Zum Hauptinhalt gehen

Create Custom Shape PAD


6 Kommentare

  • Boss .

    Can you post the shape of the pad you require. BradLevy has done a lot of work on different pad shapes so I'm sure something will be possible to fabricate.


    I have a similar issue for a chamfer:



  • Sumir Sumir

    Yes, as Murphy has posted the picture of the pad which is not available in design sparks by default.


    My pad is little similar to the Murphy's.


    Please tell us, is there any way in general to make a custom PaD in the software. I tried so hard to find any way, but I couldn't.



  • Himanshu Sharma

    Hello members

    please help me out that how can i add or make half plated holes that are used in board to board connectoions.

    i am not understanding that how to make that pad and add in my PCB design.

     I tried so hard to find any way, but I couldn't. 

     I been stuck in this problem for weeks,

    Thanks & Regards

    Himanshu Sharma

  • DesignSpark PCB

    Hello Himanshu, new requests such as this should have their own subject as a new post or they will be lost down in the replies to old questions.

    Obviously to produce a half hole or castellation a full hole has to be produced first. The PCB must therefore be larger than the actual size required and obey spacing rules.

    PCB manufacturers vary in their requirements of the hole size and copper pad size so check this is met.

    Next instruction is required to identify the final board outline, this can be done on the documentation layer.

    A very important requirement is to discuss with the PCB manufacturer your precise requirements and how and where it is documented. It would be even better to contact them and state your requirements and ask how they would like the documentation produced such that the potential for mistakes is removed.

    As an example of a 'special' requirements for slotted holes in pads please see this item 

    It would be good if you could also share your experiences in creating these and the final results.

  • Brad Levy

    I just noticed that the original question that started this thread and Murphy's similar question didn't get fully addressed, at least in this thread. So I'll go ahead and explain a method for achieving desired custom pad shapes, using Murphy's question as an example, since it includes an image of the desired pad layout.

    DS PCB does include a fair variety of common pad shapes, including rectangles, diamond, triangle, round, bullet, and others.
    One technique is to look for a combination of pad shapes that DS PCB does offer that could be overlapped with each other to achieve the desired shape.

    Looking at the upper left pad in the desired footprint, it is a rectangle with one corner cut off.
    Here is a drawing of that pad, with dimensions. In this drawing, I have overlapped a diamond shape pad and two rectangular shape pads to create create the same overall pad shape.

    The rectangle outlined in blue is 0.057" by (0.048" - 0.015"), or 0.057" by 0.033".
    The rectangle outlined in violet is (0.057" - 0.020") by 0.015", or 0.037" by 0.015".
    The diamond outlined in green is (0.020" x 2) by (0.015" x 2), or 0.040" by 0.030".

    Create and place the three overlapping DS PCB pads aligned as shown, and you have one of the four custom pad shapes needed for this particular part.

    The other three custom pad shapes are just reflections of the first one, so we can use the same built-in pad shapes to construct them, just altering the relative positions of the three built-in pads to place the cut-off corner in the correct position.

    Now arrange you 4 sets of overlapping pads to give the correct gaps between the top and bottom pair and the left and right pair.

    Now you have your desired footprint, except it is actually 12 DS PCB pads instead of 4.
    Save that PCB symbol.

    Now create a component. The component associates a schematic symbol and a PCB symbol, using a mapping table to specify which pin(s) on the PCB symbol correspond to which pins on the schematic symbol. We will take advantage of the fact that DS PCB allows us to specify that multiple PCB symbol pins should be mapped to the same schematic pin. This is done by putting the PCB pad numbers of the three pads that go to the same schematic pin on the same line of the mapping table, and separating the pad numbers with + signs to tell DS PCB that those three pads are electrically connected to each other. Here is an example mapping table row for the first custom pad:

    The next row of the table would map Sch Terminal Number 2 to PCB pads 4+5+6. The row after that terminal number 3 to pads 7+8+9, and the fourth row terminal number 4 to PCB pads 10+11+12.



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