Skip to main content

Creating Thermal Relief Vias



  • Boss .

    Yes that's exactly the application of thermal spokes to provide a thermal break between the pad/via to enable soldering.

    You said...  "The pogo pin pads aren't power connections so they didn't automatically get thermal relief spokes when I sent off the data for manufacture, so is there a way to do this manually??"

    Pads and vias should get the thermal break automatically unless you used the 'override settings and selected "flood". Right-click on the copper pour boundary and look at Properties - Area and you will see what settings you used.
    One other thought, did you perform the copper pour function last?
    If you add the pad or via after the copper was poured you will in effect just be making a hole in the copper. You need to clear the copper pour and re-pour to generate the thermal relief.

  • Aaron

    I actually didn't use the copper pour function at all when creating the board. 

    I looked at some basic pro's and con's for doing it and just figured I didn't need it. 

    I assumed this is why I can't find any settings to change anything, if i don't manually copper pour has the software done this automatically when I've outputted the gerber data to get the PCB manufactured?

    Here's what the pins look like on the board currently, I've highlighted the VCC power plane.

  • Boss .

    The settings are in the Design Technology in the "Rules" tab.

    However, you do not have any thermal spokes to the via just a single track, so you have the best situation for thermal isolation from the copper power plane. Adding thermal spokes will increase the heat transfer.

    I just noticed you said a 4 layer board.
    Enable the viewing of each layer one at a time to see if there is another heat sink for the via. Goto View - Powerplane - show to see these layers.

    What layer is your image from?


  • Aaron

    The pads for the pogo pins are on the top side of the board, so top copper layer, then there's the GND layer, VCC layer and then bottom copper layer. The image is showing the top copper layer, but I've gone into the show power plane section and shown the VCC layer (so layer 3)

    I'm just finding soldering these pins, plus anything with a GND connection an absolute pain because I can't get enough heat into the board to melt the solder. 

    I've had to resort to a surface mount rework (hot air) device to actually get the solder to flow on these connections, and the pogo pin areas have the same issue.

  • Boss .

    Hi Aaron, so the questions remaining:

    Do the GND plane or VCC plane show a thermal break around these pins i.e. a gap around the pad as you see in the top copper image?
    If the gap is present, how wide are the spokes? These can be reduced in width to reduce heat transfer to the power plane. If there is no gap then choose other settings in the "Rules" next time to get the required spacing and spokes.

    The obvious next question, is your soldering iron up to the task? If it has a low wattage or small tip for SMD's it may just cool too much when applied to the pin.
    Is there temperature control and is this set high enough for the solder used?

    Are you holding the pogo pins in position? A crocodile clip is a perfect heat shunt to remove heat and cool the soldering iron tip before the solder has flowed, as also are pliers.

    I also apply flux (from a flux pen CW8400 | Chemtronics 9g Lead Free Solder Flux Pen | RS Components ( ) in many cases as when the solder melts it flows better and faster.

  • Aaron

    No the pad only appears on the top copper layer, it doesn't appear as a connection on any other layer. 

    Spec for the pad is 2mm with a hole size of 1.2mm, when I show the power plane again (like in the image earlier) you'll see there are no spokes on the pad, the ones you see in the image are to connect the two pads together and then another running off to an IC.

    In the rules section I hadn't modified anything in here so it's still showing as default (see below)

    Iron wise it's an 80w brand new unit and the board was heavily fluxed, it's not an issue of flux it's getting heat into the board, because the inner layer heats up (assuming GND plane) when you're working on either the pogo pins or any connection to do with the ground. 

    Only way around this I've found is using a hot air rework station to preheat the board, that's why i thought it was something to do with the way I've structured the layers, or whether i can modify the pads in future to be thermally 'better'! 

  • Boss .

    Sorry, I'm still confused.

    If the board is heating up internally there must (I believe) be a connection for the heat to spread.
    However, you say there are no sign of spokes.

    I just placed two components on a board with one track and one pad using the default Rules and see the following

    The bottom shows the ground plane and the thermal break plus spokes as expected.
    If you just see the thermal break between the via and the ground plane that would suggest you have not assigned the ground plane to a net.

    However although wrong as not electrically connected, it would extract the minimum of heat from the via.
    With a correct via and thermal spokes as shown in the first image that would cause some heating but should not be excessive.
    If you check again just the ground plane post a screen capture to confirm what you have.

    If yours looks correct I can only think your soldering iron is faulty and running at a low temperature which means the board heats up due to the time the tip is applied and doesn't reach a temperature high enough to melt the solder.

    Other than the above I suggest you submit your design files to support for comment.







  • Aaron

    It's not a via, it's a physical drill hole in the board (a through hole pin is passing through it), and there's a pad I placed on top of that hole to allow me to solder the pin as it protrudes through the top of the PCB.

    Maybe that's the difference. The ground connections for the IC's have thermal spokes (4 of them), but these drill holes with a pad on top do not.

    See below for the image when viewing the GND plane (i changed the colour to green as it was black, to show context)


  • Boss .

    In DSPCB pads and vias are only distinguished by their size.

    You will only get spokes on the power plane if there is copper around the hole, as when adding a pad which are "all layers pads" by default and of the same size.

    A hole is a pad without a copper pad, so based on this I added a hole and then a pad on the top layer only over the hole. I think this is what you are describing?
    A potential problem with this is that an inner layer such as a power plane that has a hole but no copper surrounding it will probably fail in plating so may not be through-hole plated. Leaving that aside I still do not see what you observe.

    My test PCB gives the following:

    On the power plane I get a hole without a copper pad (not as you see).

    So even after this investigation, I see no PCB reason for this being difficult to solder as all results do not end up with spokes but a complete thermal break which should be easier to solder but will have no connection to the power plane.

    Your image shows copper tracks, as well as the pad so, is this the view with two layers top copper and the power plane? If the green is the power plane the gap indicates it has a pad on that layer, not just a hole.

    None of this indicates why you are having soldering issues and indicates a soldering issue as previously described, tip not hot enough, soldering iron fault, holding of the pin acting as a heat shunt.

    If you want to investigate the PCB itself further examine the Gerber files in a viewer to check precisely what you had manufactured.




  • kdahlmann

    Just saw this - the best way is to keep a lock at the gerber files exported. Try to find the position and check if there are connections and how made. To avoid situations like this it is important to have only connections on one plane. If you need to connect the planes together, it is better to use separate vias (with no thermal connections, use flooded). I had this effect in multilayers when connected to GND on inner plane and additionally on the bottom layer to an additional copper pour. Even with thermal connections, the more copper areas connected on different planes, the more the problem with neccessary heat comes up.

    You may try to reduce the thermal wire track size or the amount of connections, too. Default is 4 but you could also change to 3,2 or 1. More temperature during soldering will also help.


Please sign in to leave a comment.