Included is my 4 layer pc board design. I have installed plated through holes under a part, which will connect to the ground plane (layer three). The bottom of the holes are
I am not sure that I am doing this correctly - the DRC has many issues with my placement due to the proximity of the holes.
Should I connect all of the holes together on the bottom side with traces?
I hereby certify that I am not simply asking someone else to design a footprint for me.
This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.
Let’s call it a footprint for consistent terms while using KiCad pcb editor.
Does the footprint have a bellypad or extended pad which will be positioned over these plated thru holes?
Does the physical component have a bellypad or extended pad?
If the answer is YES then make sure that the footprint bellypad (or whatever) is connected to GND in your schematic. You would also have these PTHs connected with copper zone on your ground layer.
I am assuming that you would want your bellypad to be grounded. That is most common but is not universal. (For example a negative voltage regulator would probably have the bellypad connected to Negative Vin.)
Bob,
Thanks for the fast response.
The ‘footprint’ (through holes) does not have a bellypad itself, but the component mounted does, as it is a regulator. There is no heatsink tab on the regulator.
Sorry, I neglected to show the front copper. Here is the Front copper, showing the Ground via connected to the part. These footprints are also connected to GND net.
I have added these holes to increase the heat sinking of the pc board, as in certain situations the thermal properties may be stressed.
So I think I am okay with the footprints the way they are. Am I correct in thinking since the holes do not connect to parts on the bottom, the solder should not be sucked down by the holes? I was told this can be a problem.
Your holes are pads number 1 while the big pad has number 3.
They all should have the same pad number or you are making Net-tie and there is a way (don’t remember now) in footprint to define it as Net-tie.
See any footprint (QFP, QFN) with thermal pad with vias. I can’t specify exact name as I don’t use KiCad library and don’t see them. You will se how it is made there.
I suppose that for 32 pin footprint thermal pad will have number 33 (I use 0 for it) and all vias in it will also have number 33.
I assumed that these pads are part of footprint. Aren’t they?
These “bellypads” are called exposed pads. And also not “extended pads”.
If your heat-sink-thingies would be connected to ground, the errors (except distance) would disapear.
In your picture (part of it), you have the via to ground. And your extra vias should look exactly the same.
Press E on a selected via and check its net name.
Furthermore, I would look at the manufacturers suggestions. I assume his suggestion looks different.
Nick,
So should I just change these to vias on the GND net? I was under the impression holes provide more heat sinking.
I was told vias tend to suck the solder away from the pad, producing inadequate solder under the component heat sink. On their pc boards, they make sure no vias are actually under components for this reason.
Is this something I need to be concerned about?
a via and a hole are the same thing at the fabrication level.
The difference is that you can add a via outside of a footprint. But a hole is a pad inside a fottprint.
In your case, the main issue is that the hole added to you footprint MUST have the same pad number than the SMD pad that they are on.
So pin number 3 for all of them in your picture
Actually some vias can be supplied “plugged” so they do not suck solder.
I think that if the mounted component has an exposed pad that the footprint should also. If you have something like an SOIC with exposed pad, then the grounded top side pad can extend beyond the ends of the package, so that you can solder with (probably a wide screwdriver soldering tip). It is important to apply flux to the exposed pad before mounting the IC to the board.
Is this board design for mass production or you plan to hand-assemble a few?
Another option: One thing I and others have done is to put an appropriate through hole under the exposed pad and solder from the bottom with the tip of a very hot (400 degree C) soldering iron.
Whether or not a via (or pad) starves the SMD pad of solder during assembly depends on where the hole is relative to the SMD pad and the solder mask. You should also include the solder mask in your image. That way you can see if the position of the holes will draw solder away from the SMD pad.
As Bob mentioned, you can also order your PCB with “Epoxy Filled Vias” (or even “Copper Filled Vias”) but it adds to the cost of the PCB. These types of vias can be used for “via in pad”. That is, they are intended to be used under SMD pads. I think in your case that would likely not be required. You just want a heat sink so position the vias outside of the solder mask and you should be fine.
Here is an example of what I am talking about. The first image shows the front copper layer and the position of the thermal/power vias close to the SMD pad. The second image shows the solder mask. The position of the vias is outside the solder mask so they will not starve the SMD pad.
