PCB Solder Mask and Silkscreen

When you design and order printed circuit boards, you need to decide whether to pay extra for soldermask and silkscreen. What is the purpose of these layers and what do they look like?

After reading this article, I hope you’ll appreciate the benefits of having solder masks and silkscreen on your PCBs, even for prototypes.

Plain Copper

Let’s start with an ordinary bare-bones circuit board. Select the top copper layer and draw text, pads, and traces.

Some instructions in this article are related to the Copper Connection software. However, the board information and images are relevant regardless of the PCB layout software you use.

To see the examples in this article, click on the file and save it.
Download Copper Connection, the PCB layout software.
Free to display, edit, and etch at home.

Choose top copper layer Tools to draw elements Trace pad and text elements on top copper layer

Instructions for example software. Left: Choose top copper layer. Middle: Tools to draw elements. Right: Trace, pad, and text elements drawn on top copper layer

If you etch the board at home, the elements will have a similar look to the image below. Notice the text, pads, and traces are all made out of the same material (copper). They all have a reddish brown metallic color.

Printed circuit board copper only etched at home

Printed circuit board copper-only etched at home (poorly, I admit)

Clean copper solders acceptably, but over time the copper oxides. In that case, you will need to scrub or chemically treat the oxidized copper pads before soldering, or else the solder will not stick reliably.

Tin Plating

When you order a professionally-manufactured circuit board, they plate the copper with a mix of tin, lead, silver, and/or other metal. This coating is easier to solder and slows the rate of oxidation. The image below shows copper text, traces, and pads plated with a lead-free finish. Notice that the metal is whiter than plain copper.

Printed circuit board with lead free plating

Printed circuit board with lead-free plating

Tin-plated boards without solder masks or silkscreen are the least expensive. They are acceptable if you want to save money. You don’t need to do anything in your PCB layout software to enable tin coating, as it is simply a basic step in manufacturing.


Unfortunately, when part outlines and text are drawn on the copper layer, they are electrically conductive. You can’t put traces or parts in the same places, as the copper text would interfere and change the circuit.

In your layout program, you can place text and part outlines on the silkscreen layer instead of copper. For example, in Copper Connection simply choose the silkscreen layer before placing text, or select the existing text and switch the layer to silkscreen.

Choose Top Silkscreen Text moved to silkscreen layer

Left: Choose Top Silkscreen. Right: Text on silkscreen layer

Copper Connection includes a bulk selection feature for your convenience. If you have already made a board with text on a copper layer, you don’t have to move each text element one at a time. Instead, right click on any copper-layer text, choose “Select All Text on this Layer”, and then choose the new layer (top or bottom silkscreen).

Quickly move text to the silkscreen layer by choosing Select All Text on this layer

Quickly move text to the silkscreen layer by choosing Select All Text on this Layer

Now, when you order the boards from your favorite manufacturer, be sure to choose one of their manufacturing options that includes silkscreen. For prototype runs, silkscreen is usually restricted to the top side of the board, but some manufacturers offer both sides.

In the photo below, see how text and part outlines are now a different color than the traces and pads. The silkscreen layer is just ink. The ink is non-conductive and can be placed on top of traces without interference.

Printed circuit board with tin plating solder mask and silkscreen

Printed circuit board with tin plating solder mask and silkscreen

Besides making better use of board space, the silkscreen layer is brighter, providing better contrast for faster hand assembly. Part outlines indicate part orientation, and make it obvious when you’ve forgotten to insert a part. Below is an example of different silkscreen appearances of a part outline, as produced by various manufacturers.

Silkscreen of diode Advanced Circuits shown at top

Silkscreen of diodes

Solder Mask

When you order silkscreen, you almost always get solder mask on both sides as well. Solder mask (or soldermask) is a coating that protects the circuit from corrosion and electrical shorts. It also provides electrical insulation that allows higher voltage traces to be placed nearer to each other.

Most importantly, the solder mask keeps the solder on the pads, as opposed to flowing onto traces, planes, or empty board space. This reduces the likelihood that solder will form bridges (unintended connections) from one element to another. Solder masks are critical for wave soldering, which is a mass production technique. But, solder masks also make hand soldering faster, easier, and more accurate.

In the photo below, the green coating is the solder mask. See how the solder mask coats the entire board except for the pads. The pads are exposed to allow you to solder parts to them.

Solder mask and solder mask swell

Solder mask and solder mask swell

Usually, you don’t need to do anything in your PCB software to enable the solder mask. The software automatically makes holes in the mask that correspond to pads. Additionally, the Copper Connection application grows those holes slightly by default, so that moderate manufacturing misalignment (registration error) won’t overlap the pads.

Solder mask swell amount in Export window

Solder mask swell amount in Export window

Customizing the Solder Mask

In most cases, you won’t edit or alter the solder mask. In fact, you usually won’t even see it in the layout software. If you want to, in Copper Connection you can view the solder mask by choosing Layer Colors and Visibility in the View menu and checking the box next to the desired solder mask layer. (Make sure Show Pours and Show Automatic Pours are checked in the View menu.)

Check one or both solder mask layers to view the solder mask

Check one or both solder mask layers to view the solder mask

Look at that! You can see the green mask coating everything but the pads.

Viewing the solder mask in a PCB layout program

Viewing the solder mask in a PCB layout program

Just for fun, try placing a rectangle or ellipse on the top copper layer. Notice that it is covered by soldermask.

What if you want that rectangle or ellipse to be an electrical contact point, to be solderable, or to connect to a heat sink? The correct way is to create a rectangular or circular pad in the desired size, as pads are intended to be exposed.

Creating circle and rectangle pads without holes

Alternatively, you can use a normal shape on the copper layer, and then add a keep-out area to the solder mask.

  1. Choose a shape tool (ellipse, rectangle, or polygon)
  2. Choose the desired solder mask layer (it must already be visible -- see earlier)
  3. Choose Keep Out Fill (because we want the solder mask to keep out of this area)
  4. Draw the shape.
Choose fillable shape tool Choose solder mask layer Choose Keep Out Fill

Steps to expose a portion of the solder mask

This technique is useful for making button contact, such as for a keypad. Draw the contact fingers with traces, and then cut out a space in the solder mask so that the metal on the traces is exposed (not covered by solder mask).

Button contact made with traces is exposed through solder mask

Button contact made with traces is exposed through solder mask

The opposite is also possible. If you want to cover some or all of an exposed pad, such as a via, you can draw an element on the solder mask layer with Fill instead of Keep Out Fill. You’ll also want to right click on the fill shape and change the Pour Clearance to “None (connect to pour)”.

Partial Solder Mask

Occasionally, you need the solder mask to cover a portion of a pad, rather than exposing the entire pad. An example of this is where there is a pad underneath a chip (usually for cooling purposes) which is near enough the other pins that leaving it completely exposed could result in accidental solder bridges.

Start by designing the chip as though it had a smaller inner pad that is only the size of the exposed area. The picture below shows New Land Patten window (in the pulldown menu to the right of the Part tool) with values entered from the Texas Instruments DDA (R-PDSO-G8) PowerPad Plastic Small Outline data sheet. The data sheet calls for a total center pad of 2.94 mm by 4.89 mm, but you only want to enter the smaller exposed size of 2.49 mm by 3 mm.

Designing chip using land pattern window and datasheet

Designing chip using land pattern window and datasheet

Click the OK button to accept the design and then click on the board to place the part.

Switch to the rectangle tool and choose the Top Copper Layer and Fill from the Shape section of the ribbon. Roughly draw the rectangle near the PowerPad part, and then adjust it to the exact size of 2.94 mm by 4.89 mm by typing those values into the Width and Height of the Size and Position section of the ribbon.

Adding covered rectangle to center pad

Adding covered rectangle to center pad

Select both the part and the rectangle, and choose Align Center and then Align Middle from the Arrange menu. This places the rectangle at the same location as the pad in the middle of the part. Don't worry about whether the rectangle is above or below the part's center pad, because a pad always has priority over a rectangle. The pad will cut through the solder mask and will accept trace connections even when a rectangle is 'on top' of it.

Officially, the TI part includes a group of six tiny vias in the center. The vias provide additional heat transfer to other layers. I've created a version with and without the vias for demonstration purposes.

Below is the view with the Top Solder Mask showing (View->Layer Colors and Visibility: check Top Solder Mask), all pours shown (View->Pours->All), and the part located on the board. Notice that the part has all of the pins and the center pad exposed, but the larger copper section in the center is protected by solder mask.

PowerPad solder mask

PowerPad solder mask

The part with the vias has some additional solder mark exposed around the edges, but is likely still acceptable. However, be warned, solder mask is swelled (made larger) to compensate for misalignment during manufacturing. All of your hard work may be eliminated if the mask is swelled enough that it again touches the outer pins. If that occurs, you could make the center pad even smaller.

Enable x-ray vision (View->X-Ray Vision->All) to see the larger copper rectangle surrounding the pad.

PowerPad solder mask x ray

PowerPad solder mask with x-ray

Combining a plain copper shape (circle, arc, line, rectangle, or polygon) with a pad is a good way to create a virtual pad that is only partially exposed through the solder mask.

Tented Vias

A via is a hole that connects one layer to another, but isn’t intended to have any parts inserted into it. Usually, you’ll want the vias to be exposed so that you can test the board, or so that you have an optional place to insert a wire or hole if you made a mistake on the board. This is the default setting.

If you’re really sure that your board is perfect, and the manufacturing/soldering method permits tented vias, then you can have the solder mask and silkscreen cover all the vias. This protects them against corrosion and accidental electrical shorts, as well as provides a little more surface area for text and part outlines.

In Copper Connection, you can select Tented Vias in Board Properties in the File menu. Note that this window controls other layers as well, such as silkscreen and solder mask.

Board Properties controls silkscreen solder mask and tented vias

Board Properties controls silkscreen solder mask and tented vias

After clicking okay, the results are reflected on the screen. If you choose tented vias, you can still manually edit the solder mask and adjust the position of text to expose specific vias, if desired.

Prototype Choice

When I first began making printed circuit boards, I chose 2 layer boards without solder mask or silkscreen, due to the lower cost. This forced me to place part labels on the copper layer, or to forgo labels where there wasn’t enough room.

As my collection of boards grew, I recognized this was a false savings. It takes a lot of time to figure out where parts go on boards that lack sufficient labeling, particularly if the board was designed a while ago. Lack of labels may result in a part being soldered in the wrong location or forgotten about completely.

A lack of solder mask isn’t as much of an issue, yet a solder mask can reduce soldering time by guiding solder to the pads. (In any case, I haven’t run across a manufacturer that offers silkscreen without solder mask.)

Therefore, in recent years, I exclusively order boards with solder mask and silkscreen.