Zum Hauptinhalt gehen

Paste Stencil Sizing

Kommentare

8 Kommentare

  • Offizieller Kommentar
    DesignSpark PCB

    This topic has also been discussed on the support desk and a FAQ which discusses an alternative setting of the paste mask aperture has been produced using the "relative" option in the Design Technology.

    https://designspark.zendesk.com/hc/en-us/articles/115003126389-How-can-I-edit-the-mask-apertures-settings- 

    The 'relative' option allows the paste mask gap to be defined as a percentage of the pad size, hence allowing more solder paste to be applied on smaller pads.

  • Jayx .

    Hi Steven,

    Is the copper land size 0.200 x 0.275mm? It looks like SOD962 package. That's extremely small, you'll need some special approach for it: stencil should be 0.1mm thick, apertures 0.2mm circle, very fine grain solder paste (type 4 or type 5) and good precision pick&place machine (±0.05mm).

    0
  • Steven Pigliavento

    Thank you Jayx.

    Yes, my land pattern consists of 0.200 x 0.275mm pads ... for an STM LGA-14, 2x2mm sensor package.  See inserted pic.

    Red is top copper and small brown inset pads are the paste stencil pads or openings ... dimensionally driven by aforementioned Min. Paste Size parameter ... which defaults to 0.076mm.  I'm trying to change this parameter for the precise reason that can be viewed in the image, for which a description is provided in the DS PCB manual:

    In the above DS PCB setup & help screenshots, the problem that I'm looking to resolve is the Min. Paste Size parameter does not seem to be correcting the paste stencil pad size (brown in the above artwork view).

    Any assistance is appreciated.

    -s, ny

    0
  • Brad Levy

    Hi Steven,

    I played around with the Min Paste Size setting here after seeing your post. I wasn't sure whether it was supposed to actively influence the size of the generated openings, or whether it was just supposed to be used for design rule checking (flagging occurrences where the openings don't meet the minimum). It didn't *seem* to do either, although I didn't have time to test extensively.

    One method you could use if the paste openings are too small is to explicitly add paste openings on a paste mask layer in the PCB symbol. Make sure you have paste mask layers defined as part of the design techology you are using for both the PCB board and for PCB symbols. . (Add them if they aren't already there.)  Then draw the openings on the paste layer in the PCB Symbol editor, placing them coincident with the respective pads. DS PCB will combine any openings drawn on the paste layer with the openings it auto-generates for SMD pads

    -Brad
    (just another user)

    0
  • Jayx .

    OK, so not SOD962 package but very similar pad sizes so rules for stencil thickness/paste type/apertures will be the same.

    Anyway it seems to be some problem with stencil openings, did you have them like that generated automatically by DSPCB? It’s not driven by Min. Paste Size parameter, as Brad says it’s rather for DRC check to flag too small openings - it is working and producing error messages if violated, see picture (I’ve set it to 0.3mm for test).

    As Brad says you can add openings manually, but the ones generated automatically seems to be correct, unless there is some problem with this setting. Can you post your Paste Layer settings from the Design Technology section?

    0
  • Steven Pigliavento

    Brad & Jayx,

    Very much appreciate you both lending a hand on this one.  I'm quite familiar with the 'adding the information to the part decal definition' ... in Mentor/PADS.  Perhaps I underestimated DS PCB as not supporting that level of customization.  That said, I did see differences between my LGA-14 part's Design Technology and the base design's Design Technology; e.g., the part def not having an explicit Top Paste Layer (added).

    I'll experiment a bit more with this and follow-up in this thread.

    Will also run the DRCs with paste mask checked.

    Kind regards from NY,

    -s

     

    0
  • Steven Pigliavento

    Brad, Jayx:

    I was able to confirm that the Min. Paste Size DRC check was in fact driven by the parameter that we set in Design Technology/Rules.  That's good.

    My understanding, then, is that the above parameter does not drive the size, rather, just the checking of the size.

    I further experimented with adding Paste Mask Layer to Design Technology in the part symbol editor window.  Could not setup / confirm that DS PCB supports adding explicit paste layer features to a part decal.  As mentioned, this is standard stuff with $pricier tools -- Mentor/PADS -- and I get that this unbelievably capable/free product cannot support all of the higher-end features.

    Any forum, tutorial, help links that you might share that demonstrate/work through how explicit paste mask pad sizes can be pre-set in the part symbol editor?

    Much thanks.

    -s, ny

    0
  • DesignSpark PCB

    This requirement of achieving greater solder paste on small pads is discussed in a new FAQ https://designspark.zendesk.com/hc/en-us/articles/115003126389-How-can-I-edit-the-mask-apertures-settings- 

    The option in the Design Technology to select a "Relative" size of the paste mask opening as a percentage of the pad size is described.

    0

Bitte melden Sie sich an, um einen Kommentar zu hinterlassen.