Re: Strip line
Usage of such a rule may lead to a problem. There is well known rules that distance between via should be approximately equal to the width of the stripline. Let’s say you have about 3 Ghz frequency signals and stripline on substrate with 3.7 dielectric constant, which may be a very popular for this frequency Nelco 4000-13 material. In this case actual wavelength will be c/((sqrEr)*F)=51.95mm, roughly 52mm. When you chose the smallest 1/20 via spacing it gives about 52/20=2.6mm via pitch. 50 Ohm stripline on Nelco 4000-13 59mils thick substrate (again, very popular thickness) will require about 29mils trace width. Let consider you use via 15 mils diameter (this is the less expensive in PCB production number). In such a case you may chose two via diameter spacing of 30 mils and it should be okay and it is practically match the striplane width. But if you chose to have the via spacing to be 1/20th of wavelength or 2.6 mm, which is more than 102 mils, you will end up with via spacing about 3.5 times more than your stripline width. This is the problem. For less thick substrate this problem will be even worse. Azulikeit is right when talking about EM solver, so if have such a program you may simulate your particular situation and compare the return currents with currents between via. If latter is more than 5-to-10 % of return currents you need to decrease via pitch. Moreover, often you have unwanted higher frequency currents though transmission line and you do not want they couple with other part of the circuit. In case you probably will need the second raw of the via, but it is the different story.
Best regards,
RF-OM