How do I edit thermals on pads in Eagle?

Question

I have a ground plane and would like to increase the number of gaps in the thermals of a ground pad. I have more than 9 amps running through this ground pad and need to increase contact.

It looks like the default number of gaps is 4. I want to increase that to 8. You can apparently change this number easily in other pcb design software but I haven't been able to do it on Eagle. Also, I don't want the component to be modified in the library for every instance of the part, since the pad might not always be connected to a ground plane.

I don't want to remove the thermals all together since that might make soldering more difficult.

Looking at the ground plane, the polygon just makes a cross on the ground pads. Do I have to manually draw a new polygon pattern over each pad or is there a shortcut?

Answer 1

Eagle will only do 4-contact thermals, and only with horizontal/vertical connections.

However, you can increase the width of the connecting traces (thereby shrinking the gaps) by modifying the Width setting of the polygon you are connecting to. This doesn't require making changes to the component library.

For high-current connections I generally make the width equal to the drill diameter. This provides enough copper to match the surface area of plated hole interface, but still provides some cutouts to improve solderability.

Of course, any thermals will limit current flow for the same reason they limit heat flow. It's a design decision on how much copper to relieve, whether using two, four, or eight connections.

If you change the width of the polygon it will effect the rest of that polygon's thermals and borders. If this doesn't work in your design, you can make two overlapping polygons: one around your high-current plated through hole and the other over the rest of your filled area. Give them the same net name and the same priority setting, and let them overlap a bit. Then you can change the width of the polygon in question and leave the other one as-is.