Home

There are as many ideas about what constitutes good design of downhole printed circuit boards as there are designers (actually more since everybody in the logging business has opinions about PCBs).  Printed circuit boards have been used in well logging tools for decades, though there have also been point to point wired tools produced in the past.  This page is an effort to collect some thoughts about PCB design philosophy.

Downhole PCBs have traditionally been made from glass reinforced polyimide resin; this is the same stuff known as Kapton in its film form.  Polyimide should not be confused with polyamide which is more commonly known as Nylon, and which cannot take the temperature extremes of polyimide.  While polyimide has superior high temperature capabilities, it is not without its shortcomings.  Polyimide is quite hygroscopic (one board material sales rep described it as being like a sponge) and will absorb moisture readily.  A tool that goes wet will be hard to resurrect if it contains polyimide PCBs since the boards will not only absorb water but also the ionic contaminates in the well fluids (there are some tricks of the trade like boiling in distilled or deionized water).

Conventional glass reinforced epoxy resin laminate known as FR-4 (FR stands for flame retardant) has been used successfully in downhole tools up to surprisingly high temperatures.  It is recommended that high Tg FR-4 be used for downhole applications.  Tg is an abbreviation for glass transition temperature, the temperature at which a material changes from a hard and relatively brittle condition to a viscous or rubbery condition.  Garden variety FR-4 has a Tg of around 130 to 140° C, but Tg 170 or 180° C  FR-4 is readily available.  As FR-4 (or any laminate for that matter) approaches its Tg, there is accelerated Z axis expansion.  This Z axis expansion is potentially deadly to plated through holes, and it is plated through barrel failure that is the principal concern with using FR-4 at or above its Tg rating.  There are tricks to help minimize any potential problems like using redundant vias, replicating traces on the top and bottom copper layers wherever possible, and always soldering a wire in all plated through holes where traces switch sides.  From a practical perspective, high Tg FR-4 can be successfully used in logging tools that will see 300° F excursions, and even occasional 350° F exposure if proper precautions are observed.

Downhole PCBs are typically soldered with high temperature solder (see A Word About Solder).  It is important that no lead be allowed to contaminate the newer tin / silver high temperature solders or the melting point will be reduced, so conventional tin / lead solder plating should not be used on downhole PCBs.  Silver and nickel have both been used for downhole PCBs, but both have solderability issues after a relatively brief period due to inevitable oxidation.  Pure tin has been used, but there is always concern about "tin whisker" formation.

Straight gold plating has been used in the past, but there are known metallurgical problems with gold plating due to copper dissolving in the gold and creating brittle solder joints prone to failure.  A nickel plating barrier between the copper traces and the gold plating can prevent the copper from dissolving in the gold, but a thick gold plating can cause its own problems with intermetallic compounds that can cause solder joint failure.

With present technology, the ENIG (Electroless Nickel and Immersion Gold) seems like a reasonable choice.  Several downhole tool manufacturers are using ENIG on their PCBs.  The gold layer is much thinner than that obtained with electrolytic plating, hence less likely to cause problems.  In comparison testing, ENIG had the best solderability after long storage of any of the now commonly available surface finishes.

Historically, downhole PCBs were made without solder mask, also called solder resist.  However, solder mask is very nice to have, especially with modern surface mount parts (it is a must with automated assembly).  Solder mask must be tough enough to withstand mechanized assembly processes which involve high temperatures at least for a brief time.  Conventional solder masks appear able to withstand high temperatures encountered in well logging tools, but darkening of green solder mask has been observed after prolonged exposure.  Solder mask is commonly available in the ubiquitous green as well as red, blue, yellow, white, black, and other colors from some board houses.  Some colors may experience marked color shift after prolonged exposure to high temperature.

On high voltage PCBs, leakage has been observed at elevated temperatures when solder mask is used.  It may be advisable to avoid solder mask on high voltage PCBs, and to have them made as "bare bones" boards without solder resist.  This would include high voltage power supplies, high voltage filtration circuits, etc.  However, since some colors from some solder mask formulators can exhibit up to a couple of orders of magnitude less leakage than other colors, it may be possible to use solder mask on high voltage PCBs after appropriate testing.

Silk screen legends are usually white.  Again, the inks used appear able to withstand high temperatures encountered in well logging tools.  Other silk screen ink colors like yellow and black are available from some board houses.  It is possible that long term discoloration at high temperatures could be less pronounced with some colors than others.  Be sure to label all connection points, all adjustments (like trimpots), and to be as generous with component labels as space permits.  Tenting vias on downhole PCBs is not recommended, so place labels accordingly to prevent ugly silk screen results.

The worst mistake some designers make on downhole PCBs is to use narrow traces.  As a practical matter .020 inch (20 mil) is about as narrow as should ever be used downhole.  Whenever possible .030 inch (30 mil) should be the minimum trace width used.  With downhole PCBs bigger is better with respect to robustness and serviceability.  If smaller traces must be used, consider "tear drop" or equivalent structures at pads to reduce stress.  If smaller traces are needed to pass between pads of devices like integrated circuits, consider "necking down" trace width in just that area.  It is good practice to replicate traces on both the component side and the solder side of the board whenever routing constraints allow same.  This redundancy could be enough to prevent tool failure in certain circumstances.  Trace clearances should be as great as practicable, but probably never less than .010 inch (10 mil)

Again, with downhole PCBs bigger is better with respect to robustness and serviceability, and this applies to pads and vias as well as trace width and spacing.  Use the biggest pads for through-hole components and for vias space constraints permit.  Consider dual vias for dependability (high temperatures and temperature cycling contribute to the likelihood of plated through hole barrel failure).  Soldering wires through vias may help prevent failures attributable to plated through hole barrel failure (silver filled epoxy is sometimes used to fill vias, but this may not be as effective at high temperatures).  Vias probably should not be tented on downhole PCBs so they are available for testing or soldering wires through for remediation if not done when the board is initially populated (tenting is a trade term of art for applying solder mask over vias).  As mentioned above, extra caution is needed in silk screen label placement with bare vias to avoid ugly results.

Decent downhole PCB layout is labor intensive principally because of the limited space available.  Typical downhole boards may be only 0.6 to perhaps 1.0 inches wide with 0.75 or 0.8 inches being fairly common.  Such limited space may necessitate non-intuitive layout solutions, and will usually vex auto-routers.  As discussed above, it is always wise to avoid vias on downhole PCBs, but doing so may require a little extra effort with respect to component placement and routing.  Always budget adequate time for downhole PCB design; very often, revisiting the board after a brief hiatus will result in a brain storm leading to much better routing than initially envisioned.

Surface mount (SMT) technology is all the rage, and is indeed a wonderful innovation.  However, it is arguable that through-hole components make for a more robust and serviceable downhole circuit board.  No matter how stubborn a designer might be, it is now practically impossible to escape the use of some SMT components due to cost considerations (some leaded high temperature capacitors can cost over twenty times as much as an SMT version, for instance).  Hybrid boards with both through-hole and SMT components are common in well logging tools these days.

Board design has come a long way since the days of dry transfer symbols and black adhesive tape for laying down tracks.  There are dozens of PCB CAD software packages, including a few pretty good free open source offerings.  Eagle is a moderately priced package used by several logging tool industry players including AnaLog Services, Inc.  Eagle is produced by Cadsoft which has recently been acquired by the Premier-Farnell-Newark empire; looking at said acquisition in the best possible light, at least there is an indication Cadsoft will be around for awhile.  Eagle is far from perfect, but it is a very powerful package at a very good price if you can get past the learning curve and acquire the "Eagle Way of Knowledge" (ala Carlos Castaneda).  The Yahoo eaglecad reflector mailing list is a wonderful resource with a group of great guys who are amazingly generous with their Eagle expertise.

Happy PCB designing!

| Home | Tech & Tips | Downhole Hardware | Service Tips | PCB Photos | PCBs |

01-18-10
Last 10-20-10