How to use PCB Calculator for 50ohm transmission lines?

[rwgast_lowlevellogicdesin]

Im starting to learn kicad for EDA work and it has a nice little calculator built in for doing transmission lines. The problem is I dont know what all the parameters mean, I was hoping someone could help me.

Er = Dialectric Constant of PCB material
TanD = ?
Rho = ?
H = ?
H_t =?
T =?
Rough = ?
mu Rel S = ?
mu Rel C = ?

W = Width of Trace
L = Length of Trace

I have no idea what the ? parameters mean. For simplicity sake, if I wanted a 50mm long 50ohm and a 50mm long 100ohm trace on FR4 how would I figure that out? Im trying to make a patch array with matching network printed on rogers but I need to figure out how to make impeadence controlled traces before I can do anything.

[hendorog]

Im starting to learn kicad for EDA work and it has a nice little calculator built in for doing transmission lines. The problem is I dont know what all the parameters mean, I was hoping someone could help me.

Er = Dialectric Constant of PCB material
TanD = ?
Rho = ?
H = ?
H_t =?
T =?
Rough = ?
mu Rel S = ?
mu Rel C = ?

TanD is the lossyness of the dielectric - i.e. Rogers will have a smaller tand than FR4 and so there is lower loss in Rogers.
Rho is the conductivity of the conductor
H is the height of the dielectric - shown in the diagram in KiCad
H_t - not sure.
T is the conductor thickness - shown in diagram
Rough is a measure of the surface roughness of the conductor

I don't know what mu Rel S and mu Rel C are.

[T3sl4co1l]

Most conclusive would be to look up what paper it's from.  (Does it say?  Look in the help?  Ask a developer?  Check the source for comments?)

Offhand,
TanD (D is lowercase delta) = dielectric loss tangent (the dielectric isn't purely capacitive, but has an imaginary component as well; delta = real/imag)
rho = resistivity of copper
H = height (either copper trace thickness, or laminate thickness / height over ground plane)
H_t = height again?  Oh probably height of trace, and other one is over plane.
T = thickness?  Or maybe Trace width?
Rough = roughness parameter.  Must be a good model to have this?  Although I don't see frequency in here, which matters.  Maybe it's just a scalar for resistivity.
mu = ?  Would be permeability something or other, but who uses permeable materials?  Don't understand the Rel, S and C parts.

In any case, a very accurate calculator isn't very useful, as fabs are only 5% tolerance -- and that's if you pay them enough to use the best materials, and measure the results!  (Well, RF fabs are probably better than that, but...)

If you're doing controlled impedance for digital signaling, 20% (which is typical of most main line fabs) is good enough.

Note also that, if you have ground poured on the same layer, that reduces impedance.  That structure is called a coplanar waveguide.

Note further that, for standard fab widths (minimum trace width) and component pitches (maximum practical trace width), you can't get impedances very low on two layer board (even 0.8mm thickness).  A 50 ohm trace (CPW, minimum clearance) is about 1mm wide, on 1.6mm board.  Typical impedances are in the 100 ohm range (which, by the way, works very nicely with most CMOS logic; add a 47-100 ohm source termination resistor, and you're mostly good to go).  Controlled impedance designs, needing lower impedances (like 100 ohm diff pair), really have to be done on multilayer boards.

I like these calculators:
http://www.chemandy.com/calculators/calculator-index.htm
They include three different formulas for microstrip.  Take your pick.  Which one is best?  I refer you to my above discussion on fab accuracy.

Tim

[hendorog]

I found some comments in the code thanks to google:

H_t = Height of Box Top - i.e. how high above the trace is the top ground plane.
mu Rel S = Relative Permeability (mu) of Substrate
mu Rel C= Relative Permeability (mu) of Conductor

[rwgast_lowlevellogicdesin]

I guess what I really need is to find a tutorial on this stuff, im looking but nothing is helping fill in the blanks. The PCB calculator gives back ErEFF and losses. Im guessing the goal is to try and match ErEFF to ER as close as possible? I was thinking I could feed it frequency length and board properties then it would shoot back the correct width

[hendorog]

Disclaimer: Many people here understand this better than me, but hope this helps:

Er EFF means effective Er. Effective Er is the Er that results from having the fields below the conductor in the dielectric, and those above the conductor in Air. The Er of Air is 1, which is quite different from the Er of the dielectric (~4 for FR4).

The above is true for microstrip, which is a conductor sitting on the top of a dielectric with air above it. I think you cannot have an Er Eff the same as Er for microstrip.

For stripline the conductor is buried inside the dielectric, and so the Er Eff can be the same as the Er of the dielectric.

The dielectric losses are the result of what is entered in the tand field and the length of the conductor (L).
The conductor losses are the result of what is entered in the rho field and the length of the conductor (L).
Tinker with those two values and you should see the losses change - and they also change with frequency.

[T3sl4co1l]

e_eff will always be lesser than or equal to e_r, because it's the weighted average between air (e_r = 1) and the substrate.  Most of the time, e_eff is just for information.

Frequency and length only matter if you need to know the time delay, phase shift and scattering matrix.

If you are using a two-dimensional formula (i.e., one that does not use length), you only need to know impedance and velocity.  If the calculator does not provide velocity (or velocity factor), it's probably because you can use e_eff instead.  The velocity factor is simply: 1 / sqrt(e_r*mu_r).

Most formulas calculate impedance from width, because width is a boundary condition and it's easier to calculate forward from a boundary condition, than backwards to reconstruct it.  Anyway, once the function has been solved (numerically speaking), the reverse is trivial: apply a root finding algorithm to solve for X.  (The solution is by no means guaranteed, because root finding is a nontrivial process.  But useful solutions exist, so it's trivial in that respect.)

By the way, if you take velocity (if you get a dimensionless velocity factor, multiply by c to get velocity in m/s), and impedance, and multiply or divide them together, you happen to get units of capacitance or inductance per unit length.  These are precisely the capacitance or inductance per length that is characteristic of the transmission line.  If you are working with a low frequency circuit (i.e., where length is much less than the edge rate or 1/4 wave frequency), this also gives the equivalent capacitance (Z > Zo) or inductance (Z < Zo) of the trace!  Very handy for calculating trace inductances for power circuits.

Tim

[G0HZU]

I've always used the =TLINE= program from Eagleware (now Keysight) Genesys for stuff like this. Back in 1990 it was a DOS command line program and it cost $500 but it changed to a decent GUI a few years later. It was always very expensive but I think they bundle it as a licence free addon these days. It seems to run OK with or without a USB dongle fitted. Worth checking out!

It covers maybe 25 different Tline types and groups them as circular or rectangular and the image below is for classic microstrip. As you can see it provides some useful data. I think the original command line (MSDOS) version from 1990 was even more comprehensive but I haven't used it for a long time.

[rwgast_lowlevellogicdesin]

Ok I was thinking that getting a controlled 50ohm impeadence trace could only be one possible width depending on the length and board paramaters. What is the goal here when looking at kicad pcb calc? If I want a 50 ohm trace 50mm long, do I just enter in the parameters for the board material and then play with the width until I am satisfied with the amount of loss? At the moment I just want to cut a 50ohm trace on to a piece of rogers4003 thats about two inches long with an sma connector on both sides.... Thst sounds kind of pointless but its a good way to probe whats running through your coax. I thought this would be pretty simple.

[hendorog]

It is very simple once you know how:

1. Click the ... beside Er and select "RO4003" <- because you said you were using Rogers 4003
2. Click the ... beside TanD and select "RO4003" <- because you said you were using Rogers 4003
3. Enter the thickness of the PCB board in the H box
4. Put 50 in the Z0 box <- You said 50 ohms
5. Leave all of the other boxes alone.
6. Click Synthesize
7. The width of the trace you need is in the "W" box.

Now to see the loss do these extra steps:

8. Enter the length of the trace in the L box.
9. Enter the Frequency in the frequency box.
10. Click Analyze.
11. Read the loss figures. They will be tiny.

[rwgast_lowlevellogicdesin]

Awww ok thank you very much!!

One last quick question about finding PCB params the calc needs. I have a bunch of sheets of rogers with 2oz copper, this company is so nice they sent me a ton of sample I didn't ask for! There datasheets are very detailed and there support is super good! So basically hand cutting (these pcbs are so soft its like drawing with an exacto and using hardly any pressure to do it) or toner transferring impeadence controlled lines on to rogers without a board house is too easy! This stuff is awesome for prototyping anything really, but the price isn't right for that!

Besides Rogers I get PCB at TWO other places. #1 Radio Shack 4x3 double sided clad. Very hard definately needs dremel or saw to cut. I have always assumed it was FR4, it is about the same hardness as an OSHPark pcb. The thing is the packaging nor the website tells you if it is fr4 let alone  any of the other parameters, not even dialectic constant (I know fr4's constant can vary a lot based on manufacturer)

This is the RS PCB I buyhttps://www.radioshack.com/products/2-sided-copper-clad-pc-board

I could also use 50 ohm traces on the point to point stuff here and there. It would be easy enough to cut copper foil to the calculated size and lay it out over the veri board. Im sure I am not the only one who does home prototyping on RS Clad and there Point to Point boards. Can anyone verify they are at least fr4 (the traces dont have to be perfect but even a 60 ohm trace is better than no matching) and that I should use 4.6Er?
I also use PCB that is flexible and cut table with scissors. I buy it from a surplus sight called Electronics Gold Mine. It is made from glass epoxy and would be great for antenna on pcb type projects! Can I just get the dialectric constant for glass and wing from there if the company cant give me anymore parameters? Lastly I only use oshPark, At the moment (this will change when I have to go to 4 layer and rogers), and browsing there site I dont see any of these parameters, nor do I see anything stating there PCB is defiantly FR4  I would have thought a maker friendly more open flexible pcb service like OSHPark would list there PCB Parameters, I mean just in general im sure they see there fair share of hams design PCBs through them>

[hendorog]

You could roughly measure the Er by treating a double sided board as a capacitor and then doing the calcs for a parallel plate capacitor.

I wouldn't worry too much. When using cheap ingredients its best to just take a punt and build it. Then measure it and try again.