Last update:


Site Map Location FAQ

  FAQ Menu

PCB Design
PCB Manufacturing
PCB Assembly
Company Info
Contact Us


Questions and Answers

Q: Hi, Here is a question that has just popped across my desk from an engineer. A board has been populated (All SMT - 0402's, BGA's, etc.) mounted into its housing on stand-offs. How much deflection is acceptable if the board has not been properly supported in the middle?

Is there a specification for this? Thanks In Advance. - Alan


A: Alan,  I will attempt to address your question as best I can given the information you provided.

A properly designed non-flexing enclosure with rigid mounting for the board should restrain the rigid board from flexing. If it isn't properly restrained, it isn't designed correctly to survive for long. How long must it survive the potential stress it will encounter? Which particular mode of 'flexing' are you most concerned about?

A pressure from a human finger pressing a switch or button? Or, perhaps the flexure that happens under continuous sinusoidal vibration at some given frequency? Or perhaps instantaneous shock of some given number of g-force in inch/lbs? Or simply the expansion and contraction of the material over temperature... perhaps all four?

The survival of the circuit depends on it NOT being stressed beyond its ability to recover intact. Work hardening of solder joints and the components mounted to the board through that solder joint can cause them to fail. Repeated flexing can cause breakdown of the epoxy/fiberglass board, glass fibers, or other materials, or even the copper conductors and their adhesion to the board material can suffer from work hardening and structural failure can be a possibility... if the vibration is intense enough and sustained over a long period of time.

As far as my seeing a spec that calls out an acceptable maximum single flexure of a rigid board electrical assembly, I really have not seen anything that specifies a restriction on that particular design feature. Most requirements are saying that it must not fail given a certain maximum or minimum environmental exposure. If you were using Flex circuit materials it would really be able to survive a lot of flexing, but the components might not... it all depends on how you protect the solder and components from being exposed to undesirable stresses that cause failures.

Your board may survive a tremendous flex of many inches... once, or twice, but if you repeat it over and over, eventually you will find the breaking point and the weakest link will fail. Each board will be different depending on the modulus and tensile strength or even ductility of the materials involved and what amount of stress is being applied to the assembly and where and how often and at what temperature and humidity.

Sorry it isn't a simple yes or no question... I don't suppose that any of that helped with your question a bit. - Bill


Q: Does anyone have any tips on manufacturer's of 1/4 W resistors in packages smaller than 0805? Everything I've seen is 0805 or larger and I need something smaller. I know one manufacturer makes 0402 but the resistances they make are very, very limited.


Matt B.



A: IF you are trying to convert a 'thru-hole technology' board to surface mount technology the ¼ watt rating may be 'over kill' to start with. Many older through hole circuit designs that specified ¼ watt axial leaded resistors were done so for cost and availability reasons rather than being required by design. It may be that the 1/8 watt 0805 or the 1/10 watt 0603 or even the 1/16W 0402 surface mount resistors would work just fine in your circuit but you need to evaluate the circuit for the amount of voltage and current required worst case to determine the appropriate watt size needed.

You can see some of the standard watt sizes for surface mounted resistors at the following link.


To evaluate the circuit you need to understand Ohms Law...

E=IR, R=E/I, I=E/R

Voltage equals the Current times the resistance
Resistance equals Voltage divided by the current
Current equals the voltage divided by the resistance


Power in Watts equals the current times the voltage
To find the maximum current the resistor will see in the circuit you need to know the maximum voltage the resistor will see in the circuit and solve for maximum current I=E/R or the current equals the voltage divided by the resistance in ohms.

Once you know the maximum worst case voltage and current you can solve for how many watts will be dissipated in the resistor, worst case...

Let's say you had a 10 volt battery source and a 100K ohm resistor as the load... since the power is steady 10V is the worst case voltage is 10V and so we plug that into the equation I = E/R so I = 10V / 100,000 ohms = .001 amps....

Now we look at the power P = I x E which is P = .001 amps times 10 volts which is .01 watts

So you would need a 1/100th ( .01) of a watt resistor to dissipate the heat to be generated which would suggest you use a 0201 size part at the minimum since that is the smallest available and is a 1/20th watt part still 5 times more than adequate to the job.

Now you might not want to go that small because of limitations on availability or price or lack of pick and place equipment to handle it or test it... but you certainly could go larger with the package size and get a part that would meet all of those needs and still work in the circuit... and that might be more cost effective.

I hope that description is helpful in your situation as you really did not describe WHY you needed a surface mount part in ¼ watt size in something smaller than an 0805 package... it may have been less complicated than that but it was a great opportunity to look at it from a different angle...

Q: If I do immersion gold/electroless nickel on top of an impedance line will it affect the result?

 Steve Kelly

PFC Flexible Circuits Limited



It depends....

What results are you trying to 'not affect'?

Nickel is lossy at RF frequencies.. The higher the freq. and longer the

transmission line the worse the effect gets if I remember correctly from my

Microwave days...

Does it change the impedance of the line... probably not.

Impedance is a result of the relationship between the dk of the material,

distance of the conductor from it's return path or ground plane and the

width of the transmission line... in a microstrip arrangement.

I don't believe the thickness of the plating is a large enough influence on

the line to change the impedance by any measurable amount.

But lossy RF might be a reason to choose a different surface finish that

doesn't contain nickel. Especially if you are dealing with very low voltage

signals... It's kind of like a trickling stream running along a nice solid

rock bed and then suddenly hitting a huge sand bar... where the water slows

and sinks into the sand... disappearing from view completely... You don't

want nickel plating on high frequency boards.

If it's not that sort of an application, then you most likely will not have

a problem.


Bill Brooks, CID+

Q: From Steve Gregory on Technet -  - We just recently built some boards here that have a hand full of SOD323 packaged Schottky diodes from International Rectifier on them, and have had a pretty serious problem with the part and pads being ripped off the board. It's been happening mostly during hand cleaning.

We have a open cased DC/DC converter that we have to hand solder, and then hand clean. No, we can't use no-clean flux and leave the residues, the customer won't allow it. But that's where it seems they are getting ripped up. After the first couple of diodes got ripped up, we've made it known to the operators who are working on these assemblies how easy it is to do this, and that they need to be very careful when cleaning. We've got our best operators working on these assemblies, and I know their skills. But even when they try to be as careful and gentle as they can cleaning the assemblies, parts are still getting ripped-up...it's really unbelievable how fragile this part is.

Has anybody had similar experiences with this part?

I've got pictures of things on my page. Go and look at:


There you will see a picture of the part. The part is kind of tall in relation to the size of the two pads it gets soldered to.
Now look at:


There you will see what International Rectifier recommends for a footprint...pretty small pads huh?

Now look at:




This is what I measured the footprint to be from the Gerber for the board. The pads are a little undersized from what International Rectifier recommends, and they also are oriented 90-degrees out from the recommended footprint, but do you think that difference explains why these things are so easy to damage? Would you go with larger pads than what is recommended to provide more surface area for the pads to provide more mechanical strength to them?

Just curious if anybody else has had the same problems..

-Steve Gregory-


-----Original Message-----
From: Roger Stoops [mailto:Roger_Stoops@Trimble.com]
Sent: Tuesday, November 16, 2004 9:56 AM
To: TechNet E-Mail Forum; Brooks,Bill; Steve Gregory
Subject: RE: [TN] SOD323 problem...


Okay, I misread the package type, thought it was a SOD123.  But we still have had no problems (yet) with the 323.  Used the latest version of the PCBLibraries calculator to derive the "latest" land pattern for the SOD-323, and the calc says 1.4x.5mm lands on 2.2mm center (3.6mm overall length).


Sent a pdf file with what the calculator came up with.  For $57US, the   calculator is a pretty good buy, takes a lot of guesswork out and meets IPC-735x standard.  (http://www.pcblibraries.com)


Attachment sent to Bill and Steve, maybe Steve could put it on his website for comments?






I modeled the part from its spec sheet and this is what it looks like to scale... compared to another part from ProTEK  - and the one from PCB libraries...  notice the pad geometries...


SOD323 land pattern.pdf





I would guess the IRF pattern is undersized...as you indicated in your e-mail... The PCB libraries one looks long and skinny for lack of a better description, I wonder what advantage is gained by that...perhaps they are trying to increase the amount of 'heal' on the solder fillet.   I like the look of the Protek pattern much better, just intuitively.... However, it may let the part skew more than the PCBLibraries one does as it would limit its movement in the 'Y' axis and allow adjacent parts to be closer.


- Bill Brooks, CID+




Q: Will FR4 material handle a trace with 2500VDC or is there a better laminate material to call out?


A: According to MIL-P-13949/4C for FR4 material, The Electric Strength, (perpendicular to laminations), average, minimum volts/mil = 750 V per mil (.001) which is 29.25 KV per mm as one millimeter = .039 inches.

I believe this has not changed over the years. It has been my guide for designing boards for years. A good design would de-rate by 50% and allow for tolerances.


All of the Woven E-Glass materials in the IPC-4101 spec call out 30KV/mm for cores that are less than .0197 thick, a direct take from the Mil-P-13949 spec for 'Electric Strength'. I don't know if anyone has done some demonstrations of this, however, if I was tasked with this and was concerned about verifying the results, I would include a test coupon on my boards and require the board vendor to test lots to verify that the boards pass the voltage requirement. A couple of areas on the panel that were an example of the circuit configuration would be a good test case and allow non-destructive testing outside the bare board area.


In your case, I would use an FR4 type laminate and make sure I had 6 mils or .15mm between the layers that carried the high voltage. That's like 3 layers of 2 mil thick prepreg. This will ensure that you have some margin on the break over voltage, of 2,500 volts which at minimum, when all the tolerances go against you, must be 3.3 mils. That means, check to see if the voltage is a max level or peak voltage. Can it spike over the value you are targeting?


You must also think about break over voltage on the surface of the board between conductors and keeping the circuit material surface clean from any contaminates that could create an ionizing path for a spark. Some circuits are very sensitive and need protection from 'leakage' as well and you might want a ground barrier in cases like that between the source and victim traces.



Q: Occasionally, we find it necessary to have boards built where we do not have supporting Gerber data files. Only the original film exists which we have scanned to Gerber data. Can you recommend companies who can scan film to Gerber?


A: There is one company I have used for years to scan in film or artwork. Talk to Holley Erwin.


    Cad /Art Services, Inc.

    12170 Flint Place

    Poway, CA 92064

    Tel: 858-375-3000 FAX: 858-375-3006

    BBS: 858-375-3007




Q: I am making my degree thesis and I am trying to find an answer to the question: How much cheaper is it to use SMT components than THT components to do same electronic product?


A:  I think 'bean counters' or accountants make a living answering this sort of question. Statistics on component sales and the like are probably available from the manufacturers in their stock holders reports... there may also be info available from organizations that support manufacturing and distribution and assembly. In fact you may find some info available from the IPC...


The big problem I find with your question is its too general. There are many factors that affect 'cost' which could be rolled into a study of 'which is cheaper'. The retail purchase price of a component of either type is not the only factor to consider. Machine handling, layout 'real estate' which affects the cost of the board, stocking space, special requirements for board surface finishes, brokers fees, international taxes and tariffs, component development costs, materials costs... I'm sure there are probably other aspects that don't come to mind at the moment.


Generally, surface mount components are more cost effective to use for most applications. The larger volume demand for manufacturing and ready availability through distribution of these parts makes their retail cost lower. Also their wide use drives the sale of pick and place assembly machines or availability of contractors that have them and the capacity to do the assembly of surface mount parts. Through hole components and the machines to automate their assembly used to be the most common parts and methods back in the 1980's. Most electronics manufacturers have transitioned to smaller more compact high volume electronic assemblies with surface mount components. They are now the most common parts available, hence the most cost effective to use for new applications.


That does not mean that THT or 'through hole technology' does not have a place in electronic design. There are clearly conditions under which surface mount components are not a good choice. Extreme vibration, extremes in hot or cold environments, high reliability applications, all require through hole parts to survive... The leaded brothers of our surface mount parts have a more robust ability to withstand abuse. So you will find them in military applications and in high-rel products or aerospace applications often. They are much cheaper than having to replace a surface mount version over and over due to failures, which could cause very expensive damage if they happen at the wrong moment in time... replacing a board on the Hubble Space telescope is not cheap.


Cheaper is a relative term... you really have to take into account many factors and decide, is it cheaper how and for whom?


At any rate, Good luck with the research project. I hope the thesis goes well.



Q: Can anyone quote the spec for how close a non-plated thru hole can get to the board edge? I know the rule of thumb, but I need to see something in writing.

A:  I have made 1/2 a plated thru hole ON the board edge... I don't believe there is any restriction on hole to edge spacing but there are good design practices that we all follow. That should not stifle a designers creativity in solving packaging challenges. A non-plated hole is typically used for tooling or mounting... Some boards break out the hole like a slot in the corners... I don't believe we are restricted in 'hole to edge' spacing by any specs, plated or non-plated.



Q: What would a standard via size be for a SMT board using 10 mil traces, Diameter?, Hole size?

A: That would depend on the aspect ratio, dia. vs depth of barrel. The process of plating into the holes gets more difficult the 'longer and skinnier' or more narrow the barrel of the hole is. The other cost driver is the accuracy requirements and annular ring restrictions place on the board. Most shops can handle 14 mil holes with 24 mil pads.... in a .062 thick or thinner board without a cost hit. There are a growing number that can do much smaller vias in smaller pads but the costs go up. Here is an interesting contrast, look at the following site and compare what is being done.




Q: I was reading about fiducials in J-STD-013. Are they necessary or just something that may come in handy? Might a board assembler tell you he can't pick and place if you don't have them? My board has 4.9mil traces and spaces and many of my components are 10mils apart.


A: Fiducials are highly recommended for surface mount component placement. I think some assembly machines can deal without them by picking an unused pad nearby but its much harder and more error prone without them. You should try to use them.


Also you can add global fiducials on the manufacturing panel to help. Local fiducials are good when you have a fine pitch part like a QFP package or BGA. They are only 3mm in overall diameter counting the clearance and if you locate them at diagonal opposing corners they work best.


If you contact Jerry or Jeff Hughes over at Hughes Circuits in San Marcos, he can give you some of the Pro's and Con's... and workarounds. 760-744-0300.


Also a good reference book on the subject of Design for Manufacturability is available from Printed Circuit Technology, P.O. Box 334. Burlington, MA. 01803 (781)438-0064 published in 1997 called "Bare Board PWB Design Manual by Norman S. Einarson ". This is a great little book that was distributed to me by CORETEC a number of years ago.


It sounds like from your description that your board will be a candidate for fiducials on the panel edges.


Also, check IPC-SM-782 page 24, figure 3-14, for a description of proper fiducial creation and figure 3-15 for placement.


Q: If I have a 6A/110V fuse in my circuit, can I use a 6A/250V fuse in place of it?


A: The correct answer is 'yes'.

  The fuse voltage rating is: "The ability of the fuse to quickly extinguish the arc after the fuse element melts and the maximum voltage that cannot jump across the gap of the fuse after the fuse opens." The current rating is: "The amount of current the fuse will allow without opening." The higher voltage rating is fine and actually more safe, but still using the same current (A) rating for this is the current that must not be exceeded or damage can occur to the circuit it is protecting. Specifically, the voltage rating on a fuse is pretty much determined by its length since that determines the gap after it melts. The longer the fuse, the higher the voltage rating. Since fuses are insensitive to voltage changes, the proper voltage rating selection is strictly a safety issue. Fuses can operate at any voltage below their rated voltage.

Ref: http://www.belfuse.com/Data/DBObject/fuseterm.pdf


Of additional interest is the article written by Doug Brooks (no relation) of UltraCad Design, Inc. in Washington State entitled "Fusing Current: when traces melt, without a trace" . He speaks of how to design a trace that acts like a fuse on a PCB.




Q: I was reading EDN yesterday, and noticed a picture of a PCB with vias through the pads for 0805 chips. Is this allowed? I guess the solder would fill the via, but who cares, right? What do you suggest?


A: It can be done, but the via must be very small diameter. Otherwise it will tend to 'suck' the solder away from the part and you won’t get a good solder fillet. The pcb manufacturers will offer to fill the vias to prevent ‘thieving’ of the solder for a ‘price’ with conductive epoxy and over plate the top and bottom of the via… This gives you an ‘invisible via’ that takes up no additional real estate on the board, but understand the epoxy material can and will expand at high temperatures and pop the plated tops off the vias, most likely causing a failure. So use this method with caution... More research into via-in-pad technology is called for before going down that road. Notice the lead on the SOT-23 where a via is in the center of the pad...


Do not confuse this with laser vias in pads. They are much more reliable than a plated through hole via in a pad that travels all the way through the board. A laser via usually only goes through one layer of the board to the layer just beneath it. It will not take away solder from the connection.



There is some reading material on-line regarding that type of via. .



Understand that with each higher level of complexity, you jump a corresponding level in cost. You should consult with the manufacturer before embarking on this sort of design strategy. But it's nice to know it CAN be done, when that is just the solution you need to get your product to market.







Q:  Out of curiosity, is there a recommended clearance between two through-hole solder pads, assuming it is too small to run a trace through.


A: There are no recommended clearances between pads except those driven by design with maybe the sole exception being annular ring requirements for through-hole pads. Even in that instance you are limited only by tolerances.


For example:

  1. If your through-hole component is going to be auto-inserted, the machine that does the insertion will have guidelines for clearances to avoid crashing the head of the inserter or clincher into the component next to it (see IPC-2221 Section 8).
  2. The proximity of pads to adjacent pads will also determine whether or not the wave soldering machine will short the pads on the primary side of the board when the wave soldering is done.
  3. The voltage levels in the traces will determine how much spacing is required in order to prevent flash over or arcing.
  4. The manufacturer you choose will have limitations on how fine line a space they can maintain with their etching process or imaging process. Today most shops can do 5 mil lines and 5 mil spaces. (0.127mm for those who read in millimeters) If you want to use the less expensive shops, give them more spacing. I use 8mil lines and 8mil spacing, typically, when at all possible.
  5. Access to the pads with test probes may also drive their spacing.
  6. Electrical interference or noise could also be a factor in the spacing between through-hole pads...


There are probably other issues, but I can't think of any at the moment... But, as far as I know, there are no specific rules that say " a through-hole pad must be X amount of distance from any other through-hole pad"... Just make sure the other issues are taken into consideration when spacing them. It is customary, to use a grid to make holes on some finite spacing if you can. But it's not 'required'.


Just use good design practice and your designs should be fine.






Q:  Where would I find info on trace spacing based on voltage levels? How far should components be spaced for 1000V vs 4000V that type of thing?


A: Get a copy of IPC-2221 and IPC-2222. Its a good investment in your career. The old  "0.0002 in./volt" (0.00508 mm/volt) reference in there originally came from MIL-I-46058. It refers to this being the standard spacing for voltages over 500V between conductors, DC or AC Peak Volts from sea level to 10,000 ft. for an "uncoated board"... Per IPC-ML-910A... and for "coated and internal layers" on a board, according to MIL-STD-275D & IPC-ML-910A it was .00012 in./volt (0.003048 mm/volt). Above 10,000 ft. it says .0010 in./volt (0.0254 mm/volt)


Now I just went to my copy of the IPC 2221 specs, table 6-1 on page 39, and it says basically the same thing... but only in metric, they leave out the inches... (Thanks goes to San Diego Designer Tom Hausherr, CID+, the 'Metric System' promoter for encouraging the IPC to change from inches... The rest of the civilized world uses metric.). I believe IPC has gone all metric so unless you are good at translating... the calculator sounds like a good idea. I have this little windows utility called 'convert.exe' that translates between inches and millimeters for me... I still get it wrong from time to time on my pocket calculator... (I hate when that happens...) I learned in inches and the change over will probably affect me for life... <twitch, twitch>  :)


So, for your 1000 Volts AC/DC at sea level to 10,000 ft ASL (3048 m) conductor to conductor spacing on your board should be:


Std 500v spacing 0.1 in.(2.54mm) plus the remainder(1000v-500v)= 500v

500V x .0002 in/volt or .1 inches (2.54mm) add that to the original .1 in. and you get 0.2 inches or (5.08mm)


Voltage Between Conductors

( AC Peaks or DC Volts )

Minimum Bare Board Spacing







0.05mm (.002 in.) 0.1mm (.004in.) 0.1mm (.004 in.) 0.05mm (.002 in.)
31-50 0.1mm (.004 in.) 0.6mm (.024in.) 0.6mm (.024 in.) 0.13mm (.005)
51-100 0.1mm (.004 in.) 0.6mm (.024 in.) 1.5mm (.06 in.) 0.13mm (.005)
101-150 0.2mm (.008 in.) 0.6mm (.024 in.) 3.2mm (.126 in.) 0.4mm (.016 in.)
151-170 0.2mm (.008 in.) 1.25mm (.05 in.) 3.2mm (.126 in.) 0.4mm (.016 in.)
171-250 0.2mm (.008 in.) 1.25mm (.05 in.) 6.4mm (.252 in.) 0.4mm (.016 in.)
251-300 0.2mm (.008 in.) 1.25mm (.05 in.) 12.5mm (.492 in.) 0.4mm (.016 in.)
301-500 0.25mm (.01 in.) 2.5mm (.1 in.) 12.5mm (.492 in.) 0.8mm (.0315 in.)
>500 add ---> 0.0025mm/volt( .0001in.) 0.005mm/volt(.0002 in.) 0.025mm/volt(.001 in.) 0.00305mm/volt(.00012 in.)

B1 - Internal Conductors

B2 - External Conductors, uncoated, Sea level to 3050m ( 10K ft.)

B3 - External Conductors, uncoated, over 3050m ( 10K Ft.)

B4 - External Conductors, coated with permanent polymer coating


Note: The IPC-2221 6.3 paragraph refers to insulation between conductors over the board surface and through the dielectric. I would guess this simplifies the spec writing... The dielectric actually has a 750V per mil insulation resistance perpendicular to the layers according to Mil-P-13949/4C for FR4 glass epoxy laminated materials.  So 1.3 mils of material perpendicular to the layers would net you 1KV insulation resistance. top to bottom or internal layer to layer. Always give yourself some margin... The back side of the copper foil is rough and can be 'spiked' on the laminated side for adhesion... those spikes and cause the spacing to be less than the minimum target spacing you require when laminated. Also there can be bubbles or voids in the materials that could occur right between your two high voltage conductors... Unless you are trying to mimic a capacitance plane pair, there is little or no reason to have the high voltage lines that close. You don't want a short to occur internally in the board. Give yourself a buffer of at least a couple of layers of prepreg on internal layers.


The chart for 500v for the .00012 per volt section indicates the 500V spacing is .030. Now if you divide .030 by 500v you get .00006 per volt.


So I would say that the .00012 number is not the linear multiplier used to get to the 500V spacing.


They did intend though that you figure out the difference between the 500v and the voltage you are targeting above 500v and add .00012 per volt above 500v to the 500v spacing which is .030.


So for internal or polymer coated traces, at 1000 volts you would need to add .06 to the .03 to get .09 spacing... that's between conductors on the same layer.


For external uncoated traces below 10k ft ASL the spacing is .1 at 500v plus 500v times .0002 which is .1 so you would be at .200 mils for 1Kv.


Q: What does it mean when they say that the PCB material must meet UL94 V-0 or better?


A: This is taken from the Boedeker plastics website, see below...


94V Vertical Burning Test

This test includes three classifications – 94V-0, 94V-1 and 94V-2 – and would typically be acceptable for portable, unattended, intermittent-duty, household-use appliances (i.e., coffee makers). Which classification applies to a particular application depends on many factors, including:

bulletSize and thickness of part.
bulletDistance from uninsulated live parts.
bulletHot wire ignition.
bulletHigh current arc ignition.
bulletHigh voltage arc tracking rate.

This test uses a ½" x 5" specimen which is held at one end in the vertical position (see Fig. 3.1). A burner flame is applied to the free end of the specimen for two 10 second intervals separated by the time it takes for flaming combustion to cease after the first application. Two sets of 5 specimens are tested. The following are recorded for each specimen:

bulletDuration of flaming combustion after the first burner flame application.
bulletDuration of flaming combustion after second burner flame application.
bulletDuration of glowing combustion after second burner flame application.
bulletWhether or not flaming drips ignite cotton placed below specimen.
bulletWhether or not specimen burns up to holding clamp.

Table 1. Material Classification

  Criteria Conditions 94V-0 94V-1 94V-2
  Total flaming combustion for each specimen less than or equal to 10 sec less than or equal to 30 sec less than or equal to 30 sec
  Total flaming combustion for all 5 specimens of any set less than or equal to 50 sec less than or equal to 250 sec less than or equal to 250 sec
  Flaming and glowing combustion for each specimen after second burner flame application less than or equal to 30 sec less than or equal to 60 sec less than or equal to 60 sec
  Cotton ignited by flaming drips from any specimen NO NO YES
  Glowing or flaming combustion of any specimen to holding clamp NO NO NO

UL94 Figure 3.1 -- Vertical Burning Test for 94V and 94VTM Classifications












Hit Counter

Copyright © 2004 PCB Wizards.COM