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

Hi

since version 5 you can drag&drop a package or a whole device from one library into another. Open Control Panel and Library editor window simultaneously, expand the libraries branch in the CP and drag the package (click onto the package entry in the list) into the library editor window.

regards,

Richard

Probably, after you cut/copy the part(s) you open a new eagle page. That's after you cut/copy you must go to the file menu and find the file that you want to paste the copied components. This is the same for schematic and board sides.

Strangely, you need to use CUT not COPY. To copy from schematic to schematic you need to select your group of components, right click and CUT group and then that's what will be in the paste buffer. Then you can paste it into the same, or another schematic. Not sure about the layouts though, I've always had the fear of back-annotation/erc discrepancies.

Thx for the info on copying from library to library.... Now how about copying from schematic to schematic.   I want to use a big section from one schematic and put it into another.  I don't want to re-enter by hand.  Every time I cut and paste, the message says there is nothing to paste.  Going one more level, is it possible to paste one layout into another (I don't think so)

Thx in advance

How I transfer package from one library to another (EAGLE-4.16):

1.    Open existing package in old library;

2.    "Display all";

3.    "Group" whole package;

4.    "Cut" (place cursor on origin, click);

5.    Open new library;

6.    Open new package (could has the same name as old one, of course);

7.    "Paste" (pay attention to place picture into desirable origin).

          Boring... but works.

               Good luck!

                     Lev.

Moving packages from one device to another.

I have created a new device but want to move the SOT-5 package from another library so that I do not need to redraw it.

How can I do this?

Thanks!

Nora

Good morning Damian,

I am sorry but EAGLE does not support an Online-DRC. But what can be helpful is the Follow-me router. But this requires the Autorouter module.

The Followme router is a special mode of the manaul ROUTE command. As soon as you click onto an airwire EAGLE draws the connection automatically. The position of the mouse cursor decides about the way the trace has to take. In this mode you don't have to take care on Design Rules because the Follow-me router does automatically.

Regards,

Richard

Excellent.  Thank you, Richard.  I had also found (very short) post on this at SparkFun: http://forum.sparkfun.com/viewtopic.php?f=20&t=8370 .  It is good to have the FAQ for reference for everyone now.

Hi,

the restring parameter is always taken into consideration. As soon as the value for "minimum restring" is bigger than the resulting value from the library definition, the value will be adjusted. So the pad is bigger than in the library. Please change the resting settings to make it work as you expect.
For a better understandig how this all works I add a FAQ here:

How to Define the Pad Diameter?

Since EAGLE version  4.0 the default libraries contain only information about the drill  diameter and the shape of a pad. The diameter value is set to auto, which is the same as 0, by default.

What does this mean?
The actual diameter will be calculated in the Layout Editor only. The  calculation rule can be found in the Design Rules (menu Edit/Design  Rules…) in the Restring tab. There you are allowed to define different calculation rules for Top, Bottom, and inner layers.

How is it Calculated?
The percentage, which is related to the drill diameter is used to  calculate the width of the copper ring that is around the drilling.  Default is 25%. A drill diameter of, for example, 0.032 inches results  in a ring width of 0.008 inches.
In the next step EAGLE checks if  this value is within the given minimum and maximum boundaries. If so,  the diameter of the pad results for our example in (2 * 0.008) + 0.032 =  0.048 inches.
Let’s assume the minimum value is set to 0.010  inches. In this case the previously calculated value of 0.008 inches  will be increased in order to accomplish this criteria to 0.010 inches.  The resulting pad diameter will be 0.052 inches now.
If the  calculated value for the restring exceeds the value of the maximum limit  it will be decreased to the maximum tolerated value.
The minimum  value represents in principle the Board house’s given production limits.  This is the reason why it is forbidden to exceed the lower limits.

What Happens if I Define a Diameter in the Package Editor?
If you choose a value for the pad diameter in the Package Editor, EAGLE  calculates again the width of the copper ring by the given percentage  as soon as you add the part to the layout. The calculated value will be  compared to the pre-defined one, resulting from the given diameter in  the library. If the pre-defined value is smaller than the calculated  value or the minimum limit is exceeded, the pad diameter will be  increased.
In the case of exceeding the maximum limit, EAGLE will tolerate this. The pad’s diameter won’t be reduced automatically!

Changing the Design Rules affects the board immediately! Modify the settings for Restring and click the Apply button and you will see the result in the layout directly!
Restring settings are valid for all the pads in the layout!
It may happen that the pad diameter shown in the Package Editor or in  the preview of the Device Editor or the Control Panel is not displayed  exactly the same as it is in the Layout Editor because the Design Rules  can be applied in the Layout Editor only!

Regards,

Richard