メインコンテンツへスキップ

DIsable solder paste for a component

コメント

11件のコメント

  • Brad Levy

    If not as part of a component, I use a shape (not pad) on copper for test points, and place a corresponding shape on the solder mask layer to create the opening, so the point isn't covered by solder mask. You can add the shape (on copper) to a net, so you don't get any design rule violations from using this technique.

    To add points within a component definition is more problematic, because there isn't a way to assign a shape within a component to a net. You can still create and use the component, just expect some design rule check errors which you just have to ignore when you use it.

    Here is a sample PCB symbol for a part with three pads (which will get paste) and a test point (also part of the symbol) connected to one of them:

    When converting a pad to a shape (by right-click -> change shape type) the shape will be unfilled by default.
    So right click the shape again, choose Properties, and check the Filled box to make it filled.
    You will need to add Top Solder Mask and Bottom Solder Mask layers to your Design Technology settings for
    PCB symbols (and for designs you create that will utilize this component) if the Design Technology settings
    for these doesn't already include these layers.
    Here is the view of the part placed on the board, showing the paste as well. You can see the test point
    (being a shape, not a pad) doesn't get auto-generated paste. The rectangular-pad-converted-to-shape
    connecting the pad and test point doesn't have an opening drawn for it on the solder mask layer, so it
    will be covered by solder mask, protecting against any excess solder from the pad flowing onto the test point.

    0
  • Martin Dusek

    Hi Brad,

    thanks for your reply. I don't think defining a test point as a part of a component is good practice. I would like to place the testpoint on arbitrary position on my board. The testpoint must be a standalone component with its schematic and pcb symbol. Is it possible to set no solder paste for a component so no pad of a component will have solder paste?

    0
  • Brad Levy

    I wouldn't usually make them part of another component, either - I was just trying to respond to the wording you used in your original post: "I have a component with some SMD pads. I don't want these SMD pads to be on solder paste layer (they are test points"

    There is not a way in DS PCB (at least, the free version) to tell DS PCB not to create a solder paste opening for a surface mount pad.

    You can have plain copper shapes (which lack the pad number attribute), however, and place solder mask openings over those, which gets you the physical construct you desire. If you draw those in the PCB editor (as opposed to the PCB Symbol editor), you can also assign the copper shape to a net. But unlike pads, plain copper shapes do not have an equivalent in the schematic.

    So if you want a test point component that shows up on the schematic as well as the PCB, then you need to pair a pad in the PCB symbol (which can be linked to a schematic pin, but will have solder) with a very-close-by plain copper shape, and a corresponding shape on the Solder Mask layer, defining an opening in the mask for accessing the test point.
    This is like the component I defined above - except you can get rid of the other two pads, and make the remaining pad very tiny, since its purpose is just schematic linkage, and won't have a component physically mounted to it.

    One thing you need to do in any case where you plan to have solder mask opening without an opening in the paste mask is to make sure you have solder mask layers in your Design Technology. (They don't have to be there if your design doesn't need any solder mask openings except those over pads, which the software autogenerates.) DS PCB  "ORs together" the openings drawn on the solder mask layer with those it generates algorithmically for the pads.

    As I said, you will get some design rule check errors flagged using the test-point-as-a-symbol approach. You just have to live with them, or use a different program for PCB CAD.

    It is the one I most wish there was a cleaner workaround for. But I can live with it.

    If the asymmetry of a tiny pad to the side of the test point bothers you (or you have problems remembering that is where the trace needs to connect to), you can choose an annulus shape for the pad style, and make it with the inner diameter of the annulus just a bit larger than the diameter of the copper shape for the actual test point. That would look like this:

    0
  • Martin Dusek

    OK, so it will always be some kind of workaround.

    I realized that the pads which I don't want to create paste opening for are near the edges of my PCB. So if I crop edges of my pcb I can get rid off paste openings for my testpoints. Let's say my PCB is 10 x 10 units wide and high and its origin is (0; 0). The area which I want to create solder paste openings for is from (1; 1) to (9; 9) (so the edges are excluded from the plot). I tried to modify some numbers in Output Manufacturing Plots, Position tab for my solder paste output. I set Plot From to (1; 1), Plot To (9; 9) and Offset By (1 ; 1) to align all my plots. However, these settings don't crop my solder paste layer.

     

    The question now is how to crop edges of my plot?

    0
  • Brad Levy

    I don't think I'd use plot cropping to achieve the desired result.

    Since you want the test points to show up on the schematic, as well, here is what I would do.

    For this example, I'll create test points for a Microchip six-pin in-circuit-programming (ICP) connection.
    Assume the test pads are for spring loaded pins on 0.1 inch centers.

    I created a 6 pin component:
    I created it using a generic symbol from the DesignSpark schematic symbol library,
    and a simple PCB symbol I created using the wizard, defining a BGA with 1 row and 6 columns, 0.100" spacing, and 0.01" diameter round pads. (You could use even smaller if you'd like - I just wanted ones that wouldn't be small enough to trigger DRC violations on boards with 10 mil line/space drc rules.)
    I assigned the pin mapping 1-1 between the schematic and PCB symbols in the component definition, and defined pin names corresponding to the signal names used by Microchip ICP tools.

    I then placed this component (which I named 6pinICPcon in the component library) on my PCB.

    Next I placed six round circles on copper, 0.026" diameter for the test probes to land on, adjacent to the component. Then I placed six 0.032" round filled circles diameter on the the solder mask layer, to "uncover" the six test points.

    (At this point, you could copy the arrangement of 6 adjacent test points pads and solder mask openings to an otherwise empty board which you could save for quick re-use later via copy-paste to new boards.)

    Then connect things up. Run a trace from each pin of the 6pinICPcon component to the adjacent circle shape on copper, and run the traces from appropriate parts of your circuit to the corresponding points of the 6pinICPcon component, per the schematic.
    The tiny circles will have solder, the bigger ones will not.
    You needn't end up with any DRC errors this way either, 
    and don't need to remember to use any special plot settings.
    You could place the copper circles closer to the ones of the connector component if you desire.

    0
  • Martin Dusek

    Brad, thank you for this extensive tutorial, I will definitely use it for one of my boards.

    I also have this kind of component which mustn't have any solder paste on its pads:

    The component consists of pads connected alternately to just two nets. Above the PCB, there is a conductive rubber that, when pressed, shorts some pads of the component, making contact. The green filled circle is solder mask opening, and the red circle is copper keep out area. They are there to make adjacent area of the component as flat as possible, only exposed ENIG pads being there. I don't think I can use your technique for this components very well as even tiny pads nearby with solder paste applied would cause the area to be not as flat as I need it which can then cause difficulties making contact. I know I can place the tiny pads far away from the actual component, but that would be quite awkward.

    For this PCB, the ideal solution would be to crop the solder paste gerber plot as the components are just near the edges of the PCB. They are the only components near the edges. So, can you please help how to crop gerber plot so it includes just the center of the PCB and it is also aligned with the rest of the plots?

    0
  • Brad Levy

    Nope. This is an easier one. Define the component as having through-hole pads (not vias) arranged around the ring, as you have them. DS PCB doesn't generate paste openings for through-hole pads, so you don't need to worry about placing them far away from your contacts. I'd make the contact pattern separate, on a .pcb file kept around just as a template to easily copy from.

    As an example, for a twelve-direction item similar to the 16-direction one you are defining,
    here is the PCB symbol I defined for HourJoy:


    and the copper shapes pattern saved separately for reuse, in a file I named
    HourJoy.pcb to make it easy to remember:

    Then the component placed on my real actual target board, followed by
    copying the shapes from the HourJoy.pcb, and connecting some of the
    traces from the component to the shapes, and from the component to
    a nearby IC:



    This approach allows a DRC check with no errors, and the component can have
    representation on the schematic as well.
    You do need to remember to draw the traces from the pads you are using to the
    corresponding copper shapes, but that is quick and easy to do, as I've done here
    for the four directions I'm using of the 12-direction pattern. There won't be any
    paste on the pattern or its pads.

    0
  • Martin Dusek

    It seems DS PCB can do anything with clever workarounds :) Thank you.

    However, I would really like to use the plot cropping option. It is way easier for me at the moment as I don't have to redesign my component. Can you please advise how to crop the plot?

    0
  • Brad Levy

    If you read DS PCB's built-in help on Plot Position, it states:

    Plot From/To - This pair of boxes define the lower left and upper right corner of the area to be printed. Normally this defaults to the lower left hand corner of the design, but it can be changed if it is intended to tile a design at a larger scale than normal. Note that these controls can be used to 'crop' the output when writing to Windows devices, but not for Gerber, Excellon, etc, which will all output the complete design data.

    (I added the bold/italic emphasis.)
    It also puts up a warning in the dialog if you attempt to do cropping when outputting to Gerber.

    Even if it didn't, I'd recommend against that approach as likely to cause problems/confusion when it goes to the board manufacturer and the films don't match in size/extents.

    But I've given you a way to do it without cropping. And now need to get back to my own projects.
    (I'm just another user - not a DesignSpark employee.)

    It really shouldn't take you too long to do it using the component + copper shapes approach, since it looks like you already have the copper shapes drawn, which you can copy/paste.from.
    And you can create the ring-of-through-hole pads very quickly using the PCB symbol wizard (choose the Can component type).

    The one step I forgot to include in my example was to draw an opening on the solder mask layer for copper shapes. I would think one circle big enough to encompass them all would do, and be more reliable than individual openings for each wedge, which might leave solder mask thick enough in between them to interfere with the conductive rubber pad going all the way down to make consistent connection across the copper.



    0
  • Martin Dusek

    I see. So, DesignSpark can't crop gerbers. Thanks.

    0
  • Martin Dusek

    For gerber clipping we can use https://github.com/ThisIsNotRocketScience/GerberTools/tree/master/GerberClipper. Very nice set of tools. Just call the clipper: GerberClipper.exe clip.gko in.gbr out.gbr . The clip gerber must be with .gko suffix.

    0

サインインしてコメントを残してください。