Plated Slots: Stop Fitting Square Pegs in Round Holes

Most through hole components in PCBs have circular or square leads which fit nicely in circular holes, but what happens when you have a component that have non circular or square pads? For example, let’s take a look at the 2.1 mm DC jack made by Switchcraft (Part Number: RAPC722X).

This part has three leads each of which are rectangular in shape. Here is a snapshot from the datasheet of the DC jack dimensions:

Figure 1: DC jack dimensions

The three leads on this device are thin and wide rectangular shapes that can be soldered into a circular hole but this is not the most ideal solution. Let’s take a look why.
Here is a picture of the recommended footprint for using circular through hole pads from the datasheet.

Figure 2: Through hole footprint

If we take that information and make a footprint in our EDA tool we can get a better idea of how it will look.

Figure 3: DC jack EDA footprint

In general, this footprint appears to be acceptable, but check out what happens when we superimpose the outline of the DC jacks lead size in the circular pads that we just created.

Figure 4: Pins in holes

Since the hole in the pad needs to have a diameter wide enough for the pin to fit through we are left with a lot of open space from the pin to the to the copper on the edge of the hole. In the next image the open space is highlighted blue to demonstrate this.

Figure 5: Open Space to be soldered

The reason this method is non-ideal has to do with the soldering process. The open space shown in the image above will have to be filled with solder when building the board. Since this open space is significant, a lot of solder will be required to bridge the gap.

Electrically there are no issues with this style of component mounting, but consider the case if you wanted to mount other components that had wider leads. At some point the hole would be too large to fill with solder becoming non practical. Mounting pins such as the ones on the DC jack in circular holes works well, but we need a better method for mounting larger and odd shape pins. Using large circular holes are not well suited for layouts requiring tight size constraints or dense component population.

Luckily, we have the capability to manufacture plated through hole pads that are non-circular in shape and can accept pins such as the ones on the DC jack with much less open space to solder. Let’s take a look at how to do this.

To create a plated through hole we have to define a few things in our EDA tools. For most EDA tools, plated through holes are created through a manual process where the designer specifies all the aspects of the hole as opposed to simply placing a standard pad. There are three things to consider when creating a plated through hole: the shape of the copper on the top layer, the shape of the copper on the bottom layer, and the shape of the hole.
The following is a rendering of a PCB with a plated through hole which give an idea of the items that need to be defined in the design tools.

Figure 6: Plated through hole rendering

And here is a cross section cut of the same pad:

Figure 7: PCB Cross Section

To create a plated through hole such as this we start by placing a pad on both the top and bottom layers to create the top and bottom copper. These pads can actually be SMD rectangular style pads or they can simply be shapes drawn directly on the top and bottom copper layers. It is critical that both the top and bottom pads are larger than the hole. It is not necessary for both the top and bottom pads to be identical, but in most situations they will be.

Here is a footprint of the DC jack from earlier with SMD rectangular pads on both top and bottom layers.

Figure 8: Footprint with SMD pad

The bottom pads are not visible in this image because they were created to be identical in size and shape to the top. Now that the pads have been defined, we need to add the holes.

Plated through holes differ from most other holes in PCB design as they are not included in the standard drill file, instead they are drawn on the board outline layer. When manufacturing files are sent to a PCB manufacturer, the board outline is interpreted as cutting information. If a shape exists on the board outline layer, the PCB manufacturer will route the board inside the shape that has been drawn. If a hole is drawn inside pads that are on the top and bottom of a PCB, the board manufacturer will interpret this as a plated through hole.

Knowing this, we need to draw the holes we wish to have in our footprint on the board outline layer. In the following image I have shown the footprint from above with the cutouts shown as purple slots. The pads are not shown for clarity.

Figure 9: Board Outline Slots (pads not shown for clarity)

That’s all it takes to make a plated through hole. When generating the manufacturing files, the pads will exist on the top and bottom layers and the slot will appear on the board outline file.
Here is a picture of a board that was recently manufactured with this footprint.

Figure 10: PCB with Plated through holes

To recap, making plated through holes is as simple as creating pads on the top and bottom layer and defining a hole on the board outline layer. Plated holes allow designers to use parts with non-circular leads and pins while maintaining good electrical and mechanical connections. With a little creativity, even components such as panel mount potentiometers can be mounted to a PCB using plated holes.

Ready to get started?

Sign up today


  • Mikey McLaughlin says:

    Excellent explanation for how to implement this, I was fussing with an off center PTH and adding a mill slot. However, on this point, would a milling operation be interpreted a post operation to follow plating/pouring? (i.e. such that the board would already have copper applied and PTH can no longer be added when the milling layer is called for)

    • Parker Dillmann says:

      Depends. If it is a plated slot then it is milled before hand then plated when the vias are done.

      • Mikey McLaughlin says:

        In Eagle, there is a separate milling and dimension layer. The geometry from the milling layer typically is only shown in the outline Gerber. While for creating the physical outline of the board it is a milling operation either way, but it seems that in order to capture a slot on the edge of the board, it should be included in the dimension layer in the aforementioned stack up so that dimension is added to each individual Gerber file and not just the outline Gerber .

        • Parker Dillmann says:

          Correct. I always put the cutouts and slots in the border gerber file. In Eagle I typically draw it in the dimension layer 20.

          • Mikey McLaughlin says:

            Can you add minimum slot widths to the capabilities pages? I’m making up a component library for components to be placed in-plane with the pcb and essentially just need the minimum milling bit size for both dimension and milling layers.

          • Parker Dillmann says:

            Hi Mikey I sure can. Should be up soon.

          • Parker Dillmann says:

            Minimal width of 1mm for slot width for both internal or external slots.

Leave a Reply

Your email address will not be published. Required fields are marked *