Stats

  • Replies 9
  • Subscribers 162
  • Views 16100
  • Members are here 0
More Content

Strange Dot on final Footprint ?

Cailloux

Picture 1 show a Shape created in Allegro PCB Editor 16.6, file LTshape.ssm      The Shape Origin is dead center of the outline 565X400 mils.    This Shape is utilized in the PadStack Editor to create a special Pin for a custom Footprint.
Picture 2 show the PadStack Editor first page with drill size and offset. File  LTshape16.pad         Picture 3 show the PadStack Editor page 2 with that LTshape utilized as the BEGIN LAYER for copper area. Picture 4 show the actual Package (footprint) finished with Outline, padstacks for pin 1,2,4,5 and that special Pin 3 LTshape. Its origin is also dead center, same as LTshape.ssm

Notice the round dot at the bottom of Pin 3. It only appear in the Package drawing, not in the original Picture 1, the actual LTshape.ssm or LTshape.dra

Picture 5 shows that same Footprint in the final board in PCB Editor. That same dot, now pink, is still there and cannot be selected separately. When using the Find Option and selecting each object separately, the only way to select Pin 3 is when Option > Pin is selected. Then I can hover on the dot near Pin 3 and the whole LTshape lights up as pin 3, but not the pink dot. There is absolutely no way I can select that dot as an object. There is no way to know the existence of that dot except by looking at it. Cannot be deleted, cannot be selected, can only be invisible if I use the Color Visibility manager and disable all 4 layers, TOP GND VCC BOTTOM. If I turn On TOP then the dot becomes pink. With GND On the dot is green, VCC On will get a Red dot, BOTTOM On will not show the dot but Pin 3 turn On since LTshape is the actual Net connected. This Net is not GND nor VCC, it is N357726.

Where is this dot coming from and why is it not a selectable object ? Why can I not delete it ?

   

  

Parents

  • So this will be the pad that you defined on the Bottom / Default Internal layers. The drill array you define is only for the drill holes. You can't define a pad for the drill holes like this. If you want to do something like this then the pad must be the same on all layers or you will just see drill holes with no pads on inner and the bottom layers. The better way to define this is place the SMD pin in the footprint then use Layout - Connections and double click to add a via. You can then copy this via to the locations you want. If you want to setup wish via you look at go to Constraint Manager - Physical and define the via there for the DEFAULT rule as you would in any board. 

  • in reply to steve

    Spot On Steve ! I changed the Pad Geometry for both INNER and BOTTOM and found that it is the BOTTOM part of the Pad that shows as that dot. 

    As for your instructions on How to do this properly, I not sure at which level I should do that. When you say "place the SMD pin in the footprint then use Layout > Connections..." , do you mean when I am editing the Package in PCB Editor or when I am in my final Board editing the PCB  ? 

  • in reply to Cailloux

    Sorry modify the pad and remove the drill holes and make this just a surface mount layer, then open the package symbol (filename.dra) update the pin so it's just a smd pin and add the vias there. 

Reply Children
  • in reply to steve

    Great ! Thats what I thought. But now I am in PCB Editor trying to build a brand new Package. First thing I did was to put my special Pad LTshape as a SM pad. Now that my LTshape SM pad is placed on my Design window I am trying to Layout > Connection and I can see in the Option window that no Via is defined by default. If I want to chosse one, nothing is available. If I go the Constraint Manager and try to edit the default VIA there is one and I can even change it for another VIA. Still the Option window will not let me choose what Via to use. So the question now is: How do I define a default Via that I can use when in PCB Editor Package mode?  I kind of lokked pretty much anywhere I can think but that seems like a dead end. Any suggestions ? Can we actually put Vias when in Package mode?

  • in reply to Cailloux

    Yes, you can add vias to *.dra files.  Try Layout->Connection then click once on the location you want the via to start routing (your default via should now show in your option tab), then right-click "Add Via".

  • in reply to Cailloux

    The Options pane won't show the VIA until you left click to start the Connection. By default it uses the one at the top of the vialist but you can select others if you have more than one in the vialist.

  • in reply to steve

    Yes it works !  Far from being an intuitive UI but alas I got it. Thanks guys, much appreciation.

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.