[EAGLE] How to modify all the pads?

[Tom1884]

I have to enlarge all the pads of the components on the PCB. Does a rapid solution exist? Like a script, for example?
If not, how could I change the pad of a component?

In this image there is a large pad (diameter: 1.93 drill: 1) and four smaller. I want to enlarge the small to the large one size.

[madbean]

Open the corresponding library for the components whose pads you want to enlarge. Then, run the ULP "change pad in library" (it's called something like that). I believe it defaults to mm for sizing. Once you run the ULP, it will change all the pads within the range you provide. Save the library, now in Layout, update the library.

[eda123]

Madbean,

This is a great tip.

I already have a layout drawn.. I want to make a backup copy of the lib Im about to change before resizing the pads for its components. Is this as simple as making a copy of the lib directory (and copying it back if I want to restore it)?

[Grendahl]

Yes, you can back up a library by just saving it outside of the library folder it's found in, and to restore it you just move the original file back into the library folder it came from.

[eda123]

Great!

So I backed it up, then ran the "change-pad-in-lib" ULP... and when I look at the components in the library the pads have been resized.

But my current layout using these components shows the old pad size still... ? Any ideas?

[madbean]

You need to update each package. With layout open go to Library-Update. Then select each package in turn and update it. The Update All never seems to work, so you have to do it one by one. You only need to do this with layouts you've already created. From this point on, when you create a schematic from the libraries you changed it will automatically pull in those resized pads. Make sure you run Ratsnest afterward (esp. if you are using a ground plane).

Also, I suggest using the following DRC rather than the native one: http://www.custompcb.com/SilverCircuits.dru

You can have multiple libraries with different names. I have one specifically for stuff to manufacture and one for etching, with the first one having somewhat smaller pads. But I always use the same DRC to check the layout.

[eda123]

OK that updated them- pads are now smaller.. but not as small as the ones in the library themselves.

I cant seem to get the drill "hole" in the middle of the pad to be 0.8mm. I need a 0.8mm hole and 1.02mm pad diameter.

I used the same ULP to resize the hole- specifying both options to resize the drill size and pad diameter.. and the library looks correct after this. I save it, then update again from my layout, however the hole in my layout is still larger.. could some setting in my layout/DRC be overriding this value from the library package info?

[madbean]

Maybe if you're DRC has been set for larger minimum drill sizes. I doubt it though, since .8mm is plenty large.

Email the library to me and I'll take look at it, if you like.

[rapmusic]

Is there a way to change the width of the isolating space around the thermal pads?

[marshmellow]

Yes, you can do that. Open the DRC dialog, go to the supply tab. There you can adjust the
thermal isolate setting to your needs. Afterwards, recalculate the polygon by using ratsnest
and you're finished.

[madbean]

Yes, you can do that. Open the DRC dialog, go to the supply tab. There you can adjust the
thermal isolate setting to your needs. Afterwards, recalculate the polygon by using ratsnest
and you're finished.

F'n A...thanks, I did not know that

[RnFR]

mr. marshmellow definitely knows his eagle. a simpler, although a bit more crude, way of changing pad size, is of course to go into Design Rules and use the Restring function.

[rapmusic]

Thank you, very helpful.