Announcement

Collapse
No announcement yet.

How to avoid top-bottom GND via in Internal GND plane

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • How to avoid top-bottom GND via in Internal GND plane

    I have a regulator that dissipates much heat and It need to have a heat sink pad in PCB. I have placed a pool of Ground vias in the Heat sink pad area. The board is 4 layer with top and bottom signal/Gnd layer and middle layer GND and PWR. I want the dissipated heat to get sink into either top Layer or bottom layer pad and avoid the internal GND and Power layers to get connected to these heat sink vias so that the internal layer can avoid the regulator heat.

    Problem:
    The ground vias from Top to bottom layer get connected to the internal GND layer. Is there any way to avoid the Internal GND layer?

    I checked the Middle layer Thermal Relief of these Vias to No Connect but still they are connected to Internal GND Layer.

    If there is any way to achieve this then someone please guide me.

    Thanks.

  • #2
    Question is Why? Your regulator should never get so hot that the heat going into inner layers should somehow influence or damage the PCB. Actually I very often use inner GND planes to take heat away from some components. I know it heats up the whole PCB, but regular products should be able to work in ambient temperature 65-85C degrees and regular components are rated around 100Deg, that should not be problem pro PCB.

    If I would really need to isolate the GND VIAs from GND plane

    - I would simply create a region with no copper around the VIAs (Place polygon pour cutout)
    - or if it is on power plane, just draw a circle around the via
    - or if it is polygon, you can set specific connection type on specific layer


    Click image for larger version  Name:	void around VIA on power plane altium.png Views:	0 Size:	155.1 KB ID:	12625



    Click image for larger version  Name:	connction type on L4 altium.png Views:	0 Size:	76.2 KB ID:	12626


    Click image for larger version

Name:	no connection GND.png
Views:	151
Size:	93.3 KB
ID:	12627

    Comment


    • #3
      Actually, I want to contain dissipated heat in a specific heat sink area so that the regulator heat does not change overall PCB temperature. The internal layers can not dissipate heat as effectively as the outer layers and it will also conduct heat to all corners of PCB. Therefore, I was avoiding internal layers. I will try the solutions you provided. Thanks Robert Sir.Click image for larger version

Name:	Img1.png
Views:	155
Size:	89.7 KB
ID:	12630Click image for larger version

Name:	Img2.png
Views:	162
Size:	119.0 KB
ID:	12629

      Comment


      • #4
        technically you are creating a few very large ground loops. i would not recommend this.. it depends on lot of things but if your potential is GND on that heatsink and you manually override the connection on the inner layer. then your whole ground connection is done through this area, this will cause more trouble than the heat would.
        Click image for larger version

Name:	2019-12-10 14_08_55-Window.png
Views:	138
Size:	88.1 KB
ID:	12648
        Attached Files

        Comment


        • #5
          Ok, I am reconsidering it as both Robert and you suggested to avoid it. Thanks

          Comment

          Working...
          X