Saying FR4 is like saying i used wood. What wood ? oak ? spruce ? birch ? plywood ? osp ?
FR4 = Flame retardant class IV
It is NOT fiberglass-Resin. That is a common misconception. People call it that but if you use that in front of a pcb fabricator they will give you the eye-roll.
You need to know what is the material being used. Manufacturer and type. Some people will go , oh i used Rogers for my RF project. That is still saying "i used wood". Rogers has hundreds of different materials. So does Isola and anyone else.
ok, i used Isola 370HR. That's still saying you used wood.
What is the resin content ? 370HR material comes in different resin/fiberglass ratios.
ok, 63% resin. That's still wood.
What is the weave of the fiberglass ? Which fiberglass ?
Specifying : 1 need a board made from 17micron rolled copper foil with 4 sheets of 2116 glass 53% resin 370HR-type. Is a specification. the 2116 tells you the strand desnity, strand type and what kind of glass you are dealing with) If you are doing controlled impedance you will need some other numbers too, as well as the post-press thickness of the prepreg or core.
All that being said, there is a difference between creepage and clearance.
Creepage is the path along a surface. Clearance is the path in open air. There are rules for both. Rules that change based on contamination levels ( this can be dust , but this can also be ionic contamination that happens in the production process. ) They also change depending on surrounding air pressure ! ( height. a board for aircraft that goes above certain altitudes has different rules, and it's not uniform, there are classes based on actual height)
Then there is the soldermask. Soldermask can have a lower breakdown voltage than the raw pcb material. In some applications it is necessary to not put soldermask near high voltage components.
I'm working on a 800 volt battery system for an aircraft. We need to pick our materials VERY carefully. Especially because altitude is involved. Soldermask is a disaster.
the problem is we are working with surface mounted, small parts so copper features are relatively close together. we need a good isolator. So we need a material with a high CTI (comparative tracking index). Tracking is the creation of conductive paths (creating a track) on the surface and inside the pcb material based on temperature, aging, and other factors. The higher the CTI the longer the life of the board will be and the higher the voltage it can hold.
Your household "FR4" (i know, i know, but that's what people call it) has the WORST possible tracking index.
it can hold about 275 ~ 300 volts -edit- in the CTI test. -end edit-. Go above that and pathways will start forming that will start discoloring the material, reacting and create conductive paths.
clarification. the CTI is determined using a standardized test with electrodes spaced a certain distance apart and a "contaminant" dripped on the pcb material. its part of IEC 60601-1:2005 and the test is explained in IEC 60112.
The CTI has a direct impact on the creepage needed for a given voltage.
You can meet all the regulatory clearance and creepage rules you want : the board material itself will give out. Clearance and creepage only defines copper to copper spacing. it does NOT look at what happens in the pcb substrate itself. the CTI tells you how to adapt the creepage.
For 1 kilovolt you will need a material in PLC0 (Performance Level Category 0) >600VDC
The curing of the material is also important. Most fiberglass boards use the DICY process (dicyano-mumbojumbo i can never remeber how it is spelled, look it up) . Phenolic curing is much more resilient but more expensive.
Another enemy is the formation of CAF in the board. This is heavily dependent on the glass weave and resin content pre-curing. Another factor is how they drill the boards. Especially for larger holes that are made using endmills instead of a true drill , and how many strikes they allow per drill bit.
CAF is a conductive anodic filament. It grows between two points of different voltage. CAF can form with as little as 12 volt ! It grows along the glass strands and spreads like wildfire. it can form in seconds under the right conditions. boards can fail spectacularly. (Especially in big battery systems that have lot of "oomph" behind them. The filament forms, vaporizes, an arc forms and the arc carbonizes the resin even further. it's a cascade effect)
It always forms along the glass strands and in voids. So if you use a material with big glass strands with a loose weave and there is not enough resin you risk creating voids that do not fill during the lamination step. Drilling pcb material is a violent action. You are literally drilling through glass. The fibers shatter and it creates voids. Depending on the wear of the drill bit this gets worse. a new bit drill cleaner than a bit with 1000000 piercings behind it. your PCB fabricator knows this. If you specify this board is for high voltage you can pay a bit more to change drills more often.
The same is true for milled holes. Holes larger than 1.5 mm diameter are typically milled, not drilled. The collet in the spindle simply cannot hold anything larger than a 2mm shaft.(depending on the machine. 2mm used to be the limit , but newer machines are going to 1.5). It matters what kind of milling bit they use. again : if you tell the fabricator they can use dedicated milling bits for those holes. They may use a cheapo bit for the mounting holes but an expensive and newer bit for the important holes.
if the hole wall is damaged and the glass pretty broken up there is a risk for moisture entrapment during electroplating. Power up the board and you get spectacular CAf induced failures.
Copper : the surface finish of the copper matters too. Rough copper tends to arc easier than smotth rolled copper. Even the plating finish becomes important.
For high voltage : Panasonic R-3566D / R-3551D, Shengyi S1600
None of what i have stated here is the end-all. You need to do your own homework and understand that every board is different. What works for me may not work for you and vice-versa. If you build everything on teflon standoffs using long-body thru-hole parts in dead-bug construction then none of it matters. Air is a better insulator than the pcb material. (provided it's not 99% humity and dusty)
I'm just providing some insight into PCB materials and factors that are important when selecting materials and processes when dealing with high-voltage boards.
Home
Help
Search
Login
Register
