+ Post New Thread
Results 1 to 15 of 15
  1. #1
    Newbie level 2
    Points: 27, Level: 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?

  2. #2
    Super Moderator
    Points: 78,487, Level: 68
    Achievements:
    7 years registered
    Awards:
    Most Frequent Poster 3rd Helpful Member

    Join Date
    Apr 2014
    Posts
    15,925
    Helped
    3610 / 3610
    Points
    78,487
    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.

    Klaus
    Please donīt contact me via PM, because there is no time to respond to them. No friend requests. Thank you.



    •   AltAdvertisement

        
       

  3. #3
    Advanced Member level 3
    Points: 4,877, Level: 16

    Join Date
    Nov 2013
    Posts
    723
    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/



  4. #4
    Super Moderator
    Points: 261,221, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    45,641
    Helped
    13878 / 13878
    Points
    261,221
    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.



  5. #5
    Advanced Member level 5
    Points: 34,034, Level: 45

    Join Date
    Oct 2001
    Posts
    4,856
    Helped
    1444 / 1444
    Points
    34,034
    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.

  6. #6
    Super Moderator
    Points: 261,221, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    45,641
    Helped
    13878 / 13878
    Points
    261,221
    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.



  7. #7
    Advanced Member level 5
    Points: 14,284, Level: 28

    Join Date
    Apr 2014
    Posts
    2,239
    Helped
    890 / 890
    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...stic-impedance



    •   AltAdvertisement

        
       

  8. #8
    Newbie level 2
    Points: 27, Level: 1

    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?



  9. #9
    Advanced Member level 5
    Points: 34,834, Level: 45
    Achievements:
    7 years registered Created Blog entry Created Album pictures
    SunnySkyguy's Avatar
    Join Date
    Sep 2007
    Location
    Richmond Hill, ON, Canada
    Posts
    6,729
    Helped
    1679 / 1679
    Points
    34,834
    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 ohms
    Last 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



  10. #10
    Advanced Member level 5
    Points: 34,034, Level: 45

    Join Date
    Oct 2001
    Posts
    4,856
    Helped
    1444 / 1444
    Points
    34,034
    Level
    45

    Re: Microstrip line and ground on same layer

    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.



  11. #11
    Advanced Member level 5
    Points: 34,834, Level: 45
    Achievements:
    7 years registered Created Blog entry Created Album pictures
    SunnySkyguy's Avatar
    Join Date
    Sep 2007
    Location
    Richmond Hill, ON, Canada
    Posts
    6,729
    Helped
    1679 / 1679
    Points
    34,834
    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 counter-intuitive.

    -Click image for larger version. 

Name:	strip-coplanar Zo.jpg 
Views:	7 
Size:	350.8 KB 
ID:	155919

    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



  12. #12
    Advanced Member level 5
    Points: 14,284, Level: 28

    Join Date
    Apr 2014
    Posts
    2,239
    Helped
    890 / 890
    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.



  13. #13
    Advanced Member level 5
    Points: 34,386, Level: 45

    Join Date
    Dec 2004
    Location
    New England, USA
    Posts
    4,823
    Helped
    1350 / 1350
    Points
    34,386
    Level
    45

    Re: Microstrip line and ground on same layer

    Quote Originally Posted by vfone View Post
    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.
    i was going to say three line widths away



    •   AltAdvertisement

        
       

  14. #14
    Super Moderator
    Points: 261,221, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    45,641
    Helped
    13878 / 13878
    Points
    261,221
    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.



  15. #15
    Advanced Member level 4
    Points: 6,871, Level: 19
    Achievements:
    7 years registered

    Join Date
    Jun 2012
    Location
    Edmonton, Canada
    Posts
    1,057
    Helped
    301 / 301
    Points
    6,871
    Level
    19

    Re: Microstrip line and ground on same layer

    Quote Originally Posted by WengCheng View Post
    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.
    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.



--[[ ]]--