0
\$\begingroup\$

I'm new to all of this but I'm trying to make a breakout board to a 51 pin micro-d connector. There's a lot of pins like so: enter image description here The breakout board is used too check continuity so no current actually passes through. I don't need to worry about traces being too close.

Below, I tried the auto-route feature on multisim, since there's so many points that it would be too difficult to manually route. As you see, the inside pins all are deemed unreachable. I tried to lower my trace width and clearance all the way down to 5mil and that made no difference.

What is the correct approach to tackle this problem? enter image description here

\$\endgroup\$
  • 2
    \$\begingroup\$ 51 signals is very, very far away from "not manually doable", in fact, I wouldn't even think to try an auto-routed on a semi-dense connector with so few nets. "How to route this" depends at the least 90% on where the signals are going and how many layers you have, or can have. \$\endgroup\$ – Asmyldof Apr 7 '16 at 1:04
  • \$\begingroup\$ What is the hole diameter in those pads? \$\endgroup\$ – The Photon Apr 7 '16 at 1:06
  • 1
    \$\begingroup\$ Use your brain, don't use autoroute! \$\endgroup\$ – Daniel Apr 7 '16 at 1:24
  • 1
    \$\begingroup\$ I have NEVER had to use an autorouter, and every time I tried (just to experiment) it has NEVER worked properly. The autorouter doesn't save you anything, they are generally total garbage. I once had a connector very similar to this on a board I designed at work. The easiest way to handle it if you can't fit traces between the pads is to make a 4+ layer board and put vias around the pads. Then you can bring the signals out to different layers (whichever has the most room). \$\endgroup\$ – DerStrom8 Apr 7 '16 at 12:48
2
\$\begingroup\$

No matter what you end up doing, you will probably end up needing to make 'escape routing' to the outside some way or other (multiple layers with a consistent escape strategy for example) and then route everything from there. If you're really dead-set on using autorouting, get it to that point and then let it have a shot at it. You will probably end up with a lot of vias.

Maybe something like this enter image description here

\$\endgroup\$
  • 2
    \$\begingroup\$ This is the only real way to handle higher density breakouts. BGA is ironically very similar. Most fabs can do 6 mil clearance on traces no problem but budget ones may price their services for a larger clearance so important to verify rules \$\endgroup\$ – crasic Apr 7 '16 at 2:33
1
\$\begingroup\$

Cheap to midrange autorouters are shit. People tell me that the ones from really expensive packages like cadence allegro are better but still can't do as well as a good PCB designer routing by hand. I've never used those packages myself so I can't say for sure.

first you need design rules fine enough that you can get a track between two pads. If you don't have that then you will never succeed. Since you haven't told us the pad size I can't say what those design rules would be but basically you need to take the pin pitch, subtract the pad size and then divide by 3. Some high density connectors will basically require a PCB process that is a step up from some of the cheapest hobbyist services. You also want to be on a grid that is an exact subdivision of half your pad pitch and have your pads aligned to that grid (yes this is a PITA when working with a mixture of metric and imperial components).

Looking at your board I notice the autorouter is putting tracks closer to each other than to the connector pads. You might want to check if your tool has some sort of "pad to track clearance" setting that is larger than the regular clearance setting.

Once you get a suitable set of design rules you can "escape" the connector by following a pattern. You can escape the first row straight out. The second row can use the gaps between the pins in the first row. The third row can use the gaps in the first and second row on the other side of the board. The remaining rows can route out the other side.

Unfortunately even once you have escaped the connector you still have to get the tracks to their destinations. How difficult this is depends on how rigid your circuit design is. If you can swap pins then life is much easier, if you can't swap pins and the pin arrangements on the two sides don't match up well then life gets very painful. Lots of vias, lots of time spent routing and re-routing. Sometimes you may have to make the board bigger or add more layers.

Speaking of vias your vias look as big as your connector pads. That seems weird to me. Once you have figured out your track and gap you might want to look at what PCB manufacturers can meet those specs and what their hole size/annular ring specs for vias are.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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