Cannot set layer for test point pad

Comments

4 comments

  • Avatar
    Boss .

    Hi Bill, not sure why you have that behaviour, but another issue you will face is solder paste on the pad. Have a look at https://designspark.zendesk.com/hc/en-us/articles/115003349025-How-can-I-add-a-fiducial-mark-to-my-PCB- which shows how to get a copper area (pad) without solder paste and should not have the issue you are experiencing.

    1
    Comment actions Permalink
  • Avatar
    Brad Levy

    Bill, I take it you were trying to change it from [All] layers to [Top] layer by editing the properties of the pad in the PCB editor after placing the component on your PCB. You can (if you check the Pad Exception box in the properties editor) change the style of the pad, but not its type (through-hole vs SMD, which is controlled by the Layer: setting).
    The way to fix it is open the library manager (ctrl-L), and edit the PCB Symbol you are using for your Test Pad component. The PCB symbol editor does let you select the Layer assignment for the pad. If you change it to [Top], it will be on the top layer when you later place the component on the PCB. Once it is on your PCB, you can use the Flip command to flip it from the top side to the bottom side of the PCB.

    If you need a component that is in some cases through-hole and other cases surface mount, you can define two PCB Symbols (one through-hole, one surface mount), and define the Component in the library as having two available packages, one using the through-hole PCB Symbol, and the other using the surface mount PCB Symbol.

    As Boss pointed out, though, if you want a test point without solder paste, you need to create the test point as a shape on the copper layer and a corresponding shape on the solder mask layer. Unlike a fiducial which you usually don't connect to a net, you do want your test point connected to a net. You can make a PCB Symbol like the following:
    Where the highlighted white rectangle is an actual pad, and the red is a shape on the copper layer, and the same red shape is copied to the solder mask layer of the symbol. (You'd need to include a solder mask layer in your design technology of the PCB Symbol, and also in the design technology of the board you are placing the test points on.
    The red portion then gives you a test point without solder paste (so you get good contact), and the highlighted pad gives you a place to connect the pad to a net. You can make the rectangle (which will have solder paste) smaller if you want.

     

    -Brad

    1
    Comment actions Permalink
  • Avatar
    Brad Levy

    The one disadvantage to the test points is that you will get a design rule check error about the pad overlapping the shape. You can safely ignore the error, because you know the overlap was intentional in this case. But it would be nice if we could turn off that message on a per-PCB-Symbol basis.

    0
    Comment actions Permalink
  • Avatar
    Bill Marriott

    Thanks for the tips - Brad's tip to edit the component fixed my problem and I actually prefer that test points get solder on them since it helps  probes dig in so they don't slide around when using the test point

     

    Bill

    0
    Comment actions Permalink

Please sign in to leave a comment.