www.logwell.com

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 laminate sales rep described it as being like a sponge) and will absorb moisture readily.  Assuming pristine dry polyimide, there is a slight advantage with respect to board resistance / leakage over FR-4 laminate, but at much higher cost.  If price is no object, there are also other exotic high temperature laminates available, but FR-4 as discussed below is often more than adequate.

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 (149° C) and even occasional 350° F (177° C) and slightly higher 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 depressed, 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 weak solder joints.

With present technology, the ENIG (Electroless Nickel and Immersion Gold) process seems to be 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, and it sure is pretty.

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.  Liquid photo-imageable (LPI) solder mask is the best choice for downhole PCBs, and it is commonly available in the ubiquitous green as well as red, blue, yellow, white, black, and other colors from some board houses.

Some solder mask formulations / colors may experience marked color shift after prolonged exposure to high temperature.  Both white and black solder mask are quite opaque, with other colors exhibiting varying degrees of translucency.  Since FR-4 will often darken / brown to varying degrees at high temperature, the translucent solder masks will appear darker or color-shifted from the laminate browning even if the mask itself is color stable.  Black solder mask is the most color stable at high temperature and its opaque nature hides traces completely and prevents a darkened board from being noticed.  Sadly, black has the worst resistance / leakage characteristics of the various solder mask colors, sadder yet because black mask with white or yellow silk screen legends, and gold ENIG plating makes for the ultimate PCB bling.  White solder mask would be good (decent leakage characteristics and excellent hiding power) but for its own unfortunate tendency to discolor in an uneven manner at 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 and high voltage filtration circuits, but certain critical signal processing circuits may also suffer if leakage is excessive.  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.

LPI solder mask has the best resistance / leakage characteristics, screenable liquid solder mask is in the middle (LPI is sometimes applied with a screen process, but this middle category is the old pre-LPI liquid), and film solder mask has the worst resistance / leakage characteristics (there are some exotic films that do not obey this generalized rule).  In our limited testing, we have found red LPI solder mask to have the best resistance / leakage characteristics followed by blue, white, green, with black being the worst (this generalization may not hold for all LPI solder mask vendors).  Tenting vias on downhole PCBs is not recommended (tenting is a trade term-of-art for applying solder mask over vias, and is most easily done with film solder mask).

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, red, and black are available from some board houses.  Long term discoloration at high temperatures is less pronounced with some formulations / colors than others.  We have had the best luck with white and black inks, but black cannot be used on most solder mask colors due to lack of visibility. 

Be sure to label all wiring connection points, all adjustments (like trimpots), and to be as generous with component labels as space permits.  Since tenting vias on downhole PCBs is not recommended, 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 (except for the occasional jumper).  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).  Sensitive signal traces should be kept a reasonable distance (perhaps .050 inch) away from drilled holes that are not plated-through.  In general, it is good design practice to keep all copper back from board edges by about half the board thickness, or around .030 inch for the typical board.  Downhole tool PCBs are usually quite small, so .030 inch seems like a mile in PCB CAD software when designing downhole boards.  From a practical perspective, edge clearance of .008 or .010 inch (8 to 10 mil) is plenty for even the most nit-picking of board houses.  In space critical situations .005 inch (5 mil) board edge clearance is usually acceptable.  A useful PCB CAD trick is to make the board outline a 16 mil line which will center on the actual dimension giving an automatic 8 mil clearance indicator; reset to a narrower or zero width line after completion of the design.

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 as 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.  As mentioned above, extra caution is needed in silk screen legend placement with bare untented vias to avoid ugly results.

"Restring" and "annular ring" are interchangeable terms for the copper pad around holes.  The restring or annular ring is measured across one side from the OD of the drilling to the OD of the pad.  Board houses differ in their acceptable minimum, with 10 or 12 mil being common.  A premium is usually charged for smaller rings due to the greater difficulty in making thinner rings concentric (drill locational accuracy issues).  Most boards we create have the design rules set to 12 mil minimum restrings, but rarely we must use 8 mil restrings / annular rings.  Exercise caution regarding restrings; both PCB CAD software and well-meaning board houses can cause all manner of headaches.

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 (there are situations where vias are unavoidable, of course).  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.

All PCBs will exhibit some leakage.  One path for leakage is the reinforcement fibers that form an integral part of the laminate and another major contributor is solder mask.  Obviously it is wise to go with the least problematic of the solder masks, LPI, and to stick with the colors that have tested well like red and blue.  But the importance of cleanliness cannot be overstressed.

Keep in mind that ion mobility and leakage currents double about every ten (10° C) degrees Centigrade; this is true for bulk semiconductors, all types of printed circuit boards, and all "insulating" surfaces, even glass and Teflon.  Fingerprints alone can leave enough ionic contamination to cause problems.  Always carefully clean downhole PCBs after assembly, especially if it will be used at high temperature.  Pure Grain Alcohol (PGA) a/k/a Ethyl Alcohol or Ethanol is a good choice for flux removal (we have been using it since 1,1,1 was outlawed).

As mentioned above, polyimide PCBs are notorious for their proclivity to absorb moisture.  This can be disastrous if a tool "goes wet" since well fluids usually contain salts, and ionic contamination is readily absorbed by a polyimide board.  For severe contamination, soaking or boiling a PCB in high quality distilled or deionized (DI) water (one megohm/cm quality at a minimum) for a prolonged period may rescue a board.  Long soaks in clean Ethanol or in clean consumer grade rubbing alcohol (70%, or better yet 91% Isopropyl Alcohol) may also help.  Completely Denatured Alcohol (CDA) sold simply as "denatured alcohol" in stores should be avoided for electronics use due to the undesirable additives used for denaturing the Ethanol.  For more information, see our Cleaning Secrets Revealed page.

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.  Here is a zipped package of Eagle files you may find useful if you use Eagle for PCB design.

There are countless PCB manufacturers or "board houses" located all over the world.  It is beyond the scope of this effort to recommend specific board houses (and none have offered an attractive enough bribe).  It is probably wise to avoid any board house that offers free proprietary PCB design software.  We previously recommended ExpressPCB for small quantities of printed circuit boards, but have reconsidered our position.  Their little PCB design program has a proprietary file output designed to lock customers into using only their service.  This is an unacceptable arrangement for a commercial customer.  For a $60.00 fee they will supply the Gerber files, but enabling Gerber file output would generate good will far exceeding any business they might lose (Advanced Circuits will supply free Gerbers after a second order when using their little PCB program, an offer ExpressPCB refuses to match).  It is far better to use a PCB design program that does not generate proprietary files.

At present, the best deals on having PCBs manufactured are in China.  Some Chinese board houses have a bad reputation when it comes to quality control, but others do an excellent job.  Be prepared for some difficulty communicating, but if you have done a good job on your PCB design, there will be little to communicate about.  It is entirely possible to have boards manufactured in China that meet or exceed the best domestic board house quality.  Shipping from China is amazingly fast and inexpensive.

No matter what board house you use, the key to minimum aggravation is supplying good information.  It is always a good idea to furnish a "Read_Me.txt" file with the manufacturing file package.  Here is a Sample PCB "Read_Me" File.

Happy PCB designing!

FTC Disclosure: Neither AnaLog Services, Inc. nor the author has an economic interest in any of the companies or products discussed above, and no monetary compensation was received.  Free samples have been received from various manufacturers.  None of the manufacturers was aware this page would be written.

01-18-10
Last 05-01-10