Quick EagleCad question

Is there anyway to change the sizes of individual pads, not every single one

eg

i want to change the size of copper pads circled in red

its too hard to drill the holes with so little leeway

Right click the object in the board view and choose properties
Make note of the pertinent info (the package name)
In the schematic, click the add component button
Search for the package name (put asterisks before and after the name in the search box) and make note of where it is.
Cancel the add component window
Bring up the control panel window and open the Libraries tree
Right click the library that contains the part and choose open
Click the package icon in the menu bar and select that package to edit it.
Right-click the pad (or whatever you want to change) and choose properties.
Set the diameter, drill and shape size
Save and close
Right click the part again in your board view, choose replace
Find the updated package and choose it.
Accept the dialog to update with a new version
Voila!

14 easy steps. :wink:

There may be an easier way to do it. I’d love to hear if there is.

You can use the “restring” of the DRC panel to force a minimum width of the “ring” around pads (it will do all the pads, but that’s usually what you want.) If specify a “minimum” ring size instead of a percentage, it may not enlarge some pads. (however, my experience with components like USB connectors that have large holes is that the have narrow rings as well, and so DO get enlarged.)

You can modify the libraries, as has already been mentioned. Having your own library is generally a good thing…

You can draw polygons for each signal around the pads you want to enlarge. Polygons have the advantage that you specify the minimum clearance to other elements rather than the min/max copper size…

You can probably drop a larger via on top of each pad; this will result in DRC errors about overlapping drill holes, but it may be easiest.

See also the “drill-aid”, which makes the holes smaller (so that they are pilot-hold like, instead of “actual size.”) A slight modification of this ULP should probably be able to draw the polygons around each signal automatically…

See also http://www.instructables.com/id/Make-hobbyist-PCBs-with-professional-CAD-tools-by-/

I found a better way of doing this:

Right click the object in the board or schematic and choose properties
Make note of the the package and library names
Bring up the control panel window and open the Libraries tree
Right click the library that contains the part and choose open
Click the package icon in the menu bar and select that package to edit it.
Right-click the pad (or whatever you want to change) and choose properties.
Change as necessary
Save and close the library editor
Right-click the library in the control panel and choose update.
All parts in your project from that library will be updated with the new design.

Much easier! :slight_smile: