3 Replies Latest reply on Dec 7, 2009 2:32 PM by David Ricketts

    Question on Via Symbols

    mthayer

      Hi everyone,

       

      I've been reviewing a board layout, and we've got some symbols in there that we're not sure about.  There seem to be different ways the vias are drawn, and we haven't been able to get a good answer as to what they represent and why they're different.  We've been told at one point that they're all the same, all vias, yet they're sometimes drawn with distinctly different symbols, so I don't buy it.

       

      Excuse the crude MSPaint masterpieces (bottom of the post); I hope they get their point across.

       

      1). Holes A and F... F is a through hole part, while A is a large Via... so I'm assuming that explains that difference.  Is this correct?

       

      2)  A and C... Both large vias that are drawn differently.  If C connects, it should look like A... if not, it should be an empty hole.  Once we were told that they don't mean anything, and then later we were told that the vias drawn like A and D indicate an error that there were things overlapping that shouldn't - we found those before when we had a split region in a ground plane that was accidentally overlapping an identical area beneath it.  Those problems seemed to be fixed, but after the latest changes, they're back, and we need to stop and find out for sure what's going on.

       

      3) Notice also in the C picture, the smaller connected vias on the right seem to have several different looks (the top one looks different from the lower two.. smaller?).  I believe this may just be due to them being different sizes and the way they render in the display.  Is that what's going on there?

       

      4). B and E... these appear to be half-connected to the plane, half not.  In the case of E it looks intentional, as that other via is placed butted up overlapping, but B makes me wonder what's going on there and why.  It looks like this may be because there is a dedicated AGND plane, and then above that is a plane where the center region is isolated as a sensetive ground, and the exterior region duplicates AGND - it shows the top half connect on one of those and the bottom on the other - but other vias have full connections on both planes.  It's these inconsistencies that bother me, and lead me to believe that things may be hooked up in incorrect ways that we don't understand.

       

      Anybody have any insight into what these various symbols mean, or where I can find documentation of such things?  I've been through the help file a bit, but haven't come across any symbol or via type pictures or anything that looks helpful.

       

      Thanks,

       

      Matt

       

       

      photo6.jpgphoto2.jpgphoto3.jpgphoto4.jpgphoto5.jpgphoto.jpg

        • 1. Re: Question on Via Symbols
          David Ricketts

          This is a complicated issue, and you're more than justified in questioning the results you're seeing.

           

          Let's get some terminology and background out of the way.

           

          Your question is about thermals, or more properly, thermal reliefs, for Through Hole (TH) connections. A common term for these is "wagon wheel" for obvious reasons, and each of the little legs are called spokes.

           

          Thermal reliefs can be both for TH component leads or wires (which get soldered to the hole), and vias, which are electrical connections between layers of a PCB (sometimes to a plane) and do not get soldered. (OK, there is an ongoing discussion for whether vias should have any thermal relief at all, since they don't get soldered. That's for another time.)

           

          It appears the attached pictures are positive images of the PCB or gerbers, and all black areas are copper. Is that right?

           

          1. Picture F is a perfect example of what a TH thermal relief should look like. A via's thermal relief connection should look the same.

           

          Picture A is not right. Neither is D. The thermal reliefs looks like they're intended for a negative gerber. Gerber files can be created both as positive or negative images, so the thermal looks different. There is no connection to the plane if this is a positive view.

           

          2. Picture C is correct, but different than F. Remember, A is wrong. F shows a solid pad, whereas C shows a ring. Designed correctly, the ring will work, as long as the drill is larger then the inside diameter of the ring, but I don't recommend using a ring.

           

          3.Yes.

           

          4. You are correct that the spokes are missing because they were removed when the plane is generated due to a DRC conflict. I cannot tell you why there's missing spokes for B, as there's no obvious reason.

           

           

          PADS has somewhat complicated and overlapping procedures for creating thermal reliefs, and it looks like your design has not had all of these methods consolidated.

           

          Here are the places where you and/or the designer need to look.

           

          The oldest and most basic control for thermal reliefs is the Thermals tab on the Options menu. This sets up the default for all poured planes.

          Next is the Split/Mixed Plane. It also is found as a tab of the Options menu. This feature was added later in the history of PADS, and was a paid option. This is why the controls are separate.

          The third is Pad Stack Properties on the Setup menu. Here, individual pins and vias can have special thermal reliefs assigned, which will override the defaults.

           

          The type of layer is also a consideration. There are three types:

           

          If it's No Plane, then the Thermal tab controls the thermal relief.

          If it's Split/Mixed, then the Split/Mixed Plane tab provides the settings

          If it's CAM Plane, then the layer is a dedicated plane, and the gerber created will be a negative image.

           

           

          There's a lot here to digest. I'll try to answer any more questions when I can if you have any.

           

          David

          • 2. Re: Question on Via Symbols
            mthayer

            Thanks, David.  That helped me get a feel for what was going on, and to be more confident that the problem really was fixed once we found the causes.  Turns out there still were problems with the way we had defined a split ground region, which affected the vias and thermals.

            • 3. Re: Question on Via Symbols
              David Ricketts

              You're welcome.

               

              Split planes have another level of complexity I did not address. Since there can be multiple planes per layer, they can be embedded or overlapping. You can assign priorities (0 is highest, and also the default) for the plane that is most critical, and higher numbers for the lower priority planes. This will affect which pins get assigned thermals, as a pin outside the poured area determined by these priorities will not be connected, even though it is within the correct pour outline.