Actions
Forum Thread Details
  • State Suggested Answer
  • Locked Locked
  • Replies 6 replies
  • Answers 4 answers
  • Subscribers 84 subscribers
  • Views 2003 views
  • Users 0 members are here
Related
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Making irregular fill shapes and assigning nets

stuartrumley

I come from OrCAD layout where I can make copper fill or copper area in any arbitrary geometry. That copper area or fill can be assigned a net connection to a specific pin or net.

 

It looks like that can only be done in CS by assembling a number of "pieces" to form an irregular geometry.

For example, I would like to make a copper ground pad for this LLGA-9 package like this:

image

In order to make that irregular ground pad shape I pieced together a number of regular rectangle shapes like these:

image

Is that how irregular fill shapes are made in CS? 

If that is the case, how do these or any final shape get assigned a net connection?  To I have to subsequently go back an edit each piece of the shape to attach a net name?

Thank you,

Stuart

Parents
  • 0

    It's similar to Orcad although probably not in the same order (as I recall).

     

    Click the Polygon Pour tool.

    Make your selections of name, pour style, associated net, locked, poured or not, etc.

    Your cursor turns into a large vertical cross.

    Draw your polygon with as many vertices as you desire.

    When you close the polygon and escape out of the command, it will be poured with the style you chose.

     

    There is also a tab in the dialog box for entering actual vertex coordinates.

    This can be handy if, for instance, you were laying out a PCB antenna from a specific design or, if you were

    entering the shape from a spreadsheet with IPC rules, etc.

  • 0 in reply to nhee

    Yes, this can be done using the polygon pour.  That would be done on the PCB level.

     

    To make an irregular shape on the footprint I suggest searching for "Altium Designer custom footprint" and read a number of related threads.

     

    Summary wise:

    1) You can combine pads by overlapping them and give them the same pad number to match the schematic symbol pin.  When a net is connected to the pin all the pads will pick up the net name.

    2) You can draw a custom shaped polygon on the copper layer and corresponding shapes on the paste and/or solder mask layers.  If these overlay with a pad then the copper will connect to the pad net.

  • 0 in reply to tarribred61

    Good points regarding an arbitraty footprint shape.  #2 makes it a piece of cake.

     

    And regardless of method, it's always a good idea to examine your Gerber outputs to see if you're getting what you hoped for.

Reply Children
  • 0 in reply to nhee

    There is a benefit to using #1 method.  If you combine overlapping pads then they will be subject to the mask expansion rules.  If you use arbitrary shapes then they do not change with rule changes.  For some footprints it might not matter much.  For others that are more generic, such as some four pin voltage regulator devices, then having the rules helps reuse of the footprint.

     

    For the LGA shapes above, the center pad shape may be using windowed paste mask anyway so paste mask expansion rule isn't so important.  I would probably draw as shapes on the various layers to get that.