PCB Solder Jumper Pads

Summary
This blog summarises the tests performed on a selection of Printed Circuit Board (PCB) solder (bridge) jumpers. PCB jumpers are frequently found on PCB's used in electronic equipment. For testing, jumpers were reproduced on a single PCB in various sizes for comparison and testing purposes.

Solder Jumper Test PCB

Solder Jumper
The PCB solder jumper electrically connects two, or more, separate circuits. The function of the solder jumper performs is as varied as the type of jumpers seen on electronic equipment.

Solder Jumpers on LCD PCB

Solder Jumper Design
Some of the early solder jumper designs were novel as two or more pads places relatively close to each other, consider an 0201 style footprint. Either a blob of solder, a soldered zero-ohm link or a short piece of wire was required to join adjacent pads.

Some websites have entire pages dedicated to PCB jumpers for CAD packages such as Eagle.

Example Eagle PCB Jumper Design

 

The technique of using two pads is still widely used however, there have been some variations to the solder jumper design. For example, the forum posts on DIP Trace show four alternative jumper designs.

Changes in the solder jumper design have been a result of improving manufacturability, reliability when reworking the jumper and in some instances a general reduction in the footprint size.

For example, changing the two side by side pads, think of an 0201 resistor, to a chevron (arrow) or pad in pad can increase the mating area between the two solderable surfaces. An increased surface area can result in a better chance of solder adhesion. The adhesion can be important for boards that are run through reflow soldering.

Solder Jumper Prototyping
Some of the PCB jumpers depicted in this blog were replicated on a test panel. The focus of the prototyping was for small to miniature solder jumpers.

Unsoldered Jumper Test PCB

Only J11 has a minimal solder mask between the jumper pads.

PCB Arrow Jumper

J1 and J2 represent the arrow jumper which was created in a nominal and miniature size.

 

PCB Tongue and Groove Jumper

J3 and J4 represent the jumper design seen on portable/wearable electronic equipment. Two very small jumpers were created.

 

Various Ball and Socket Jumpers

J5 through J10 were designs similar to those presented on DIP trace with a few personal variants using a pad inside a pad.

Large Small Pad Jumper

J11 was a design mentioned on an Engineering blog where a larger pad with more solder was more likely to bridge to a smaller pad.

Side by Side Pad Jumper

J12 was a common design used by the Open Source forums for Arduino shields, OLED or LCD boards.

Dual Round Pad Jumper

 J13 was created to test round pads side by side.

Four Pad Jumper

J14 was inspired by the LCD to test a variant of inward facing arrows.

Testing Solderability
A 1.2 mm chisel tip (Hakko T12-D12) with lead-free solder was used to bridge the solder jumpers. As shown in the image below, not all jumpers (J2, J4, J11 and J13) would bridge using the chisel tip.

Chisel Tip Soldered Jumper Test PCB

The same chisel tip was used to remove the solder bridges. For most of the solder jumpers, the solder was removed in one pass. All jumpers were tested for continuity, none were shorted.

Chisel Tip Desoldered Jumper Test PCB

For a second test, a 1.0 mm 45 degree conical tip (Hakko T12-BC1) with lead-free solder was used to bridge the solder jumpers. Again not all jumper (J2 and J4) would bridge with the conical tip.

Conical Tip Soldered Jumper Test PCB

Desoldering jumper with only the 1.0 mm conical tip was time-consuming due to the small amount of solder removed in each pass. Desolder braid was required to remove enough solder from the jumpers in a single pass. Alternatively using a 3.0 mm 45 degree conical tip (Hakko T12-BC3) allowed cleaning of the jumpers without desolder braid.

As a third test with reflow soldering, solder paste (NC 254 SAC 305) was applied to the PCB manually.

Solder Paste Application on Jumper Test PCB

The result of the reflow process was that the smallest solder jumpers, J2 to J4 and J11 and J13 formed a bridge. Any soldering iron tip could be used to remove the bridge. Larger pads did not bridge likely due to the pad size and small amount of solder paste.

Reflow Solder Result on Jumper Test PCB

Summary
For testing in this blog, soldering iron tips in the form of chisel, conical and different 45-degree were used.

Using the metrics of solderability and ease of desoldering, jumpers J5, J7 and J12 worked with all the types of soldering iron tips.

The smaller jumpers, J2, J3 and J13 required a small tip for reliable production of a solder bridge during hand soldering.

Jumpers J4 and J11 did not solder reliably using hand soldering however reflow soldering was successful in all three attempts.

Larger jumpers J1 and J4 together with the multi-pad jumper J14 required larger soldering tips for creating the solder bridge. These jumpers were not tested extensively with reflow soldering.

Some of the jumpers detailed in this blog are found in hobbyist or consumer equipment with each designed to suit their application.

To suit the home hobbyist, jumpers J1, J5 or J12 would be ideal choices.

Finally, a note concerning PCB production. The smallest jumpers with small pads and 0.1 mm pad to pad spacing significantly increased the cost of the PCB; a salient point when moving to miniature or high-density PCB designs.

Downloads
Gerber files downloadable using the link below.

Jumper Gerber Files

PCB vias solder mask tenting

Summary

This blog highlights some of the implications for PCB 'board' loaders during the reflow or wave soldering process when Printed Circuit Board (PCB) designers choose not to tent solder side vias.

PCB Manufacturer Tenting Limitations
With the advent of higher density devices such as microcontrollers with configurable logic, Field Programmable Gate Arrays (FPGA), System On Module (SOM), System On Chip (SOC) and high power FET drivers becoming more prevalent in commercial equipment and hobbyist designs, there comes a requirement to manage exposed pads and vias beneath these devices. 

In some instances high density components may have an exposed pad that require a connection utilising vias for a variety of reasons. The exposed pad may serve as electrical connection, such as an input power supply, output in the case of a switch mode regulator, the pad may be used for PCB mounting by providing bonding strength (due to the ever decreasing component footprint) or for heatsinking, by acting as a thermal pad such is the case for high power FET drivers.

In the image below are a few examples of different sized vias which have been used for different reasons on the same PCB.

Tented and Untented Vias

Identified in the red box are vias which are used for standard TTL signal connections. The via hole size is 0.3mm. Vias with this hole size are commonly tented during the PCB manufacturing process using solder resist, unless they have been earmarked for alternative purposes such as test points, probing, programming or other similar purposes.

Shown in the light blue box are larger vias with a 0.7mm hole which are used for connections to the PCB internal power planes. Vias of this size are tented where possible unless there is a good reason not to do so or the PCB manufacturer is unable to mask to this via size. Reasons for not tenting may include thermal connections to exposed pads or a need to increase the current handling capacity of the via. Both of these reasons may require solder or a 'plug' to fill the via.

The purple box shows a cluster of untented vias with a 0.5mm hole. These vias reside below a microcontroller featuring an exposed pad. The vias on both sides of the board are not tented although these vias are usually tented on the solder (non-component) side of the PCB.

Lastly shown in the yellow box is an array of vias with a 0.381mm hole. The grouped formation of vias is commonly termed 'stitching' in software packages such as Altium Designer. For this design the top and bottom copper layer represent the ground plane which are stitched together using multiple vias. Vias of this size and smaller are usually always tented.

For the example board shown, almost all of the vias are listed as tented in the PCB file and the Gerber files. Clearly not all the vias appear to be tented in a thick solder mask. The reason for the discrepancy can lie with the capability of the PCB manufacturer. Not all PCB manufacturers detail their limits for tenting vias with solder mask or are able to open the latest PCB files from software packages such as Altium Designer (a good reason why Gerbers are used in the industry). This issue can be remedied to some degree by supplying the Gerber files to the manufacturer, in the format requested, and then asking to verify the machine Gerber files that the manufacturer intend on using in their PCB production equipment.

PCB designers should be mindful however that even the final Gerber files supplied by the PCB manufacturer may not always be what is actually produced. For example, mutlilayer boards with power planes to the edge of the board will have, in general, a 'pullback' rule applied to that layer even if the PCB does not have a pullback rule. To prevent these rules from being applied by the PCB manufacturer comments or notations should be explicitly noted on the PCB file or Gerber file as 'no pullback on this layer'. Somewhat off topic although this concept also applies indirectly to vias and solder mask.

With regards to the maximum size of via which can be covered with solder mask, for a standard manufacturer a 0.8mm hole may be too large where for the more experienced or better tooled manufacturer, a 1.2mm hole may be considered the upper limit. Asking the manufacturer will at least provide an idea of their manufacturing capability. This information can then be included in the PCB design file for the PCB manufacturer.

Via Placement and Tenting Issues
A single untented via rarely causes placement or issues for the PCB loader. The word rarely is used with caution however because a single, poorly placed via, without tenting can cause issues when located too close to another surface mount component, to the pad of a PCB mount metalised connector or the under the metal body of a mechanical component such as a HDMI connector.

The image below shows vias with an equidistant spacing of 1.1mm connected to a component with an exposed pad on the opposite side of the PCB. A via spacing down to 0.5mm should usually not cause a problem for the PCB loader whether the soldering process is reflow, as shown below, or solder wave.

Via Spacing

Shown in the subsequent image is a higher density via placement with a spacing of 0.8mm. Due to the increased number of untended vias and possibly solder paste, the solder readily flows from the top side of the board to the bottom during the reflow process.

Higher Density Via Spacing

Although the protruding solder could easily be removed as part of the post manufacturing process, this additional work can increase the final PCB cost and is best avoided during PCB design by tenting the vias. It should also be noted that the solder protruding from the vias may not be excess solder but instead solder that should be between the exposed pad of the component and the copper pad of the PCB.

No Via Tenting
Where vias are used for other purposes, such as ground planes or heatsinking, the PCB designer has the option to leave the via with no tenting. During the PCB population process solder may fill the vias, although using solder to fill vias in this manner is not a guaranteed process. The image below shows the via arrangement under a high current switch where not all of the vias have been filled with solder.

Staggered Via Layout Connected to Polygon

The subsequent image shows the component side of the board without the physical component fitted.

Staggered Via Layout Component Side

Via Tenting
Although this blog focuses on vias without tenting, it should be noted and sighted in the image below, that even vias with a 1mm hole can be tented with solder mask by a sufficiently qualified PCB manufacturer.

Tented Vias Connected to Polygon

Design Suggestions
Knowing the limitations of the PCB manufacturer and the PCB loaders soldering process would allow ideal selections to be made during the PCB design process.

This comment is idealistic, not realistic. 

More often than not people utilise online PCB manufacturers which do not fully disclose the capability of their PCB manufacturing equipment. Additionally the PCB manufacturer's website may be a PCB broker that farms large groups of common layer boards to the most suitable PCB manufacturer at that time.

With this in mind, the suggestions below for tenting and spacing, of through PCB vias, are for a typical PCB manufacturer and largely depend of the via size and use.

Max via hole size for tenting: 1.2mm
Min via to via land separation for untented vias: 0.3mm
Min via to via land separation for tented vias: 0.15mm

Tented Vias Connected on Multiple Polygons