Skip to main content

Pads and vias are essentially the same, a hole surrounded by copper, however, the distinctions is how and where they are used.

Pads generally have a large hole to accommodate a wire or pin and are "all layer", i.e. the hole passes through all layers.

Vias have a small hole and copper land and are generally used for connecting tracks or copper between layers. DSPCB Engineer subscription allows the production of blind and buried vias where the distinction is even more important.

DSPCB and Engineer subscription both have a similar "Add Pad" icon ( and shortcut F4) on the toolbar to allow you to add a pad with a "Style" directly to your PCB design.

Similarly both DSPCB and Engineer subscription offer from the Menu Bar under "Add" the ability to select from the many options to add a Via.

DSPCB menu

Here we show what happens if we add a pad of style "small via" and a Via of style "small via".

pcb Pad and Via

The first obvious difference is the colours (using the default settings), but from mouse-over text, the pad is not associated with a net whereas the via is associated with the next available net, in this case, N0000. We will cover the relevance of this in a moment.

Firstly let us look at the Design Technology - "LayerTypes" tab.

"All Layer Pads" and "Vias" have separate control over the solder mask layer which provides an easy way of controlling the covering of vias with solder resist.

pcb Pad and Via

This example illustrates Pads on the left which are of style "Small Via" and on the right Vias of style "Small Via". The vias are covered with solder mask as can be seen by the absence of openings in the solder mask layer.

The top part of the image is the Top Copper and Solder Mask layers, the lower is the Solder Mask layer only showing they follow the setting from the Design Technology.

pcb Pad and Via

 

Vias are often used to provide additional screening by connecting copper on different layers together and also to increase the current capacity by the paralleling of copper tracks which also require regularly placed vias to balance the current sharing.

Both are commonly referred to as stitching.

DesignSpark PCB with an Engineer subscription has advanced features related to this as detailed in the Users Guide, however, manual placement of vias can also be used as detailed below.

To illustrate stitching with vias for a copper pour area we place multiple vias as required. Each will have its own net assigned on placing, in this case, N0005 to N0015.

Note. You will normally have the copper pour area defined before placing the stitching vias, but for clarity, we show the via placement first.

pcb Pad and Via

These now need to be assigned to the same net that will be used for the copper pour.

Select all the vias using a selection window or my multiple selections (CTRL+Left Mouse Click) and then right-click and select Properties - "Net" tab, chose the required net (in this case Gnd) and click <Apply>. A message will appear regarding joining multiple nets, but as this is what you require select <OK>.

pcb Pad and Via

You will now have the net rubber band indicating all the vias are placed on the same net.

pcb Pad and Via

To illustrate the difference between Vias and Pads. Place a Pad of Style "Small Via" and right-click and select "Add To Net" as pads are not assigned to a net when placing. Add the pad to the "Gnd" net.

pcb Pad and Via

Using Copy (CTRL+C) and paste (CTRL+V) place a row of pads. For each placement, you will need to confirm that you wish to merge with the existing net and this will be confirmed by the net rubber band.

Note. You can also select and copy multiple pads to speed up this process.

pcb Pad and Via

Using the above example of vias and pads (some of which are assigned to the Gnd net) we now produce a copper poured area with a flood fill.

pcb Pad and Via

With the above Design Technology settings, we have the solder resist covering the vias but not the pads. The pads not assigned to a net will have a thermal barrier and remain isolated from the copper pour as will any vias that are not assigned to the Gnd layer.

For DesignSpark PCB with an Engineer subscription, the distinction between a Pad and a Via is even more important as the via can be used where blind and buried vias are required.

For DSPCB both pads and vias can be used to achieve the same result, but it is important to understand their difference regarding the assignment of a net. It can also simplify the requirements of where a solder mask is applied.

Technical Support for DesignSpark PCB
DesignSpark Electrical Logolinkedin