.support.eng, 2008-01-23, 01:20 AM by Mickey Reilley

The Procedure:

-

Sometimes circuit boards will have duplicate sections of schematic that you

want to layout identically. You could do this by laying out each section

separately, but for large or complex layouts this would be very time

consuming. Eagle does not have a function that allows you to directly

duplicate your layouts, so you have to use this workaround:

1. Create the schematic for the section you want to duplicate. You can have

additional schematic done at that time too if you like.

2. Create the layout for that section. You can have additional layout done

at that time if you like.

3. Close the layout so that you only have the schematic open.

4. Use the window selection tool to surround the section of schematic you

want to duplicate in the layout.

5. Use the scissors tool to copy the selection to the buffer.

6. Use the dropdown EDIT: PASTE to finish the copy operation.

7. Save the schematic and close it.

8. Open the layout. Click OK to acknowledge the warning about the schematic

and board not being consistent. Close the schematic that opened when you

opened the layout so that you only have the layout open.

9. Do the same window select, scissors, paste operation on the layout. YOU

MUST COPY EXACTLY THE SAME ITEMS AS YOU DID IN THE SCHEMATIC. THIS INCLUDES

COMPONENTS AND NETS.

10. Save the layout and open the schematic. You should have both the

schematic and layout open at this point.

11. In the layout, run ERC and you'll get a long list of nets that don't

match. Don't worry: you only have to fix each net once. This is usually

only 5 or 6 nets to fix the whole list.

12. The original section of layout will have nets named GND. The new

section will have them named GND1. The original section of the schematic

will have the nets named GND. The new section will also have them named

GND. The task here is to rename the net GND1 to GND in the layout.

13. Type "show GND1" in the command line. This will highlight GND1.

14. Use the name tool (R2 Icon) to change the name GND1 to GND. If

prompted, the rename applies to all nets.

15. If you run ERC again, you'll find that all of the GND/GND1 errors are

gone. Redo this renaming process a few more times for the remaining name1

nets and you're done.

Additional note: If you don't have any airwires for the net you're trying to

rename then you'll have to create one using the line tool and the name tool:

Create a line. Rename that line using the R2 tool to the net name you need

to rename (e.g. GND1). This will connect the line to the pad that was

previously un-airwired. Now you can rename the airwire or line to the right

name (e.g. GND) to fix that net.

-

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

FAQ: http://www.cadsoft.de/training/faq/

Former Member · Answer

Dean B wrote:

I cannot seem to get a group to rotate as an

assembly; is this possible? Further, is it possible to group an
assembly so that all actions taken on it (move, rotate, mirror, etc.)
move the whole assembly?

Sure can.

Group the area of interest.

Select 'rotate"

Then, position the cursor at rge point of rotation

Hold down the CTL key and right click the mouse.

The "Hold down the CTL key" assumes you have not changed the setting that

negates the neesd to do so.so that group

"Block Copy" in Eagle PCB Layout

Top Replies