I have trouble connecting a THT HDMI Connector to a pcb:

The HDMI Connector I'm talking about is this.

The holes are too close to go in between them:

enter image description here

(The blue line is 0.15mm thick)

Is this usual (such close and small holes)? Should I be using a pcb manufacturer who can produce thin pcb traces? (like 0.10mm?)

Or just route the trace other way around?

  • \$\begingroup\$ yes but most probably they will charge you more \$\endgroup\$ – Angs Aug 21 '15 at 20:23

Options (in order of my preference):

  1. Route such that you don't have to do that.
  2. Make that pads octagonal.
  3. Make the pads as thin as possible.
  4. Go to thinner traces (if possible).
  5. Utilize additional layers.
  • \$\begingroup\$ Just a drift off but are "wiggly" traces bad for signals like HDMI? \$\endgroup\$ – d3L Aug 21 '15 at 21:23
  • 2
    \$\begingroup\$ Differential signal routing matters, yes. Trace width, spacing, and distance to ground plane are intimately related \$\endgroup\$ – vicatcu Aug 21 '15 at 22:39
  • \$\begingroup\$ Hm, is there any good tutorial on this subject? I really want to know what matters on this high frequency level \$\endgroup\$ – d3L Aug 21 '15 at 22:58
  • \$\begingroup\$ @Houston Fortney "Make the pads as thin as possible" What is the minimum length between drill and pad size? For example: drill=0.45mm pad=0.50mm -> pad is 0.05mm thick \$\endgroup\$ – d3L Aug 22 '15 at 16:02
  • \$\begingroup\$ Both your board house and the part may impose requirements on these dimensions. You may already be at this limit. \$\endgroup\$ – Houston Fortney Aug 22 '15 at 16:14

In terms of width, 6mil traces are quite common nowadays (roughly 0.15mm). Though you may have clearance issues - the gap between pad and trace seems much narrower than the trace.

I have used a similar (not identical) connector in the past. The only difference as far as I can see is that yours is horizontal and the one I used is vertical. This is how I ended up routing it in order to get away from the issue of trace thickness.

The traces in my drawing are quite large as it was a 0.8mm thick 2-layer board and the traces needed to be wide enough to get a roughly 100Ohm impedance.

HDMI Routing

Seems to work fine - don't know about high res as I was using 1280x720. For 1080p the clock frequencies may be higher and other issues may arise.

  • \$\begingroup\$ I see you used curved traces, is this any better than 45 degrees corners? \$\endgroup\$ – d3L Aug 21 '15 at 22:53
  • 1
    \$\begingroup\$ @d3l Less of an impedance change on curved traces as you don't have the angles (the effective trace width at corners is wider so the impedance changes). \$\endgroup\$ – Tom Carpenter Aug 21 '15 at 23:00
  • \$\begingroup\$ Thanks. One more question: how did you get the roughly 100Ohm impedance? Did you manually calculated the trace's lengths and widths? \$\endgroup\$ – d3L Aug 21 '15 at 23:12
  • 1
    \$\begingroup\$ @d3l I used this: eeweb.com/toolbox/edge-coupled-microstrip-impedance \$\endgroup\$ – Tom Carpenter Aug 21 '15 at 23:26
  • \$\begingroup\$ Sweet, thank you \$\endgroup\$ – d3L Aug 21 '15 at 23:29

You may indeed route tracks between the pins of one row to the other row, as I saw it on a graphics card on my desk. The pitch of the pins in one row is 1mm, as it is for your HDMI connector.

enter image description here

However, this need a PCB manufacturer who can produce really small structures. With the pad size from your drawing, a 4mil track has a clearance of 3mil to the pads, which can not be produced by each manufacturer.

May be, you can reduce the pad size (but not drill size) to get more space between the pads, but again, manufacturers have limits on the minimum size of the pad (with respect to the drill size)

Often, the pad size is smaller on the inner layers, so routing may be easier there. (And again: Check what the manufacturer can do)

So, this is really tiny stuff, and it depends on what the manufacturer can do.

Another solution is to change to an SMD connector. A pitch of 0.5mm is quite common today.

  • \$\begingroup\$ I did considered using a SMD version of the connector, but I think this is very fiddly to solder so I chosed a THT version \$\endgroup\$ – d3L Aug 21 '15 at 22:53
  • \$\begingroup\$ Well, you need a really, really fine solder tip, a steady hand and good eyes (and/or a magnifier). I did it by hand. \$\endgroup\$ – sweber Aug 21 '15 at 23:19

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.