+ Post New Thread
Results 1 to 15 of 15

5th October 2019, 15:19 #1
 Join Date
 Oct 2019
 Posts
 3
 Helped
 0 / 0
 Points
 27
 Level
 1
Microstrip line and ground on same layer
Hello,
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?

5th October 2019, 21:14 #2
Awards:
 Join Date
 Apr 2014
 Posts
 15,932
 Helped
 3610 / 3610
 Points
 78,516
 Level
 68
Re: Microstrip line and ground on same layer
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.
KlausPlease don´t contact me via PM, because there is no time to respond to them. No friend requests. Thank you.

5th October 2019, 22:17 #3
 Join Date
 Nov 2013
 Posts
 724
 Helped
 193 / 193
 Points
 4,877
 Level
 16
Re: Microstrip line and ground on same layer
Are you talking about coplanar waveguide maybe? A lot of calculator available for it via browser.
"Try SCE to AUX." /John Aaron/

Advertisement

5th October 2019, 22:40 #4
 Join Date
 Jan 2008
 Location
 Bochum, Germany
 Posts
 45,661
 Helped
 13881 / 13881
 Points
 261,317
 Level
 100
Re: Microstrip line and ground on same layer
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.

6th October 2019, 13:29 #5
 Join Date
 Oct 2001
 Posts
 4,856
 Helped
 1444 / 1444
 Points
 34,042
 Level
 45
Re: Microstrip line and ground on same layer
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.
1 members found this post helpful.

6th October 2019, 15:29 #6
 Join Date
 Jan 2008
 Location
 Bochum, Germany
 Posts
 45,661
 Helped
 13881 / 13881
 Points
 261,317
 Level
 100
Re: Microstrip line and ground on same layer
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.

6th October 2019, 17:23 #7
 Join Date
 Apr 2014
 Posts
 2,239
 Helped
 894 / 894
 Points
 14,284
 Level
 28
Re: Microstrip line and ground on same layer
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...sticimpedance

Advertisement

7th October 2019, 08:15 #8
 Join Date
 Oct 2019
 Posts
 3
 Helped
 0 / 0
 Points
 27
 Level
 1
Re: Microstrip line and ground on same layer
Is there any paper or article about this rule of thumb?

7th October 2019, 09:03 #9
 Join Date
 Sep 2007
 Location
 Richmond Hill, ON, Canada
 Posts
 6,729
 Helped
 1679 / 1679
 Points
 34,857
 Level
 45
 Blog Entries
 7
Re: Microstrip line and ground on same layer
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 ohmsLast edited by SunnySkyguy; 7th October 2019 at 09:17.
A best design is easily achieved with good test specs™
A better question deserves a better answer. ™
... so include all your acceptance criteria ( values, % tolerance) and assumptions in your question or any design.
... Tony Stewart EE since 1975
 slightly north of Toronto

7th October 2019, 15:51 #10
 Join Date
 Oct 2001
 Posts
 4,856
 Helped
 1444 / 1444
 Points
 34,042
 Level
 45
Re: Microstrip line and ground on same layer
There is no reason to design a highimpedance 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 highimpedance line.

7th October 2019, 16:29 #11
 Join Date
 Sep 2007
 Location
 Richmond Hill, ON, Canada
 Posts
 6,729
 Helped
 1679 / 1679
 Points
 34,857
 Level
 45
 Blog Entries
 7
Re: Microstrip line and ground on same layer
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 counterintuitive.

yet either coplanar or Microstrip impedance alone is reduced with g or h respectively, but in tandem, coplanar waves reduce dielectric thickness wave currents.A best design is easily achieved with good test specs™
A better question deserves a better answer. ™
... so include all your acceptance criteria ( values, % tolerance) and assumptions in your question or any design.
... Tony Stewart EE since 1975
 slightly north of Toronto

7th October 2019, 17:12 #12
 Join Date
 Apr 2014
 Posts
 2,239
 Helped
 894 / 894
 Points
 14,284
 Level
 28
Re: Microstrip line and ground on same layer
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.

Advertisement

10th October 2019, 12:09 #13
 Join Date
 Dec 2004
 Location
 New England, USA
 Posts
 4,823
 Helped
 1350 / 1350
 Points
 34,386
 Level
 45

10th October 2019, 12:40 #14
 Join Date
 Jan 2008
 Location
 Bochum, Germany
 Posts
 45,661
 Helped
 13881 / 13881
 Points
 261,317
 Level
 100
Re: Microstrip line and ground on same layer
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.

11th October 2019, 15:27 #15
 Join Date
 Jun 2012
 Location
 Edmonton, Canada
 Posts
 1,057
 Helped
 301 / 301
 Points
 6,871
 Level
 19
+ Post New Thread
Please login