Implement limits and warnings in pcb calculator

[Mishka]

Hi,

I've faced an issue when estimating a coplanar waveguide using the PCB Calculator. The PCB Calc produces slightly different results when compared to http://wcalc.sourceforge.net and AppCad. Looks like math precision issue.

Although resulting impedance value doesn't seem differ too much (it's like 47 Ohm in PCB Calc vs 50 Ohm in WCalc), but it makes significant difference when deriving track width and especially metal spacing on very thin substrates like polyimide.

Screenshots follow.

Thanks!

[Michael Kavanagh (michaelkavanagh)]

Please copy the full version information from About KiCad -> Copy Version Info.

[Seth Hillbrand (sethh)]

@Mishka- What leads you to believe that our calculation is incorrect and wcalc is correct?

[Mishka (mike-volokhov)]

Version: (5.1.4-0), release build
Libraries:
    wxWidgets 3.0.4
    libcurl/7.54.0 LibreSSL/2.0.20 zlib/1.2.11 nghttp2/1.24.0
Platform: Mac OS X (Darwin 17.7.0 x86_64), 64 bit, Little endian, wxMac
Build Info:
    wxWidgets: 3.0.4 (wchar_t,STL containers,compatible with 2.8)
    Boost: 1.69.0
    OpenCASCADE Community Edition: 6.9.1
    Curl: 7.54.0
    Compiler: Clang 9.0.0 with C++ ABI 1002

Build settings:
    USE_WX_GRAPHICS_CONTEXT=ON
    USE_WX_OVERLAY=ON
    KICAD_SCRIPTING=ON
    KICAD_SCRIPTING_MODULES=ON
    KICAD_SCRIPTING_PYTHON3=OFF
    KICAD_SCRIPTING_WXPYTHON=ON
    KICAD_SCRIPTING_WXPYTHON_PHOENIX=OFF
    KICAD_SCRIPTING_ACTION_MENU=ON
    BUILD_GITHUB_PLUGIN=ON
    KICAD_USE_OCE=ON
    KICAD_USE_OCC=OFF
    KICAD_SPICE=ON

[Mishka (mike-volokhov)]

@Seth, to be honest I don't know is PCB Calc does it wrong. But please note, the AppCAD shows is even further (I've attached screenshot for spacing calculation).

Such, for polyimide substrate 0.065 mm thick, 0.035 mm copper, 0.17 mm feed line, calculated top copper spacing values:

- AppCAD: 0.25 mm
- WCalc: 0.54 mm
- KiCad: 2.19 mm

Taking in account so huge difference it would be nice to know for sure which one is wrong. Perhaps factory impedance control could answer it.

[David Pearce (halzia)]

When you increase coplanar waveguide spacing "S", wcalc seems to give a result close to the microstrip solution, as you would hope.
KiCad gives a much larger difference.

[Seth Hillbrand (sethh)]

We don't include uncertainty values and limits but if we did, this would be more clear.

The grounded CPW is, in fact, two calculations: the CPW and the microstrip. The controlling relationship is the width of the microstrip line to the height above the ground plane. This equation is only valid from 0.5 < W/H < 2.0.

At ratios of much less than 0.5, the CPW calculation is dominant and should be used instead. At ratios much greater than 2, the stripline calculation is dominant and should be used instead.

At intermediate ratios, there is no valid, analytic solution and it must be simulated in FEM[1].

[1] Analytical formulas for coplanar lines in hybrid and monolithic MICs, G. Ghione ; C. Naldi, 1984

[KiCad Janitor (kicad-janitor)]

KiCad bug tracker has moved to Gitlab. This report is now available here: https://gitlab.com/kicad/code/kicad/-/issues/2524