Have a question about CadSoft EAGLE?  Ask our Expert, Richard! (Archive)

Hi Paul,

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.

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.

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

There is also an explicit description in on of the CadSoft forums written by one of our useres...... I would like to add it here, as well:

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.
--------------------------------------------------

Regards,

Richard

Frequently I have the need to replicate a subcircit in a schematic/board, perhaps with 10~30 parts;  now while this works fine on the schematic to select-cut/copy, it does however only dump the parts onto the layout/board and then they all need to be suitably placed/routed - my question is - "Is there a way to cut-copy from the schematic and have Eagle also replicate the board/routing of the existing copy? (obviously offset to some other part of the layout screen)"

Hi Kevin,

1-

You could use a SMD pad.  While creating your package instead of using the PAD command to define your contacts use the SMD command.  With the Change command you can resize the pad to accomodate the compoent in question.  You can also use the ROUNDNESS factor if you need the corners of the SMD pad rounded.

2-

This all depends of the grid you are using.  At this time there is no tool in EAGLE that will alert you that your in the center of two leads.  DRC will report if you are violating any clearance criteria.

Best Regards,

Ed

Hi, Richard,

1. I am going to make a single layer board. Can I make a pad only in one layer and no plate through hole?

2. How can route the traces exactly in the center between two pads?

Thanks,

Kevin

Hi Ralph,

It is possible to place components on either side of the board.  Use the MIRROR command to move components from Top to Bottom and vice-versa.  The Silkscreen information will transfer to the respective layer as well.

Best Regards,

Ed

Hi Richard,

I am a new user and would like to know how or if I can place SMDs on both sides of a twolayer PCB?

Thanks, Ralph

Richard_H wrote:

 

Hi,

 

it is not possible to show the clearance around a wire while manual routing. You have to run the DRC for checking the clearance values.

If you are using the follow-me router for manual routing you don't have to pay attention to clearances. The follow-me router always maintains all the values set in the design rules.

 

Concerning pads:

Pads are part of the package which is defined in a library. It is not possible to move individual pads in the layout editor. You have to do this in the library.

 

Regards,
Richard

Thanks for you reply

It seems a bit silly, if you are doing something that requires very tight clearances to have to run 'blind' and check with DRC every 5 seconds. I tried the follow-me router but it kept putting vias where I did not want them. I do not know if there is a way to stop that.

The way KiCad does it is better (by showing you the clearance as you go) unfortunately the design I am working on was made in Eagle and I cannot easily port it to KiCad without losing critical placement locations of certain components.

As for having to edit pads in the libary, again this is more inconvenient and difficuilt than the fact you can move pads in KiCad 'on-the-fly'.

Of course this is not meant to be a put-down of Eagle at all, as it cetainly does do some very good things that KiCad doesn't (a far, far more extensive library, for example) and I know that a lot of people seem to use it quite happily - but for those two main reasons (and others) it just isn't my choice of EDA software.

Hi Richard,

Richard_H a écrit:

 

Hi Jerome,

 

increasing the SMDImpact parameter should cause the Autorouter to draw the a longer trace  in preferred direction before there is a bend or a via. Did you set preferred directions? Did you increase the parameter for the Optimize passes as well?

 

Regards,

Richard

If the SMDImpact parameter depends on the preferred direction, this is a big mistake. I use many quad packages (QFN, LQFP...), so if I set a preferred direction (unless I set diagonal / or \), the Autorouter will manage to route only 2 sides, and it will not manage to route the others if it decides to put vias, because the vias will be close to the pins. So I have to put many vRestrict. I must choose the preferred directions according to the placement of the components, the shape of the board, and the way of the signals...

Any improvements to the Autorouter would be really appreciated. I think this is the worst part of EAGLE.

Thank you.

Hi,

it is not possible to show the clearance around a wire while manual routing. You have to run the DRC for checking the clearance values.

If you are using the follow-me router for manual routing you don't have to pay attention to clearances. The follow-me router always maintains all the values set in the design rules.

Concerning pads:

Pads are part of the package which is defined in a library. It is not possible to move individual pads in the layout editor. You have to do this in the library.

Regards,
Richard

Hi Ralph,

the way you described to get the problem fixed is correct. Be sure to run ERC that checks consistency between board and schematic afterwards.

Regards,

Richard