5
\$\begingroup\$

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?

A ground pad with only 3 gaps in the thermal relief. It needs to be able to take 9A

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

\$\endgroup\$
2
  • 2
    \$\begingroup\$ Eagle AFAIK doesn't have the capability. For high currents I would get rid of thermals altogether. If you don't want to turn them off for the whole polygon, you can put a second polygon over just the pad region and set that one to have no thermals. \$\endgroup\$
    – Tom Carpenter
    Jul 18, 2016 at 23:51
  • \$\begingroup\$ In your top picture, I'd also come off the 12V connection sideways with a narrower trace (same size a pad), and then after a short distance jump up to the full trace width, otherwise you end up reducing the amount of connectable area to the plane on the 0V area. \$\endgroup\$
    – Tom Carpenter
    Jul 18, 2016 at 23:53

1 Answer 1

Reset to default
5
\$\begingroup\$

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.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.