50 mil / 23 ways socket design with Eagle

Discussion in 'General Electronics Chat' started by Hyp, Apr 2, 2010.

  1. Hyp

    Thread Starter New Member

    Apr 2, 2010
    5
    0
    Hello,

    I need to solder a 50 mil / 23 ways (1.27 mm / 23 ways) socket on my PCB.

    I've started to design this new device with Eagle, creating a new library.

    Socket spec:
    - The socket is a 50 mil inch / 23 ways. (1.27 mm / 23 ways)
    - Drill/Hole size is 31 mil inch. (0.79 mm). As per constructor datasheet.

    I’ve an issue with pad size/ restring.

    Clearance between pads should be 8 mil (default Eagle setup).

    Socket Pin Spacing : 50 mil
    Clearance : 8 mil
    Drill Diameter : 31
    Free space for the Restring : (50-8-31)/2 = 5.5 mil.

    5.5 mil is out of most of PCB rules and limits.

    Any clue on how can I design the footprint for this socket ?

    Regards,
    Hyp.
     
  2. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    It's going to be tight.

    Did you try reducing the restring % in the DRC restring tab? The default is 25%; try reducing it to 10%

    That's going to change all of your other pads too, of course. I don't know of another way to do it offhand.
     
  3. kkazem

    Active Member

    Jul 23, 2009
    160
    26
    Hi,

    Since this is a surface-mount technology device (SMD or SMT), the geometries shrink much smaller than for thru-hole PWB layout and you have to adjust settings on your layout tools for these small-geometry parts. Unless you need the large 30 mil DIA pads for heat-sinking, I would shrink the pad DIA to samething much smaller as even for SMT, 5-mil is about the limit for line widths and spacings for PWB fabricators. Go and look at the websites of several PWB manufacturers as they often have good design guidelines to help PWB designers transition to SMT/SMD with specifics about pads, hole sizes, ground planes, copper thicknesses (i.e. 1-oz, 2-oz), and other important info you'll need to avoid getting a PWB that's unusable and therefore wasted money. ALso, you can generally call them and talk to thier engineers if you still have specific questions unanswered. But you'll have to find the websites of the larger PWB mfgs, like Advanced Circuits in Colorado, they also have prototype specials for as low as $ 100 for 1 or 2 prototype boards.
    Good luck,
    Kamran Kazem
     
  4. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Try this:

    Go back into the library you created the part in.

    Edit the package for the part.

    Change the drill size of the pads to 0.031 if they are not already.
    Change the diameter of all the pads to 0.042
    Since you are spacing on 50 mil centers, that should give you exactly 8 mils between the pads, as 50mils - 42mils = 8mils

    I am not certain how the DRC restring will perform when you have the pad diameter set to an absolute rather than automatic. It's going to take a bit of experimenting on your part.

    Just looked in the Help file....If the diameter is set to 0, the size of the pad is derived from the drill diameter (auto pad size). So, it looks to me like setting the pad drill size to .031 and the pad diameter to .042 will get you just where you want to be.
    If you want just a bit over 8 mils clearance, then try setting the pad diameter to 0.0415, which should result in 9 mils clearance.
     
    Last edited: Apr 2, 2010
  5. Hyp

    Thread Starter New Member

    Apr 2, 2010
    5
    0
    Hi,
    Thanks to both of you for your help.

    Karam, this is not SMD/SMT, this is Through Hole/Traversant (Samtec SLM serie, http://www.samtec.com/ProductInformation/TechnicalSpecifications/Prints.aspx?series=SLM)

    SgtWookie, I did "hard" fixed the drill dia (31 mil) and the pad dia (42 mil), e.g no more auto sizing of the pad from the drill size.
    This is OK within the Package design window. (See picture 1). However, when I add this new created package into my PCB window, pads are bigger, and overlapping each other.
    Seems that the hard fixed value are not taken in account, seems "auto" is still active.
    I'll continue to investigate.
    Regards,
    Hyp.
     
  6. Hyp

    Thread Starter New Member

    Apr 2, 2010
    5
    0
    I setup 1 miil for min restring.

    Pads are not anymore overlapping, but I still have an issue vith clearance.

    I tried with drill dia at 31 mil and pad dia at 41 mil (instead of 42 mil).
    Pads are thinner comparing from previous PCB, but still thicker comparing to the designed package.

    Regards,
    Hyp.
     
  7. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    What version of Eagle are you using?

    I am on 4.16r2, and don't care to pay to upgrade.

    This does seem to me to be a bug. I would not expect for the pad diameter to be changed by restring if I had specified a size other than zero.

    However, as a work-around, try changing your pad diameter to 40 mils or less - just get down to the 8+ mil clearance that you must have to get your board made.
     
  8. Hyp

    Thread Starter New Member

    Apr 2, 2010
    5
    0
    Hello,

    I'm on 5.7.0.

    I've installed 4.16r2.
    I've built a simple package : 4 pads, drill dia 31, pad dia 42, pitch at 50 mil.

    See first attached picture. Pad seems OK, e.g not overlapping.

    Then I went to the PCB window, inluding this new created pad. Then, pads are now overlapping. (See 2nd picture).

    Finally I went to the DRC / restring, moving from min=10mil to min =1 mil.
    Pad size is changing (see 3rd picture), not anymore overlapping, but there is still an issue with clearance.

    I think I'm doing something wrong here. Don't really know what it is.

    Regards,
    Hyp.
     
    • 1.JPG
      1.JPG
      File size:
      30.8 KB
      Views:
      13
    • 2.JPG
      2.JPG
      File size:
      18.6 KB
      Views:
      11
    • 3.JPG
      3.JPG
      File size:
      19.3 KB
      Views:
      10
  9. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    No, you're not doing anything wrong.

    Found this in the Eagle FAQ:
    http://www.cadsoftusa.com/faq.htm#06012601

    11. How to Define the Pad Diameter?


    Since EAGLE version 4.0 the default libraries contain only information about the drill diameter and the shape of a pad. The diameter value is set to auto, which is the same as 0, by default.
    What does this mean?
    The actual diameter will be calculated in the Layout Editor only. The calculation rule can be found in the Design Rules (menu Edit/Design Rules...) in the Restring tab. There you are allowed to define different calculation rules for Top, Bottom, and inner layers.
    How is it Calculated?
    The percentage, which is related to the drill diameter is used to calculate the width of the copper ring that is around the drilling. Default is 25%. A drill diameter of, for example, 0.032 inches results in a ring width of 0.008 inches.
    In the next step EAGLE checks if this value is within the given minimum and maximum boundaries. If so, the diameter of the pad results for our example in (2 * 0.008) + 0.032 = 0.048 inches.
    Let's assume the minimum value is set to 0.010 inches. In this case the previously calculated value of 0.008 inches will be increased in order to accomplish this criteria to 0.010 inches. The resulting pad diameter will be 0.052 inches now.
    If the calculated value for the restring exceeds the value of the maximum limit it will be decreased to the maximum tolerated value.
    The minimum value represents in principle the Board house's given production limits. This is the reason why it is forbidden to exceed the lower limits.
    What Happens if I Define a Diameter in the Package Editor?
    If you choose a value for the pad diameter in the Package Editor, EAGLE calculates again the width of the copper ring by the given percentage as soon as you add the part to the layout. The calculated value will be compared to the pre-defined one, resulting from the given diameter in the library. If the pre-defined value is smaller than the calculated value or the minimum limit is exceeded, the pad diameter will be increased.
    In the case of exceeding the maximum limit, EAGLE will tolerate this. The pad's diameter won't be reduced automatically!

    Changing the Design Rules affects the board immediately! Modify the settings for Restring and click the Apply button and you will see the result in the layout directly!
    Restring settings are valid for all the pads in the layout!
    It may happen that the pad diameter shown in the Package Editor or in the preview of the Device Editor or the Control Panel is not displayed exactly the same as it is in the Layout Editor because the Design Rules can be applied in the Layout Editor only!
     
  10. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    So, there you have it.

    I don't think it was a good idea for them to ALWAYS restring pad sizes.

    But anyway, with your drill size set to .031", try changing your restring percent from 25 to 17 for top, inner and bottom pads.
    Reasoning: .031 * 17% = 0.00527 ring width; x2= 0.01054; +.031= 0.04154" diameter.

    Then change Min for top, inner and bottom pads from the default of 10mil to 5mil.

    Then click Apply; you should then have just over 8 mils between pads.
     
  11. Hyp

    Thread Starter New Member

    Apr 2, 2010
    5
    0
    Hello,

    I've put auto / 31 mil for the package, 17% and min=5 mm for the restring.

    This is working, as now DRC is not reporting errors anymore.

    Thank for the help.

    I'll send my layout to fab. Hope it will be not too tricky for soldering these pads :)

    Regards,
    Hyp.
     
    • 1.JPG
      1.JPG
      File size:
      24.5 KB
      Views:
      12
  12. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Glad it worked for you.

    It was obviously a learning experience for me as well.
     
Loading...