Using Spark Gaps as ESD Protection for Microcontroller Inputs

admin

[size=+1]
An excellent way that I have found to protect inputs to electronics components from the very high voltages of ESD and EMI spikes is to use spark gaps. These can be built into your circuit board as a part of the PC board etch. The gaps should be designed as shown in the following dimension drawing.


As shown above the two spark gap pads are half circles with a radius of 0.025 inches. The designed gap spacing should be 0.004 inches. If you use care in the manufacturing process so that the board's final etched gap dimension is less than 0.005 to 0.006 inches then you can expect to have an air gap that can clamp ESD spikes to less than 200 volts. The gap area MUST be open to the air and NOT covered with solder mask.

The spark gap can be a very effective protection measure, particularly if used in conjunction with other filtering components. The schematic snippett below shows how the spark gaps can be drawn directly onto the schematic as an actual "component".


Make special note that the return or "grounded" side of the spark gap must be returned to chassis ground and the use of connector types with 360 degree shielding is highly beneficial. The connector shield should also be connected to the chassis ground.

The picture below shows the image of the spark gap "component" placed on a circuit board as viewed from a PC board layout package. Note in this picture that the return side of the spark gap is connected to heavy trace copper to a circuit board mounting hole that attaches directly to chassis ground when the PC board is installed into the final product.


The picture below shows a real circuit board where an array of spark gaps were used on a 9-pin mini-DIN connector application. An extremely beneficial location for the spark gaps is very near to the connector pins as shown. This picture also shows a good view of how the solder masking is kept away from the gap area to permit the air gap to exist.


Here is another example of the spark gap in use on another actual production PC board. The wide trace shown routes directly to a chassis ground mounting hole.


If you elect to use spark gaps in your designs then you should take note of the following additional considerations:

• If you pick a PC boad fabricator that severely over etches your board the gap width can be over etched to 0.008 or 0.009 inches. If this happens then the spark gaps become virtually useless.
  
  
• The semi-circular pad design is used because it has been seen to provide repeatable protection. If you use spark gap designs with a diamond or triangle point your gap width after board etch is far more likely to exceed the preferred 0.005 inch spacing. In addition diamond point designs have a much greater tendancy to burn back at the ocurrance of an ESD event leaving the spark gap useless for a second or recurrent ESD event.
  
  
• When you bring a PC board artwork set to a PC board blank manufacturer make sure that you point out that the gaps are designed to 0.004 inch conductor spacing and that your goal is to maintain 0.005 to 0.006 inch gap spacing after etch. I have worked with numerous vendors that normally are making boards to 6/6 design rules able to successfully manufacture the spark gaps to desired specifications even though the rest of the PC artwork may be 6/6 or 8/8 design rules.
  
  
• In production it is a good idea to sample check the gap widths on incoming board blanks. If your vendor messes up and starts giving you boards that are over etched you will not be building in the protection you thought you were getting.
  
  
• I have worked with multiple contract board manufacturers that build boards with spark gaps. If they do not have experience with spark gaps when you bring your first design to them you are sure to hear a batch of complaining. Work closely with your manufacturer and soon they will understand how to work with the gaps so that they do not present process problems.
  
  
• It is a good idea to make sure that the spark gaps on boards that are flow soldered are covered over with silicone mask to prevent bridging during the solder process. You can make things easier for the manufacturer if you organize the gap placement in a row like in the pictures above. This way a single squirt of the mask material can cover multiple gaps at one time.
  
  
• It is quite reasonable to place the gaps on the component side of a PC board and even place them under the connector body. It is essential that the spark gaps be located in a place where there is free air space in the gap area. If they are under the connector body make sure the connector is designed with a standoff that holds the body up off the board. DO NOTE HOWEVER I RECOMMEND PLACING ALL GAPS IN A CLEAR AREA so that they can be visually inspected.
  
  
• If you use an automated PC board test process with a fixture such as a bed-of-nails it is a good idea to make sure that the fixture has test points of access to both sides of each gap so that they can be tested for shorts.