Is there anything wrong with placing vias on surface mount pads?

Discussion in 'Electronic Design' started by Mike Noone, Apr 9, 2006.

  1. Mike Noone

    Mike Noone Guest

    Hi - I'm working on a really, really tight layout right now. I have a
    number of 0603 resistors very closely packed with a number of vias going to
    them. Would it be OK to place the vias directly in the center of one of a
    0603's pads? This is for a prototype board, and will be hand assembled. Gut
    instinct says go for it, but my layout editor is yelling at me so I thought
    I should check just to be sure. Thanks,

    -Mike
    Mike Noone, Apr 9, 2006
    #1
  2. Mike Noone

    Terry Given Guest

    John Popelish wrote:
    > Mike Noone wrote:
    >
    >> Hi - I'm working on a really, really tight layout right now. I have a
    >> number of 0603 resistors very closely packed with a number of vias
    >> going to them. Would it be OK to place the vias directly in the center
    >> of one of a 0603's pads? This is for a prototype board, and will be
    >> hand assembled. Gut instinct says go for it, but my layout editor is
    >> yelling at me so I thought I should check just to be sure. Thanks,

    >
    >
    > For hand soldering it might work okay, but it tends to wick the solder
    > down the via, causing a dry joint or tomb stoning (the part is pulled up
    > on one end during re flow soldering by the uneven surface tension).


    unless you use a very, very small hole ($$$)

    Cheers
    Terry
    Terry Given, Apr 9, 2006
    #2
  3. Mike Noone wrote:
    > Hi - I'm working on a really, really tight layout right now. I have a
    > number of 0603 resistors very closely packed with a number of vias going to
    > them. Would it be OK to place the vias directly in the center of one of a
    > 0603's pads? This is for a prototype board, and will be hand assembled. Gut
    > instinct says go for it, but my layout editor is yelling at me so I thought
    > I should check just to be sure. Thanks,


    For hand soldering it might work okay, but it tends to wick the solder
    down the via, causing a dry joint or tomb stoning (the part is pulled
    up on one end during re flow soldering by the uneven surface tension).
    John Popelish, Apr 9, 2006
    #3
  4. Mike Noone

    Hal Murray Guest

    In article <Xns979FEBE0E4808mnooneuiucedu127001@63.240.76.16>,
    Mike Noone <mnoone.uiuc.edu@127.0.0.1> writes:
    >Hi - I'm working on a really, really tight layout right now. I have a
    >number of 0603 resistors very closely packed with a number of vias going to
    >them. Would it be OK to place the vias directly in the center of one of a
    >0603's pads? This is for a prototype board, and will be hand assembled. Gut
    >instinct says go for it, but my layout editor is yelling at me so I thought
    >I should check just to be sure. Thanks,


    google for via-in-pad.

    It's sometimes used to reduce the inductance on bypass caps.

    The usual problem is that the hole in the via sucks up some
    of the solder applied by the normal solder-paste through a
    stencil approach so there isn't enough left for a good solder
    joint. That shouldn't be a problem if you are hand soldering
    a proto board.

    Make sure you have enough room to get the soldering iron in
    to solder the resistors.

    --
    The suespammers.org mail server is located in California. So are all my
    other mailboxes. Please do not send unsolicited bulk e-mail or unsolicited
    commercial e-mail to my suespammers.org address or any of my other addresses.
    These are my opinions, not necessarily my employer's. I hate spam.
    Hal Murray, Apr 9, 2006
    #4
  5. Mike Noone

    Robert Baer Guest

    Terry Given wrote:
    > John Popelish wrote:
    >
    >> Mike Noone wrote:
    >>
    >>> Hi - I'm working on a really, really tight layout right now. I have a
    >>> number of 0603 resistors very closely packed with a number of vias
    >>> going to them. Would it be OK to place the vias directly in the
    >>> center of one of a 0603's pads? This is for a prototype board, and
    >>> will be hand assembled. Gut instinct says go for it, but my layout
    >>> editor is yelling at me so I thought I should check just to be sure.
    >>> Thanks,

    >>
    >>
    >>
    >> For hand soldering it might work okay, but it tends to wick the solder
    >> down the via, causing a dry joint or tomb stoning (the part is pulled
    >> up on one end during re flow soldering by the uneven surface tension).

    >
    >
    > unless you use a very, very small hole ($$$)
    >
    > Cheers
    > Terry

    Better yet, use same size hole on both pads, and centered.
    Robert Baer, Apr 9, 2006
    #5
  6. Mike Noone

    Terry Given Guest

    Robert Baer wrote:
    > Terry Given wrote:
    >
    >> John Popelish wrote:
    >>
    >>> Mike Noone wrote:
    >>>
    >>>> Hi - I'm working on a really, really tight layout right now. I have
    >>>> a number of 0603 resistors very closely packed with a number of vias
    >>>> going to them. Would it be OK to place the vias directly in the
    >>>> center of one of a 0603's pads? This is for a prototype board, and
    >>>> will be hand assembled. Gut instinct says go for it, but my layout
    >>>> editor is yelling at me so I thought I should check just to be sure.
    >>>> Thanks,
    >>>
    >>>
    >>>
    >>>
    >>> For hand soldering it might work okay, but it tends to wick the
    >>> solder down the via, causing a dry joint or tomb stoning (the part is
    >>> pulled up on one end during re flow soldering by the uneven surface
    >>> tension).

    >>
    >>
    >>
    >> unless you use a very, very small hole ($$$)
    >>
    >> Cheers
    >> Terry

    >
    > Better yet, use same size hole on both pads, and centered.


    unless its a big hole - reductio ad absurdum, it better be smaller than
    the pad.....

    some contract manufacturers may refuse to make such a PCB.

    Cheers
    Terry
    Terry Given, Apr 9, 2006
    #6
  7. Mike Noone

    Fred Bartoli Guest

    "Terry Given" <> a écrit dans le message de
    news:1144566268.862502@ftpsrv1...
    > Robert Baer wrote:
    > > Terry Given wrote:
    > >
    > >> John Popelish wrote:
    > >>
    > >>> Mike Noone wrote:
    > >>>
    > >>>> Hi - I'm working on a really, really tight layout right now. I have
    > >>>> a number of 0603 resistors very closely packed with a number of vias
    > >>>> going to them. Would it be OK to place the vias directly in the
    > >>>> center of one of a 0603's pads? This is for a prototype board, and
    > >>>> will be hand assembled. Gut instinct says go for it, but my layout
    > >>>> editor is yelling at me so I thought I should check just to be sure.
    > >>>> Thanks,
    > >>>
    > >>>
    > >>>
    > >>>
    > >>> For hand soldering it might work okay, but it tends to wick the
    > >>> solder down the via, causing a dry joint or tomb stoning (the part is
    > >>> pulled up on one end during re flow soldering by the uneven surface
    > >>> tension).
    > >>
    > >>
    > >>
    > >> unless you use a very, very small hole ($$$)
    > >>
    > >> Cheers
    > >> Terry

    > >
    > > Better yet, use same size hole on both pads, and centered.

    >
    > unless its a big hole - reductio ad absurdum, it better be smaller than
    > the pad.....
    >
    > some contract manufacturers may refuse to make such a PCB.
    >


    Making the PCB? Why would they?

    Of course, making the whole assembly is another matter.


    --
    Thanks,
    Fred.
    Fred Bartoli, Apr 9, 2006
    #7
  8. Mike Noone

    Joerg Guest

    Hello Mike,


    > Hi - I'm working on a really, really tight layout right now. I have a
    > number of 0603 resistors very closely packed with a number of vias going to
    > them. Would it be OK to place the vias directly in the center of one of a
    > 0603's pads? This is for a prototype board, and will be hand assembled. Gut
    > instinct says go for it, but my layout editor is yelling at me so I thought
    > I should check just to be sure. Thanks,
    >


    I wouldn't do that. With one exception: When I need a really low
    impedance to other layers, for example in case of a connection area for
    chassis ground or a high amperage power supply cable (the garden hose
    size wires).

    Consider smaller resistors. You can go much smaller than 0603 and
    nowdays smaller sizes are almost standard. But mind the dissipation,
    probably need to run ye olde HP calculator on every resistor that is low
    enough in ohms and across a few volts.

    Regards, Joerg

    http://www.analogconsultants.com
    Joerg, Apr 9, 2006
    #8
  9. Mike Noone

    Terry Given Guest

    Fred Bartoli wrote:
    > "Terry Given" <> a écrit dans le message de
    > news:1144566268.862502@ftpsrv1...
    >
    >>Robert Baer wrote:
    >>
    >>>Terry Given wrote:
    >>>
    >>>
    >>>>John Popelish wrote:
    >>>>
    >>>>
    >>>>>Mike Noone wrote:
    >>>>>
    >>>>>
    >>>>>>Hi - I'm working on a really, really tight layout right now. I have
    >>>>>>a number of 0603 resistors very closely packed with a number of vias
    >>>>>>going to them. Would it be OK to place the vias directly in the
    >>>>>>center of one of a 0603's pads? This is for a prototype board, and
    >>>>>>will be hand assembled. Gut instinct says go for it, but my layout
    >>>>>>editor is yelling at me so I thought I should check just to be sure.
    >>>>>>Thanks,
    >>>>>
    >>>>>
    >>>>>
    >>>>>
    >>>>>For hand soldering it might work okay, but it tends to wick the
    >>>>>solder down the via, causing a dry joint or tomb stoning (the part is
    >>>>>pulled up on one end during re flow soldering by the uneven surface
    >>>>>tension).
    >>>>
    >>>>
    >>>>
    >>>>unless you use a very, very small hole ($$$)
    >>>>
    >>>>Cheers
    >>>>Terry
    >>>
    >>> Better yet, use same size hole on both pads, and centered.

    >>
    >>unless its a big hole - reductio ad absurdum, it better be smaller than
    >>the pad.....
    >>
    >>some contract manufacturers may refuse to make such a PCB.
    >>

    >
    >
    > Making the PCB? Why would they?
    >
    > Of course, making the whole assembly is another matter.


    dont laugh, i really have had contract mfgs piss and moan about IPCD275
    and IPCSM782 - no comply, no build. And I meant populate the pcb, not
    fabricate it (although I have had a pcb mfg refuse to make single-sided
    PCBs with rivets, cant say as I blame them).

    Cheers
    Terry
    Terry Given, Apr 9, 2006
    #9
  10. Mike Noone

    Boris Mohar Guest

    On Sun, 09 Apr 2006 04:11:19 GMT, Mike Noone <mnoone.uiuc.edu@127.0.0.1>
    wrote:

    >Hi - I'm working on a really, really tight layout right now. I have a
    >number of 0603 resistors very closely packed with a number of vias going to
    >them. Would it be OK to place the vias directly in the center of one of a
    >0603's pads? This is for a prototype board, and will be hand assembled. Gut
    >instinct says go for it, but my layout editor is yelling at me so I thought
    >I should check just to be sure. Thanks,
    >
    >-Mike


    If you are hand soldering the you can get away with it. Otherwise use
    conductive via plug CB100 from Dupont.



    Regards,

    Boris Mohar

    Got Knock? - see:
    Viatrack Printed Circuit Designs (among other things) http://www.viatrack.ca

    void _-void-_ in the obvious place
    Boris Mohar, Apr 9, 2006
    #10
  11. Mike Noone

    Gary Pace Guest

    "Mike Noone" <mnoone.uiuc.edu@127.0.0.1> wrote in message
    news:Xns979FEBE0E4808mnooneuiucedu127001@63.240.76.16...
    > Hi - I'm working on a really, really tight layout right now. I have a
    > number of 0603 resistors very closely packed with a number of vias going
    > to
    > them. Would it be OK to place the vias directly in the center of one of a
    > 0603's pads? This is for a prototype board, and will be hand assembled.
    > Gut
    > instinct says go for it, but my layout editor is yelling at me so I
    > thought
    > I should check just to be sure. Thanks,
    >
    > -Mike


    I think some fab manufacturers can solid-fill (plug) the via so the solder
    doesn't wick down the hole.
    Gary Pace, Apr 9, 2006
    #11
  12. Mike Noone

    Al Guest

    In article <R1d_f.10896$>,
    "Gary Pace" <> wrote:

    > "Mike Noone" <mnoone.uiuc.edu@127.0.0.1> wrote in message
    > news:Xns979FEBE0E4808mnooneuiucedu127001@63.240.76.16...
    > > Hi - I'm working on a really, really tight layout right now. I have a
    > > number of 0603 resistors very closely packed with a number of vias going
    > > to
    > > them. Would it be OK to place the vias directly in the center of one of a
    > > 0603's pads? This is for a prototype board, and will be hand assembled.
    > > Gut
    > > instinct says go for it, but my layout editor is yelling at me so I
    > > thought
    > > I should check just to be sure. Thanks,
    > >
    > > -Mike

    >
    > I think some fab manufacturers can solid-fill (plug) the via so the solder
    > doesn't wick down the hole.
    >
    >


    The problem with vias on pads that are soldered is that they develop
    circumferential fractures at the via/pad joint. Now if the via is solder
    filled, then the fracture may not bother you. If you hand solder them,
    it really makes them problamatic.

    Al
    Al, Apr 9, 2006
    #12
  13. Mike Noone

    Roy L. Fuchs Guest

    On Sun, 09 Apr 2006 10:07:33 -0400, Boris Mohar
    <> Gave us:

    >On Sun, 09 Apr 2006 04:11:19 GMT, Mike Noone <mnoone.uiuc.edu@127.0.0.1>
    >wrote:
    >
    >>Hi - I'm working on a really, really tight layout right now. I have a
    >>number of 0603 resistors very closely packed with a number of vias going to
    >>them. Would it be OK to place the vias directly in the center of one of a
    >>0603's pads? This is for a prototype board, and will be hand assembled. Gut
    >>instinct says go for it, but my layout editor is yelling at me so I thought
    >>I should check just to be sure. Thanks,
    >>
    >>-Mike

    >
    > If you are hand soldering the you can get away with it. Otherwise use
    >conductive via plug CB100 from Dupont.
    >
    >
    >
    >Regards,
    >
    >Boris Mohar
    >
    >Got Knock? - see:
    >Viatrack Printed Circuit Designs (among other things) http://www.viatrack.ca
    >
    >void _-void-_ in the obvious place
    >
    >

    All one needs to do is MASK over the via on the other side of the
    board.
    Roy L. Fuchs, Apr 9, 2006
    #13
  14. Mike Noone

    Roy L. Fuchs Guest

    On Sun, 09 Apr 2006 19:13:53 GMT, "Gary Pace"
    <> Gave us:

    >
    >"Mike Noone" <mnoone.uiuc.edu@127.0.0.1> wrote in message
    >news:Xns979FEBE0E4808mnooneuiucedu127001@63.240.76.16...
    >> Hi - I'm working on a really, really tight layout right now. I have a
    >> number of 0603 resistors very closely packed with a number of vias going
    >> to
    >> them. Would it be OK to place the vias directly in the center of one of a
    >> 0603's pads? This is for a prototype board, and will be hand assembled.
    >> Gut
    >> instinct says go for it, but my layout editor is yelling at me so I
    >> thought
    >> I should check just to be sure. Thanks,
    >>
    >> -Mike

    >
    >I think some fab manufacturers can solid-fill (plug) the via so the solder
    >doesn't wick down the hole.
    >

    Solder mask is silk screened on wet. All he needs to do is make
    sure the mask covers any vias that he wants to keep wick free.

    They only need to plug one side. It will not affect the via
    integrity.
    Roy L. Fuchs, Apr 9, 2006
    #14
  15. Mike Noone

    John_H Guest

    Mike Noone wrote:
    > Hi - I'm working on a really, really tight layout right now. I have a
    > number of 0603 resistors very closely packed with a number of vias going to
    > them. Would it be OK to place the vias directly in the center of one of a
    > 0603's pads? This is for a prototype board, and will be hand assembled. Gut
    > instinct says go for it, but my layout editor is yelling at me so I thought
    > I should check just to be sure. Thanks,
    >
    > -Mike


    "Filled vias" is what to google on. The hole-in-pad is doable but not
    all PC board vendors happily provide them and it is an additional cost.
    John_H, Apr 10, 2006
    #15

Want to reply to this thread or ask your own question?

It takes just 2 minutes to sign up (and it's free!). Just click the sign up button to choose a username and then you can ask your own questions on the forum.
Similar Threads
  1. MM
    Replies:
    8
    Views:
    201
  2. M. Noone
    Replies:
    24
    Views:
    609
    joseph2k
    May 16, 2006
  3. veeresh

    placing components above thermal vias

    veeresh, Jul 2, 2007, in forum: Electronic Design
    Replies:
    9
    Views:
    317
    Jasen Betts
    Jul 8, 2007
  4. Michael
    Replies:
    10
    Views:
    810
  5. Kasterborus
    Replies:
    3
    Views:
    425
Loading...

Share This Page