[EAGLE] How to modify all the pads?
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.
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.
Information
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.
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)?
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
- Solder Soldier
Information
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.
Resistance is futile...
( if < 1 ohm )
( if < 1 ohm )
Information
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.
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.
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?
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?
Information
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.
Email the library to me and I'll take look at it, if you like.
- marshmellow
- Cap Cooler
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.
thermal isolate setting to your needs. Afterwards, recalculate the polygon by using ratsnest
and you're finished.
Information
F'n A...thanks, I did not know thatmarshmellow wrote: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.
- RnFR
- Old Solderhand
Information
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.
"You've converted me to Cubic thinking. Where do I sign up for the newsletter? I need to learn more about how I can break free from ONEism Death Math." - Soulsonic
Blog-APOCALYPSE AUDIO
Blog-APOCALYPSE AUDIO