Copy already placed parts

You figure it Out?

"NL2TTL" <cadsoft@ttalens.com> wrote in message

news:forvp2$981$1@cheetah.cadsoft.de...

I have to creat a 7 segment display with onlu 5mm LED's

Is there a way to copy already placed segments in the board, so i don't

have

to place all the parts for every segment by it own.

 

So lets say i have to create A,B,C,D,E,F,G and i have already place

segment

A. How do I copy segment A so i have segments B,C,D,E,F,G and the

schematic

takes over the routing.

 

 

 

NL2TTL schrieb:

I have to creat a 7 segment display with onlu 5mm LED's

Is there a way to copy already placed segments in the board, so i don't have

to place all the parts for every segment by it own.

 

So lets say i have to create A,B,C,D,E,F,G and i have already place segment

A. How do I copy segment A so i have segments B,C,D,E,F,G and the schematic

takes over the routing.

 

 

 

Hello,

somebody recently posted this in the support newsgroup:

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.

HTH

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

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