---
+ Post New Thread
Results 1 to 20 of 20
  1. #1
    Advanced Member level 2
    Points: 4,439, Level: 15

    Join Date
    Oct 2004
    Posts
    521
    Helped
    29 / 29
    Points
    4,439
    Level
    15

    How to tent via with soldermask on Protel, PADS and Allegro?

    I want to know how we can tent via with soldermask on Protel, PADS and Allegro?
    Is it possible to make it conditional vi tenting(under some component)?

  2. #2
    Full Member level 5
    Points: 3,795, Level: 14

    Join Date
    Dec 2002
    Posts
    288
    Helped
    34 / 34
    Points
    3,795
    Level
    14

    tented vias

    Just do not define solder mask for those vias.
    You can have different vias in your design.

    Is advisable to add a note on FAB drawing also.

    Regards,
    M



  3. #3
    Advanced Member level 2
    Points: 4,439, Level: 15

    Join Date
    Oct 2004
    Posts
    521
    Helped
    29 / 29
    Points
    4,439
    Level
    15

    tented via

    VIA always has the soldermask and removing it needs a special care. In AD we need to check the via tenting check box of via preperty dialog box.
    I need to know to do same job on PADS and Allegro? Do I need to define special VIA or I can edit exiting vias?



  4. #4
    Full Member level 5
    Points: 3,795, Level: 14

    Join Date
    Dec 2002
    Posts
    288
    Helped
    34 / 34
    Points
    3,795
    Level
    14

    solder mask tenting

    VIA always has the soldermask and removing it needs a special care.
    What do you mean by that? What special care you are referring to?!!!

    Simply edit your via pad. Done that many many times.
    Is not tool related any tool can do this simple task.



    •   Alt10th September 2007, 16:22

      advertising

        
       

  5. #5
    Full Member level 6
    Points: 3,824, Level: 14

    Join Date
    Dec 2005
    Location
    BANGALORE
    Posts
    369
    Helped
    45 / 45
    Points
    3,824
    Level
    14

    tenting vias

    Hi,

    Tenting is a process usually delegated to dry film masks. In this process the via is completely covered to prevent cleaning solutions or flux residue from entering the plated-through hole. An issue still in debate is whether to tent one side or both sides of the via. Many users have different opinions as to which method works best in a good assembly process. With the advent and the increased use of liquid photoimageable masks, the tenting of vias has not always been possible.

    The liquid polymer applied to the surface, some solder mask gets into the hole. However, there can be skips or other process conditions where the solder mask does not properly cover or prevent entrance into the barrel of the plated-through hole. Thus, capping* or plugging* has come about. This is usually a secondary process to ensure that plated-through holes are really prevented from being open to contamination from some of the assembly cleaning and plating process chemistries.

    Capping - Via holes are Capped with Overplate
    Plugging - Via holes are Plugged with LPI mask or DuPont Silver Epoxy


    Hope this helps you.

    Regards

    Ramesh


    1 members found this post helpful.

  6. #6
    Member level 1
    Points: 1,258, Level: 8

    Join Date
    Dec 2006
    Posts
    32
    Helped
    2 / 2
    Points
    1,258
    Level
    8

    tenting pcb

    You should need a fab note in the fab drawing to describe the via tented.



  7. #7
    Advanced Member level 2
    Points: 4,439, Level: 15

    Join Date
    Oct 2004
    Posts
    521
    Helped
    29 / 29
    Points
    4,439
    Level
    15

    pcb tenting

    is via tenting a common practice in multi-layer board?



  8. #8
    Member level 2
    Points: 1,142, Level: 7

    Join Date
    Nov 2007
    Location
    CHINA
    Posts
    45
    Helped
    1 / 1
    Points
    1,142
    Level
    7

    tenting via

    Absolutely not common. Only some engineers prefer to do so. It depends on personal style.

    Anyway, whether tent or not, please noted it out on mechanical drawing to avoid misunderstanding.



    •   Alt29th November 2007, 22:14

      advertising

        
       

  9. #9
    Member level 1
    Points: 1,376, Level: 8
    eswar_babu77's Avatar
    Join Date
    Oct 2006
    Posts
    41
    Helped
    3 / 3
    Points
    1,376
    Level
    8

    via-tenting

    Few people will use the via as test points and in that case they remove the solder mask layer from vias or particular via which will be used as test point. When BGA is used in the design and fanout is done, normally vias beneath them is tented to avoid solder flow / shorting.



    •   Alt30th November 2007, 09:43

      advertising

        
       

  10. #10
    Member level 2
    Points: 1,262, Level: 8

    Join Date
    Nov 2006
    Posts
    51
    Helped
    1 / 1
    Points
    1,262
    Level
    8

    pcb via tenting

    It's better to tent the via holes. If you really want to use these via holes for testing purpose, you can leave only those required with soldermask clearance.



  11. #11
    Advanced Member level 3
    Points: 6,839, Level: 19
    buenos's Avatar
    Join Date
    Oct 2005
    Location
    Sunnyvale, California, USA
    Posts
    937
    Helped
    40 / 40
    Points
    6,839
    Level
    19

    tenting pcb via

    if you use QFPs and a huge amount of VIAs under the component, close to the pins, definitely use VIA tenting, at least under the components. this is to avoid short circuit made by left-over soldertin.
    also for BGAs, is highly recommended to cover the dogbone-vias. I have tried a board with a BGA and without viatenting. we checked with X-ray. It didnt look good:http://www.buenos.extra.hu/dspboard.html

    normally i specify testpoint-vias, they are not tented, but the others are

    Added after 3 hours 4 minutes:

    oh, and how do I specify it in Cadence Allegro?
    (I used it only in Altium, until now)


    1 members found this post helpful.

  12. #12
    Member level 1
    Points: 1,376, Level: 8
    eswar_babu77's Avatar
    Join Date
    Oct 2006
    Posts
    41
    Helped
    3 / 3
    Points
    1,376
    Level
    8

    what is a tented via

    In allegro you can edit the padstack which is used for dog bone structure under BGA area and do not define solder mask bottom.



  13. #13
    Newbie level 3
    Points: 823, Level: 6

    Join Date
    May 2008
    Posts
    3
    Helped
    0 / 0
    Points
    823
    Level
    6

    tenting of vias

    Hi

    i wonder if someone can help me on this topic: i have a via-in-pad, the type you put on exposed pad lands and connect to ground layer and i am using Allegro package designer. so i need to plug those vias to avoid wicking during soldering of the component: In allegro, defining any shape on soldermask layer means an opening; so currently, i create a void to indicate soldermask tenting of the vias... but im not sure this solves the problem... any other ideas besides sending a note with the drawings??



  14. #14
    FvM
    FvM is offline
    Super Moderator
    Points: 173,544, Level: 98
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    28,255
    Helped
    8885 / 8885
    Points
    173,544
    Level
    98

    vias tenting

    To my opinion, design of via in a pad isn't a problem of PCB tools but a question of PCB manufacturer technology. Sometimes tenting or special soldermask structures are suggested for thermal vias in an exposed pad, e. g. in an Amkor application note:http://www.amkor.com/products/notes_...MLFAppNote.pdf

    The problem is, that depending on the PCB manufacturers technology, such solutions can completely fail according to my experience. So it's generally advisable to check the possible techniques with the manufacturer before finishing the design. Apart from using soldermask for covering the vias, special plugging techniques are available from many PCB manufacturers, including copper plated plugs that allow for vias in BGA or CSP pads. But these techniques require additional processing steps and increase PCB costs.



  15. #15
    Advanced Member level 3
    Points: 6,839, Level: 19
    buenos's Avatar
    Join Date
    Oct 2005
    Location
    Sunnyvale, California, USA
    Posts
    937
    Helped
    40 / 40
    Points
    6,839
    Level
    19

    what is tented vias

    make some gerber files! then check with a gerber viewer. it will tell you if your action was successful or not. gerbers dont lie...


    1 members found this post helpful.

  16. #16
    Newbie level 3
    Points: 823, Level: 6

    Join Date
    May 2008
    Posts
    3
    Helped
    0 / 0
    Points
    823
    Level
    6

    tenting a via

    Thanks for the replies... i will do as you say Buenos.. i was being lazy but again according to FVM, i think this tenting is not so sure... so im trying this comrpomise: let the solder wicking occur and close via from bottom layer..



  17. #17
    FvM
    FvM is offline
    Super Moderator
    Points: 173,544, Level: 98
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    28,255
    Helped
    8885 / 8885
    Points
    173,544
    Level
    98

    tented vias heat

    The said Amkor application note finds this result in a comparative test of different solder mask designs:
    Code:
    both via tenting from bottom or via plugging from bottom may result in larger voids due to out-gassing
    With one manufacturer, I experienced solder resist traces in the pad area around a via closed from the bottom, thus thermal resistance of the pad was considerably increased. It may be a better solution to use open vias with minimum drill diameter and accept solder wicking, this option also looks good in the Amkor report. However, a assembly service provider feared solder shorts with CSP or MLF devices (packages with planar pads at the bottom) when the device is sucked down to the board.



  18. #18
    Newbie level 6
    Points: 1,283, Level: 8

    Join Date
    Feb 2006
    Location
    Philippines
    Posts
    13
    Helped
    1 / 1
    Points
    1,283
    Level
    8

    what is tenting need on via hole on pcb

    @ELI75

    via on pad technology is process where pcb fab house put fillet on the hole before putting as smt pad to secure metal not to go inside the drill hole. but this technology is a little bit expensive than the usual fabrication process. you wont encounter a DRC violation in allegro for this but as a PCB designer i wont recommend the use of via on pad unless space constraint.

    its just my two cent



  19. #19
    FvM
    FvM is offline
    Super Moderator
    Points: 173,544, Level: 98
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    28,255
    Helped
    8885 / 8885
    Points
    173,544
    Level
    98

    capped via tented via

    I agree, that one should try to use standard technologies as far as possible. If exposed pads have to be contacted, the vias can be probably placed outside the solder area. For higher thermal load, the exposed pad can be e. g. partitioned by two crossing rows of completely tented vias through the center.

    If individual tented vias in a exposed pad have to be designed, the solder mask pattern usually has to be assembled from a number of complex shapes. As the CAD system behaviour may be partly surprizing in the reproduction of such shapes, it's strongly recommended to check the results in a gerber viewer as buenos suggested.



  20. #20
    Newbie level 3
    Points: 823, Level: 6

    Join Date
    May 2008
    Posts
    3
    Helped
    0 / 0
    Points
    823
    Level
    6

    tent via holes

    this exposed pad is quite big wrt footprint area... its supposed to dissipate heat and short connect to ground... hence suppliers are always mentioning these vias or feedthru holes as a matrix under the pads... so anythign that jeopardizes the low impedance or thermal dissipation is not a solution (correct me if im wrong)... oh i dont know.. so whats the cheap and reliable solution? i guess that the assembly house will have some solution...



+ Post New Thread
Please login