impedance control

[Guest]

Is it possible to control the impedance for 2 sides board?
Because I though the impedance is calculated respect the uninterrupted ground layer, but now when I took a look at the impedance equations, I could not find the relation between plane and impedance (it is only a function of Trace Thickness W , Substrate Height H , Trace Width T and Substrate Dielectric Er).


P.S: right now I check your designiMX6 Rex module, and I saw that for impedance control on top and bottom layer, you used 2 ground layer on layer 2nd and 11th, and for the impedance control on layer 3rd and 10th you have 4 GND plane on layer 2nd-4th and 9th-11th.
So the impedance control is based on the UNINTERRUPTED GND plane???

Now, I am really confued

[Guest]

An Interesting question,
For the routing SD3_CLK_R you use 4 VIAs, and goes from 1st layer to 2nd layer (GND), then from 2nd to 3rd and then routed then use another VIA to goes to 2nd layer and again another VIA to 1st layer!!!!
Why you use a lot of via instead of going from 1 to 3 and then back

[robertferanec]

1) yes, you can have controlled impedance on 2 layer PCB, however the track dimensions (width and gap) are huge
2) yes, for controlled impedance you need uninterrupted planes (gnd, sometimes it can be also power)
3) because if you drill uVIAs from L1 to L3, the hole has to be bigger and you would lose advantage of small VIAs (check out VIA ratio - basically for uVIA the minimum hole size is as big as deep you drill - so deeper you drill bigger hole you need to use and bigger the uVIA will be)

[Guest]

1) yes, you can have controlled impedance on 2 layer PCB, however the track dimensions (width and gap) are huge
2) yes, for controlled impedance you need uninterrupted planes (gnd, sometimes it can be also power)
3) because if you drill uVIAs from L1 to L3, the hole has to be bigger and you would lose advantage of small VIAs (check out VIA ratio - basically for uVIA the minimum hole size is as big as deep you drill - so deeper you drill bigger hole you need to use and bigger the uVIA will be)

1)In case of 2 layer, what is the reference plane (assume on both top and bottom layer you routed)??
2) with intrrupted plane we can not control the impedance???
3) and the diameter of uVia should not be equals to D=(width_of_track)/pi (to keep the width of track constant)?

[robertferanec]

1) You need to have one layer solid GND - that is one of the reasons why 2 layer PCB is not good for PCB with controlled impedance (you only have 1 layer for signals)
2) It is safer to use use uninterrupted plane. It doesn't mean it can not be interrupted, but you would need to fully understand the currents flowing on your board and you would need to be sure, that you know where you can interrupt the plane.
3) you may want to double check with your PCB manufacturer what needs to be the minimum via ring width ( the copper between hole and edge of the via pad). Very often this depends on PCB manufacturer technology e.g. tolerance of the drilling machine. Usually, if VIA pad is bigger than track width I do not adjust track with to meet VIA pad size (so the VIA is bigger than track). If track is wider than VIA pad size, then very often I keep the track size when connecting VIA (so the track width is constant)

Have a look at some of our designs. You can download our open source boards from http://www.imx6rex.com/