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

Hello Richard,

I am currently with a customer who would like to see some key changes with Eagle:  here is what we discussed:

1 - copy/paste function

At the moment, he can only copy one schematic.  The scripts don't enable our customer to achieve what he really wants.

He would like to copy the schematic, the components position on the board and the signal routing.

This customer works a lot with sub assemblies; if he wishes to copy 20 times the same sub assembly, he has to replace all the components every time on the board.

Could the enhanced copy/paste facility he is looking for be included in Eagle? 

2 - shortcuts

He also made a comment about the scripts:  he woud love to have more shortcuts.

For example, when he is trying to find a component, he would prefer to use CTRL F, rather than have to use scripts.

The ideal would be to have shortcuts that you can customise.

3 - facilitating the viewing of different layers

At the moment, our customer has to select a number of Eagle layers (1, 17, 18, 19, 20, 21, 23, 25, 48 et 51) to display the top layers for example.

What would be great would be if you could assign a key, eg F1, to do this in one go.

This would make it easier to switch from layers to layers.

4 - export 3D

Could you please update the 'generate 3D data' script to enable exporting in the IDF4 format?

5 - packages to be available separately

The ideal would be to separate the packages from the library.

This would make it easier for him to create new components, and to switch package from component to component.

6 - sharing libraries between colleagues

Could it be possible to access libraries that colleagues create, without having to copy them manually?

Can you please let me know what you think about the above?

Thank you for your help,

Véronique

Hello Richard,

I am currently with a customer who would like to see some key changes with Eagle:  here is what we discussed:

1 - copy/paste function

At the moment, he can only copy one schematic.  The scripts don't enable our customer to achieve what he really wants.

He would like to copy the schematic, the components position on the board and the signal routing.

This customer works a lot with sub assemblies; if he wishes to copy 20 times the same sub assembly, he has to replace all the components every time on the board.

Could the enhanced copy/paste facility he is looking for be included in Eagle? 

2 - shortcuts

He also made a comment about the scripts:  he woud love to have more shortcuts.

For example, when he is trying to find a component, he would prefer to use CTRL F, rather than have to use scripts.

The ideal would be to have shortcuts that you can customise.

3 - facilitating the viewing of different layers

At the moment, our customer has to select a number of Eagle layers (1, 17, 18, 19, 20, 21, 23, 25, 48 et 51) to display the top layers for example.

What would be great would be if you could assign a key, eg F1, to do this in one go.

This would make it easier to switch from layers to layers.

4 - export 3D

Could you please update the 'generate 3D data' script to enable exporting in the IDF4 format?

5 - packages to be available separately

The ideal would be to separate the packages from the library.

This would make it easier for him to create new components, and to switch package from component to component.

6 - sharing libraries between colleagues

Could it be possible to access libraries that colleagues create, without having to copy them manually?

Can you please let me know what you think about the above?

Thank you for your help,

Véronique

Whenever I've needed to base a design on another design, I simply save it as a different name and then make the necessary modifications - although I would like to see things like this (also, keeping the sizes of the names/values if I change the component - for example, from an 0805 resistor to an 0603).

The second you should be able to assign ULPs to a key - I've got mine so that if I use F11/F12, then it prepares the board for output, so I can paste it onto a web page. This is what I've assigned the key to do:

RUN exp2image color 260 .png 1 17 18 20 21 25 27 48 51;

For the third point, you can do this already - the basic command for what you want is:

display none 1 17 18 19 20 21 23 25 48 51;

This can be assigned to a key from the assign menu.

Thank you for your prompt answer Jason.  I'll definitely pass this information on.

I look forward to hearing from Richard on the other points...

Have a lovely Easter!

Rgds

Véronique

Hello Véronique,

1 - copy/paste function

The current situation is as follows:

One can use  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.

As an alternative there are ULPs that might help. Please take a look at duplicating_vxx.zip or array_board_vxx.zip in the download area of www.cadsoft.de.

2 - shortcuts

As Jason already wrote nearly everything can be assigned with a function key. Please see HELP ASSIGN in EAGLE.

3 - facilitating the viewing of different layers

EAGLE 5 offers so-called aliases for the DISPLAY command. Select the layers you want to have displayed, do a right mouse click onto the DISPLAY icon, select New from the context menu and name the current display setting. So you can choose it each time you need it with two mouse clicks: Right mouse click onto DISPLAY icon, left mouse click to select it from the context menu.

More efficient than using a function key, I think.

4 - export 3D

The generate-3D project was initiated by one of our EAGLE customers. The author of the ULP would be your contact person. I will forward your request to our development people. I can imagine that this might be something to be implemented in a future EAGLE version.

5 - packages to be available separately

The library structure has grown in the last 20 years. So it's nearly impossible to change it easily. But EAGLE has means to keep the package definitions in the different libraries up-to-date. So take for example look into our ref-packages.lbr. It contains all packages that are used in all the other LBRs (except connectors). If you want to make a change in one of the packages, change it there and UPDATE it in all other LBRs that contain this package. There is an ULP that helps here: run-loop-all-lbr-script.ulp.

6 - sharing libraries between colleagues

Sharing libraries in a network, for example, shouldn't be a problem. But the network administrator has to take care on access rights. If the directory where the libraries are, is read-only, everybody can use, but not change them. If somebody wants to change a library he has to do this with a copy of the lbr file. There should be one person in the team that has to take care on such things and make changes available for all then.

Hope this helps.

Richard

As a sort of follow-on from your reply to Véronique, I really do like the right-click to get the list of the most recently used components - however, is there a way to increase the number in the list?

I might have missed it in the documentation...

Hello Richard,

Thank you for taking the time to reply to all the points raised...

I'll get back to you if we've got any more questions.

Regards

Véronique

Hello Richard,

Thank you for your answers to Veronique. I learnt many new things that would help me a lot.

About the "1 - copy/paste function", your solution often leads to unconsistent board/schematic, and most of the time your solution or the ULPs can't be done (because the selected components are not all together, and the signals either). I still haven't find any clean way to do the copy/paste function, and it would be great if it could be implemented in the next version of EAGLE. If you want, I could explain better what I need.

Thank you.

Jerome

Jerome,

I am sure I know what your concern is. Currently the situation can't be changed. Maybe you take look into the mentioned ULPs. If the names of signals and parts would be unique before CUT/PASTE we would not get inconsistencies. This is the way the ULP works, I believe.   But, of course, this could be an improvement for a future version of EAGLE.

Richard

Hello Richard,

About the copy/paste function requested by Veronique (2010-04-06), did the team work on a true solution ? How can I merge 2 projects (each has more than one sheet and both are already routed) ? Thank you.

Jerome

Hi Jerome,

I don't expect an solution for the current EAGLE 5.xx version. This is propably an subject that will be addressed with the next major release of EAGLE.

Regards,

Richard

Hi Richard,

Thank you for your clear answer. About merging 2 or more projects, I have half a solution :

- On each project, I rename the devices with numbers with offset (I modified the ulp renumber-sheet to do this), for example, in the first projet the devices will be MCU1001, R1001, R1002... in the second project the devices will be MCU2001, R2001...

- I copy all the boards into the same board.

- I copy all the sheets into the same schematics.

The problem is now the consistency of the nets, and I didn't find any ulp to rename the nets the same way I do with the devices, and the ulp renamnet-suffix shows a popup for each net... Making an ulp that renames the nets would permit to merge 2 projects in the current EAGLE 5.xx version. Do you have an idea on how to do it ?

In the next version of EAGLE, it would be nice if the sheets of one project could be spread into "folders" or "Tabs".

Thank you,

Jerome