2
\$\begingroup\$

I have been working on a simple 2-layer PCB primarily intended for routing various power connections (essentially acting as a power distribution junction) to clean up the cabling in my enclosure.

I wasn't able to find an official Eagle library for Molex's 5569 Mini-Fit Headers, so I downloaded Robert Starr's version: con-molex-mini-fit.lbr

Great! So I checked the part I wanted (PN: 39-30-1040), verified that the pin pitch and outer dimensions matched and added it to my design. One small issue I noticed before I was about to generate Gerbers... apparently the drill diameter for the pads is wrong?!

From the layout, the drill diameter of the pad is 1.42mm.

Molex 39-30-1040 Drill Dimensions

Going to the part's CAD drawing, the pin is 1.07mm x 1.07mm (length x width) and the hole layout says 1.80 ± 0.05mm DIA. So is this 'DIA' referring to the actual drill diameter, or the pad diameter? Either way, the pin diagonal is ~1.513mm so would I have been totally screwed had I sent the original for fabrication? What should I do from here to fix this problem?

Molex 39-30-1040 CAD Drawing

Yes, I know it's always better to make your own parts for this exact reason... but please bear with me. This is my first board where I haven't had the wonderful support of CAD engineers to make all the footprints and symbols and check this stuff for me :( I'm trying to be a good engineer, though, and make sure I've done the due diligence to the best of my ability.

Also, to piggyback off a related question, is there an official Molex 5569 library?? I would have commented to ask in that question directly but I'm a sad panda who doesn't have enough reputation to comment yet. D:

Thanks for your help!

\$\endgroup\$
3
  • 1
    \$\begingroup\$ Is this a question or a complaint? \$\endgroup\$
    – Eugene Sh.
    Jul 21, 2015 at 21:02
  • \$\begingroup\$ Sorry if it came across as that. I guess I was a little verbose. I basically want to know if I should go with the 0.180mm number as the drill size (highlighted in the datasheet). Perhaps to add on to this, are through-hole pads plated by default in Eagle? I imagine that once I stuff the connector and solder it, both the top and bottom layer will be connected electrically, but what about before? \$\endgroup\$
    – KnightsValour
    Jul 21, 2015 at 23:34
  • 1
    \$\begingroup\$ The default is through-plated. If you want non-plated, Eagle calls them "holes" instead of "drills". \$\endgroup\$
    – bitsmack
    Jul 22, 2015 at 0:22

3 Answers 3

Reset to default
2
\$\begingroup\$

The quick answer is that you should use the manufacturer's recommendation of 1.8mm hole size, unless you have a pressing reason not to.

This is the finished hole size. Eagle refers to this as the "drill size", which can be misleading. To get a 1.8mm finished hole the PCB manufacturer will actually use a slightly larger drill. The plating process adds material to the inside of the hole, and brings it down to the diameter you specified.

The manufacturers generally don't recommend a specific pad size (the size of the annular ring) because this can vary depending on how tightly spaced the design is. A large ring takes more space, but is easier to solder to. In Eagle, I would leave the pad diameter as "Auto". This way it will adjust automatically if you change your design rules.

Sometimes the datasheets only give you the part dimensions and don't include a recommended hole layout. In this case, determining hole size is a bit art and a bit science. Here's how to go about it:

  • You already know that the diagonal of the pin is 1.513mm. It doesn't give a tolerance, so take it as it is.
  • Your board house will have drill tolerance specs that they publish. It is common to be +/- 5 mil (0.127mm) unless you request something better.
  • Find the smalles hole size that will be larger than the pin. Take into consideration the worse-case tolerances for the hole and the part.
  • Add a little bit :) That's the art!

In this case, the hole is 1.513mm (pin diagonal) + 0.127mm (pcb hole tolerance), giving 1.64 mm. Add an unknown pin tolerance, and a little wiggle room, and it comes out pretty close to the suggested 1.8mm.

Good luck!

\$\endgroup\$
5
  • \$\begingroup\$ Thank you for a very detailed answer - I appreciate you having patience with me! Are there any particular references/guides you would recommend I read when it comes to PCB design and fabrication? Or is experience the only true teacher? \$\endgroup\$
    – KnightsValour
    Jul 22, 2015 at 0:50
  • 1
    \$\begingroup\$ @KnightsValour Experience is key. Of course, "experience" just means figuring out how to do things that you didn't know before. This happens by reading books, reading the EagleCAD documentation, fixing mistakes that you've made, and scouring the EE Stack :) I've learned a lot by reading through the "capabilities" pages on PCB manufacturer's websites! It gives a good idea of what's possible. Btw, I once had a run of 100 boards made that had holes too small for the component leads. Our budget was so tight that we actually shaved the corners off of the square leads! Not a fun experience :) \$\endgroup\$
    – bitsmack
    Jul 22, 2015 at 6:28
  • 1
    \$\begingroup\$ @KnightsValour The book Complete PCB Design Using OrCAD... by Kraig Mitzner has four excellent chapters about how PCBs are designed, manufactured, and assembled. It's really approachable, with nice illustrations. The other six chapters are all OrCAD-specific, though, so it might not be worth the money since you're using Eagle. Maybe one of your coworkers will loan it to you :) \$\endgroup\$
    – bitsmack
    Jul 22, 2015 at 6:28
  • 1
    \$\begingroup\$ @KnightsValour Oh, I forgot an important resource: anyone with more experience! You'll learn more spending an hour watching an Eagle wizard lay out a board than you can imagine :) \$\endgroup\$
    – bitsmack
    Jul 22, 2015 at 6:32
  • \$\begingroup\$ Thanks for all the useful advice @bitsmack! I'll check out that book when I get the chance. \$\endgroup\$
    – KnightsValour
    Jul 22, 2015 at 12:22
2
\$\begingroup\$

One can never rely on anyone else's libraries unfortunately. Even the default libs may be 95% accurate. If you get something close, then great, saves you a little work. But it's par for the course to go through each component, each pad, and make sure they match up with the datasheets. Even DIP and SO components... I've seen soldering a SO16 be a nightmare, because the default library width was one thing, and the chip width was slightly wider.

Just get into the habit of making your own libraries. After using and testing them, you'll be 100% assured anything in it will be spot-on.

\$\endgroup\$
2
  • \$\begingroup\$ This will definitely be my plan moving forward. To be honest, I thought about doing this to begin with - but this board needs to be fabricated ASAP and so I looked for existing libraries. So to resolve my problem - should I increase the drill size to 0.180mm? Are there standards that PCB designers follow with respect to how much larger the drill should be compared to the largest pin dimension? Thanks for your help! \$\endgroup\$
    – KnightsValour
    Jul 21, 2015 at 23:30
  • 1
    \$\begingroup\$ Generally I'd seen desired through-hole diameters to be the (maximum) pin size (in the case of square or rectangular leads, the cross-corner maximum) plus 6mil or 0.153mm clearance for copper plating. So if the lead were 1.64mm cross-corners, the recommended hole of 1.80mm would work (albeit snugly), because 1.80 - 0.153 = 1.653, leaving 0.013mm clearance. Most PCB manufacturers I've seen plate through-holes with a thickness of around 5mil, but certainly not all are equal. It's a good idea to check with them and determine the characteristics. \$\endgroup\$
    – rdtsc
    Jul 22, 2015 at 0:46
-1
\$\begingroup\$

OK, so you found a bug. Go fix it.

Now maybe you've learned to make your own libraries. Vetting someone else's is usually more work than just making it the way you want in the first place. And then you can make it work with your conventions for text size, what you put in the Docu layers, nice schematic symbols and silkscreen outlines, usage of optional attributes for your BOM making utilities, etc.

You can try my Eagle libraries. They are in the Eagle Tools release at http://www.embedinc.com/pic/dload.htm. These are the parts I actually use, but that doesn't mean they are all perfect. If you look hard enough, you can probably find a mistake or two.

\$\endgroup\$
3
  • 1
    \$\begingroup\$ I don't think I'll be visiting that link somehow. Not after what Norton has to say about it :) \$\endgroup\$
    – Tom Carpenter
    Jul 21, 2015 at 22:24
  • \$\begingroup\$ I appreciate you taking the time to post a response, Olin. I'm sorry if it came across as me complaining - as I mentioned, I am relatively new at this stuff and so I thought I would make a post to get some feedback. Everyone's inexperienced at one point or another, and I'm doing my best to learn and hopefully help others that post here in the future. To clarify my main question, does the 1.80 +/- 0.05mm highlighted in the datasheet refer to the drill diameter or the recommended pad size? \$\endgroup\$
    – KnightsValour
    Jul 21, 2015 at 23:26
  • \$\begingroup\$ @Tom: It is a false positive. A few years ago something changed in one of our low level libraries, and several anti-virus programs thought all our EXEs were infected. I rebuilt them all from source code, but still the same. It seems they do rather dumb pattern matching without further checking. Recently the pattern apparently changed again and most newly-built program are no long false positives, but some of the older ones still are. Eventually all will be flushed. We're moving to a new compiler soon which should change patterns completely. \$\endgroup\$
    – Olin Lathrop
    Jul 22, 2015 at 10:42

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.