7
\$\begingroup\$

In double sided PCBs it is difficult to solder through hole components like IC bases, headers, etc. in the top layer. Normally the Eagle autorouter places the solder pads on both sides. That is, in a through-hole IC base some pins should be soldered in the bottom layer and some in the top layer. But I need routes in the top layer and vias.

Is there a way in the Eagle autorouter to tell it to avoid soldering in top layer? Please see the "Design requirements for hobby boards" and "Turned-pin IC sockets" sections of Joe's Hobby Electronics: Making double-sided PCBs for more information about the problem.

\$\endgroup\$
1
  • 4
    \$\begingroup\$ As a piece of practical advice, you are better off doing the routing manually than with the autorouter, especially when you add the constraints of a handmade board and consider what an (unprintable) pain vias are in such circumstances. \$\endgroup\$
    – Chris Stratton
    Commented May 5, 2013 at 15:53

3 Answers 3

Reset to default
3
\$\begingroup\$

While I have to agree with the previous answers - you are indeed a lot better off in the long run if you route manually, I feel your question has not really been properly answered.

A quick-and-dirty workaround for you might be

  • copy the component(s) to a library of your own
  • add a new package, in which you put a GND rectangle around the entire component on the top layer only
  • in the circuit, replace the original component with your tampered component
  • let the autorouting commence
  • go back to your circuit, and swap the component back to its original package.

Now, before the rotten-egg-throwing sets in, a few extra words why you should not do that.

While Eagle takes quite a bit of effort to get the hang of, it is definitely worth practicing these things on simple designs. As you advance, you will get to the point where you have to route manually, because some signals must be laid out in certain ways. There might still be workarounds for each specific problem, but you will never have practiced to place the components in a way that it is possible to route with minimal effort and losses.

\$\endgroup\$
1
  • \$\begingroup\$ +1 This does answer the question. I've got to try that!! \$\endgroup\$
    – Ricardo
    Commented Jan 14, 2015 at 19:18
2
\$\begingroup\$

If you want to discourage the autorouter from using a layer, you can tell Eagle to increase the routing cost of a layer in the autoroute dialogue. That way possible routing solutions that use the top layer are rated lower than those with shorter track lengths or other optimized solutions. Higher costs mean less likely use of the top layers. You may need to change this on all route and optimize stages for it to be effective.

To prevent Eagle from using the top layer, you should make the PCB a one-sided board by turning off the top layer. This will make the design much more difficult to route, and will require good part placement.

I would still recommend routing the board manually - that way you know the trade-offs yourself instead of depending on an algorithm to find an answer.

\$\endgroup\$
0
\$\begingroup\$

An easy solution/hack is to draw a circle/rectangle with around the pins with the layer you want the auto router to STOP using. So in your case you will draw a circle using the top layer on every pin of the IC which will force the auto router to start routing using bottom layer.

enter image description here

\$\endgroup\$
1
  • 1
    \$\begingroup\$ The downside is you then get errors from overlapping copper. A better approach would be to draw a box (4 lines) around each pin on the tRestrict layer. That will indicate to the autorouter not to put any copper going through the tRestrict lines, and won't cause DRC errors as long as your lines don't overlap the pins. \$\endgroup\$
    – Tom Carpenter
    Commented Jun 19, 2017 at 19:43

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