Microstrip line and ground on same layer
I'm looking for an equation to calculate the distance between a microstip line and a ground plane on the same layer, so that the ground plance won't effect the microstrip line.
Is there any rule of thumb to calculate the distance?
Hi,
Call me pedantic, but in my eyes:
* a microstrip without a true GND plane is no microstrop.
* a GND plane on the same layer than signal is no true GND plane
For HF you really need a solid GND plane without splits, otherwise you get jumps in impedance and/or not correct impedance at all.
Klaus
Are you talking about coplanar waveguide maybe? A lot of calculator available for it via browser.
I understand that you are talking about coplanar waveguide with ground. A calculator can tell what's the minimal separation to get less than x % impedance reduction. Or utilize the lateral ground to make the microstrip smaller.
The rule of thumb that you ask for is that the ground plane on the same layer should be at a distance greater than 1.5 x width_of_the_line.
For example if the width of the microstrip line is 1mm the distance to the nearby ground plane should be greater than 1.5mm, if you want that the microstrip line do not be affected by the ground plane.
The rule of thumb applies if line width is > than substrate height. If you are designing a high impedance microstrip, this may be not the case.
In addition to what was posted above, you can check side ground distance here:
https://chemandy.com/calculators/cop...calculator.htm
https://www.edn.com/design/analog/44...stic-impedance
Is there any paper or article about this rule of thumb?
better to use s/w http://www.saturnpcb.com/?download=&...7.08_Setup.exe
then consider geometric ratios of w(width),coplanar gnd g(gap), h height on FR4 eg consider stripline w/h=1 Zo=63 ohms but with coplanar gnd tracks with g and w/h/g =1 same , then Zo rises to 66 Ohms or +5%
or w=5 mil , h=3, g=3 , Zo lowers to 51 ohms
There is no reason to design a high-impedance microstrip line with nearby ground on the same layer, because any nearby ground will decrease the impedance of the line, and you will not have anymore a high-impedance line.
Coplanar grd tracks actually increase Zo of Microstrip lightly by diverting the coupling. But there exists a ratio of w:h:g where coplanar gap has no effect. At first this seemed counter-intuitive.
-
yet either coplanar or Microstrip impedance alone is reduced with g or h respectively, but in tandem, coplanar waves reduce dielectric thickness wave currents.
Why have you chosen substrate thickness in your example as 3mils? That's somewhat unusual. Likewise, 2mils gap is rather extreme.
With "normal" dimensions, the effect caused by side ground that I see in simulation is simply an increase in shunt capacitance -> decrease of line impedance.
i was going to say three line widths away
Saturn PCB is exclusive by calculating an increased impedance with additional coplanar ground. Other professional tools like Polar Instruments Si6000 don't.
I prefer not to believe the results.
You can check Saturn plausibility by varying the coplanar ground separation. The impedance should converge against microstrip value for gap >> substrate height.
I believe what you're looking to do is match the characteristic impedance of the microstrip with that of the CPW-like mode of a conductor-backed CPW. You can find approximate solutions in works like Simons.