element14 Community
element14 Community
    Register Log In
  • Site
  • Search
  • Log In Register
  • Community Hub
    Community Hub
    • What's New on element14
    • Feedback and Support
    • Benefits of Membership
    • Personal Blogs
    • Members Area
    • Achievement Levels
  • Learn
    Learn
    • Ask an Expert
    • eBooks
    • element14 presents
    • Learning Center
    • Tech Spotlight
    • STEM Academy
    • Webinars, Training and Events
    • Learning Groups
  • Technologies
    Technologies
    • 3D Printing
    • FPGA
    • Industrial Automation
    • Internet of Things
    • Power & Energy
    • Sensors
    • Technology Groups
  • Challenges & Projects
    Challenges & Projects
    • Design Challenges
    • element14 presents Projects
    • Project14
    • Arduino Projects
    • Raspberry Pi Projects
    • Project Groups
  • Products
    Products
    • Arduino
    • Avnet Boards Community
    • Dev Tools
    • Manufacturers
    • Multicomp Pro
    • Product Groups
    • Raspberry Pi
    • RoadTests & Reviews
  • Store
    Store
    • Visit Your Store
    • Choose another store...
      • Europe
      •  Austria (German)
      •  Belgium (Dutch, French)
      •  Bulgaria (Bulgarian)
      •  Czech Republic (Czech)
      •  Denmark (Danish)
      •  Estonia (Estonian)
      •  Finland (Finnish)
      •  France (French)
      •  Germany (German)
      •  Hungary (Hungarian)
      •  Ireland
      •  Israel
      •  Italy (Italian)
      •  Latvia (Latvian)
      •  
      •  Lithuania (Lithuanian)
      •  Netherlands (Dutch)
      •  Norway (Norwegian)
      •  Poland (Polish)
      •  Portugal (Portuguese)
      •  Romania (Romanian)
      •  Russia (Russian)
      •  Slovakia (Slovak)
      •  Slovenia (Slovenian)
      •  Spain (Spanish)
      •  Sweden (Swedish)
      •  Switzerland(German, French)
      •  Turkey (Turkish)
      •  United Kingdom
      • Asia Pacific
      •  Australia
      •  China
      •  Hong Kong
      •  India
      •  Korea (Korean)
      •  Malaysia
      •  New Zealand
      •  Philippines
      •  Singapore
      •  Taiwan
      •  Thailand (Thai)
      • Americas
      •  Brazil (Portuguese)
      •  Canada
      •  Mexico (Spanish)
      •  United States
      Can't find the country/region you're looking for? Visit our export site or find a local distributor.
  • Translate
  • Profile
  • Settings
Autodesk EAGLE
  • Products
  • More
Autodesk EAGLE
EAGLE User Support (English) Plated hole in SMD pad
  • Blog
  • Forum
  • Documents
  • Events
  • Polls
  • Files
  • Members
  • Mentions
  • Sub-Groups
  • Tags
  • More
  • Cancel
  • New
Join Autodesk EAGLE to participate - click to join for free!
Actions
  • Share
  • More
  • Cancel
Forum Thread Details
  • State Suggested Answer
  • Replies 4 replies
  • Answers 2 answers
  • Subscribers 170 subscribers
  • Views 1100 views
  • Users 0 members are here
  • pad
  • library
  • question
Related

Plated hole in SMD pad

Former Member
Former Member over 12 years ago

Hi

 

I've been using eagle for over 10 years. Currently using Eagle 5.12.

 

I am using some smt bottom feed through recepticles from mill max PDFs below.

 

actual part -http://www.mill-max.com/pdf/datasheet/pin_rec_catalog/8874-0-15-01-11-27-10-0.pdf

footprint- http://www.mill-max.com/pdf/datasheet/sockets/388-44-102-11-740799.pdf

 

How do I make a pad with a plated through hole in it's center, without causing an error?

 

Thanks,

Kim S.

  • Sign in to reply
  • Cancel
  • Former Member
    0 Former Member over 12 years ago

    RadioCtrlDWife wrote:

    Hi

     

    I've been using eagle for over 10 years. Currently using Eagle 5.12.

     

    I am using some smt bottom feed through recepticles from mill max

    PDFs below.

     

    actual part

    -http://www.mill-max.com/pdf/datasheet/pin_rec_catalog/8874-0-15-01-11-27-

    10-0.pdf

    footprint-

    http://www.mill-max.com/pdf/datasheet/sockets/388-44-102-11-740799.pdf

     

    How do I make a pad with a plated through hole in it's center,

    without causing an error?

     

    Thanks,

    Kim S.

     

    It's not possible to make that footprint in Eagle without errors

    Eagle Version 6  cannot make it either.

     

     

    Plated holes can only exist if you use a pad the DRILL  of which is  plated

    through.

    A HOLE which is not plated through does not meet your requirements.

    So it seems you need to use a PAD. Alas the DRC will adjust the pad so the

    restring has width and that will spoil your footprint.

     

    So it's back to the hole again.

    You could instruct the board house merge the HOLES and DRILLS files so the

    HOLES are plated through. You could manually do this yourself.

    A ULP would be useful for that. Maybe there is one.

     

    So the package becomes two SMD pads with holes. Alas there will be DRC

    errors that you will need to approve.

     

    I have suggested previously that Eagle needs a  HOLE parameter named 'PTH'.

    If it is 'true' the HOLE is treated as a DRILL, is plated through and the

    signals (pours) don't keep clear of it so the PTH connects to copper. In a

    package this hole/drill would need to be considered part of the SMD /Contact

    and not generate a DRC error.

     

    HTH

    Warren

     

     

     

    --

    Viewed / responded via the newsgroup at

    news.cadsoft.de

     

     

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Reject Answer
    • Cancel
  • Former Member
    0 Former Member over 12 years ago in reply to Former Member

    Thanks Warren.

     

    Yes, The package looks fine in the libray (I put the pads on a metric grid and the holes on a english grid to avoid the overlap error) until I add it to the board, then the DRC changes the diameter of the holes of the pad within the smd pad, causing the edges of the pads to touch eacother. Of course if I change the DRC setting the rest of the board is affected causing other DRC errors.

     

    The pcb printing house I use typically plates holes, I just want to make sure the holes are connected to the pads correctly. Perhaps I should contact them and confirm this...

     

    Here's a screen shot of what happens when I add the part to a board. Note the board has other violations which are the least of my concerns at the moment. First image is in the library device editor, second image is in board.

    image

     

    Kim S.

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • Former Member
    0 Former Member over 12 years ago in reply to Former Member

    Good to see your usage on a board.

    Remember the PTH is done before the traces are etched so the barrels will

    be fully formed and you need only approach the pad from one side as

    soldering in the socket should fully fill the hole and attach to the other

    side of the pad.

     

     

    There is a way to make it work if you don't mind negating the RESTRING

    settings/protection of the Design Rules (DRC)

    In essence, what I'm about to suggest here results in the behaviour most

    people expect work when they begin with Eagle so it should not be an issue

    working this way.

     

    If I make an incorrect statement during this explanation I hope someone

    will correct me.

     

    Two areas need changing

    The DRC rules for the RESTRING

    The PAD diameter of all parts in the library that you use in this design

    with the changed DRC

     

    Change all  the RESTRING settings (top, inner, bottom)

    % of drill diameter = 0%

    Minimum = 0

     

    This causes the DRC to calculate the RESTRING with a width of zero.

     

    What appears on the board is the greater of the DRC calculated width or

    that specified in the library package.

    For most of the packages provided with Eagle the diameter is set to AUTO

    which for this point in our discussion means 'use the DRC calculated size'.

    Note that what you see in the library at this point (diameter set to

    AUTO)is not the DRC calculated size but a size based on, I suspect, the

    default DRC setting. But that is simply to provide a reasonable looking pad

    in the package view. In the background the diameter is likely zero so the

    DRC calculated size will always win.

     

    So with AUTO set for the pad diameter and our new 0% DRC settings, above,

    we get no restrings!!!!Just what we need for your footprint. But it happens

    for all pads on the board. We have to fix that.

     

    For the other packages used on the board we need to change the PAD diameter

    from auto to a specified size. That then becomes the larger of the two

    sizes(zero is the other size) and it is displayed on the board. This is the

    way novices think it should work, i.e. The way it is in the library is how

    it should be on the board, with no change.

     

    What has been lost from the DRC is the automatic creation of minimum

    restrings as specified by board houses.

    It is not hard to ensure when you set pad diameters manually that you

    exceed typical requirements.

     

    In v6 you can make a footprint exactly as depicted in the datasheets you

    identified. There would be no DRC errors(still requires the above

    arrangement though).

    With v5 you could compromise by using a LONG PAD which results in a length

    close to that in the datasheet. Just accept it has round ends.

     

    I feel some board houses may advise that there is insufficient copper

    (Restring) around that PTH hole so you should advise in the documentation

    you send them that it is not a design flaw and is required. 

     

     

    The method may cause quite a bit of work if you have many pads in your

    libraries set to a diameter of AUTO.

    If your board is basically a SMD design with only a few devices with PADs

    then you could modify only those library packages involved.

     

    For other boards you would set the DRC back to its defaults or what is

    normal for your usage. The DRC settinga are retained within the board so

    there is no issue as you move to other boards that used the more normal DRC

    settings.

     

    I feel this restring functionality is one of a few legacy behaviours in

    Eagle that need changes due to the reducing geometries and higher densities

    experienced these days.

     

    Hope this helps

     

    Warren

     

     

     

    --

    Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Reject Answer
    • Cancel
  • Former Member
    0 Former Member over 12 years ago in reply to Former Member

    The pad image won't get all the way to Element14 so here's a link

    especially for those people.

    http://www.eaglecentral.ca/forums/index.php/fa/6289/bb0eb051bd1da2ff3b30d3257c192198/

    --

    Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
element14 Community

element14 is the first online community specifically for engineers. Connect with your peers and get expert answers to your questions.

  • Members
  • Learn
  • Technologies
  • Challenges & Projects
  • Products
  • Store
  • About Us
  • Feedback & Support
  • FAQs
  • Terms of Use
  • Privacy Policy
  • Legal and Copyright Notices
  • Sitemap
  • Cookies

An Avnet Company © 2025 Premier Farnell Limited. All Rights Reserved.

Premier Farnell Ltd, registered in England and Wales (no 00876412), registered office: Farnell House, Forge Lane, Leeds LS12 2NE.

ICP 备案号 10220084.

Follow element14

  • X
  • Facebook
  • linkedin
  • YouTube