Connect with us

Question regarding (RF) microstrip design

Discussion in 'Electronic Design' started by Jasper Keuning, Aug 20, 2007.

Scroll to continue with content
  1. Hello Everyone,

    I had some questions regarding microstrip (or Coplanar waveguide CPW)
    design. Since it's my first project using a RF microstrip I was wondering if
    you could give me some advice on this subject.

    My design incorporates a GSM modem. Earlier designs had the MC35i from
    siemens, this modem had an easy accessible RF connector where the antenna
    connector was placed on directly. Now, the design needs to be reduced in
    size and a smaller modem is to be used. My choice will be the Enfora Enabler
    IIIG [1] or the Telit GE864 [2]. Where the enfora has an RF connector, it's
    almost impossible to use this for a direct connection to the antenna
    connector. The Telit is a BGA module and has no RF connector at all.

    The idea of my microstrip is to simply make a connection for the antenna on
    my PCB which can easily be reached. Basically this comes down to getting the
    RF from under the modem, to an 'open space' on the PCB. I think it will be
    no longer then 10mm. I will be working with a 4 layer board [3] and my
    prototype PCBs will come from Eurocitcircuits. I have used a piece of
    software called TXLine [4] to do some calculations for me on the CPW. I want
    to route the RF on the top layer (enclosed by GND Copper) and the layer(s)
    below will be ground as well. I am neglecting the effects of the substrate
    and copper below the 2nd layer. I chose the Gap between strip and copper to
    be 0.2mm and the program calculated for me, that in order to get a 50Ohm
    impedance, the width of the strip should be 0.66mm. A RF connector will be
    placed on the end of the strip. The frequencies on the strip will be GSM900
    and GSM1800 (and perhaps later GSM850 and 1900).

    How critical is making such a strip? Is my approach sufficient to stay out
    of trouble? Or am I overlooking things? I have never used RF on a board, and
    rather not blow up my modems or degrade the output power. Any advice is

    Thanks in advance!

    Jasper Keuning



    [3] From top to bottom:

    Cu (17u), Prepreg (100u), Prepreg (200u), Prepreg (200u),

    Cu (17u), Core (550u) Cu(17u),

    Prepreg (200u), Prepreg (200u), Prepreg (100u), Cu(17). (all Material is

  2. colin

    colin Guest

    the shorter it is the better, less than 1/4 wavelength the effects of
    mismatch start to become less significant.

    Colin =^.^=
  3. John Larkin

    John Larkin Guest

    Sounds fine to me. It's so short that things won't be critical, and
    pcb losses will be very small.

    Just be careful to keep any emi sources (uP busses, switching regs,
    things like that) as far away as feasible.

  4. Steve

    Steve Guest

    Decide on the most advantageous trace widths (and gaps and ground floods)
    before setting the layer spacings. You want to have trace widths that are a
    convenient size for the board features, rather than setting the board layer
    spacings first and then living with the required trace widths. For instance,
    set trace width to be same as any desired series coupling caps, or fine
    pitch pin widths, or same as an SMD connector launch pad. In your case, if
    the antenna line has to pass under the chip, pick a width that allows plenty
    of ground flood on both sides, at the points where you have to pass between
    pins or other routing obstructions. (Esp. since you want to use CPW, where
    the adjacent grounds are critical. Microstrip avoids the top side ground
    flood issues in routing) You'll probably want to look at all these things
    before committing to a final width and gap. And its always a judgment call
    as to which trace width will produce fewest mismatches with all the various
    sized interfaces along the path. I personally like to match to series
    elements and then the launch and termination points get some sort of
    transition to resolve the size mismatch.

    If you can keep RF on only one side, make the opposite side about the same
    thickness and take up all the extra thickness in the center, to get your
    nominal desired overall thickness. This yields balanced fabrication, which
    minimizes warpage.

  5. Robert

    Robert Guest

    As John said, the short length will make most issues less important but you
    might want to talk to your FAB house for what they recommend for the
    controlled impedance lines.

    They know their materials and process and if you've been using approximate
    values in your calc they can get you closer.

  6. Tom Bruhns

    Tom Bruhns Guest

    The wavelength of 1900MHz is about 160 millimeters in freespace, about
    half that in FR4 type material. Your 10mm length will be about 45
    electrical degrees, which starts to become significant. Keep things
    as short as you reasonably can, because short lengths are much less
    able to do significant impedance translations than long, if the line
    impedance isn't what you wanted it to be.

    On the plus side, the impedance of the line depends on the dimensions
    and the permittivity of the dielectric, but varies as 1/
    sqrt(permittivity) and as log of dimensions, so small errors in either
    don't have catastrophic effects. For example, 45 degrees of 60 ohm
    line transforms 50 ohms to 59+j11, and 45 degrees of 40 ohm line
    transforms 50 to 39-j9. If you use either of those to connect a 50
    ohm load to a 50 ohm source, you'll suffer less than a whopping 0.12dB
    transmission loss because of the mismatch (that's in addition to any
    line loss).

    It seems to be generally misunderstood how LITTLE effect there is on
    power transfer if impedances are mismatched, within moderation. A 2:1
    SWR (25 ohm or 100 ohm load on a 50 ohm source, for example) results
    in a lowering of the power dissipated in the load by only 1/9, about
    11% or 0.51dB. A 1.5:1 SWR results in just 4% reduced power, about

    You can play "what-ifs" about this to your heart's content if you use
    a program like the free RFSim99, which includes not only the ability
    to simulate your circuit very easily, but also a simple microstrip
    calculator (though not your co-planar w/ground plane design). It also
    includes an RF calculator several tabs, one of which will take return
    loss, SWR, transmission loss or reflection coefficient as input and
    tell you the other three of that set.

  7. Chris Jones

    Chris Jones Guest

    Make sure that if you have several layers that are all supposed to be
    "ground" that you tie them together with LOTS of vias. Here's a relevant

  8. <snap>

    Thank you all for your response!
    What I got from them was:

    Keep the strip as short as possible.

    Make sure all grounds around the strip are really "Groundy", not being
    afraid of putting lots of via's in.

    Try to keep noisy traces such as powerlines from switchers and High speed IO
    as far as possible from the strip.

    Choose a trace width that best suits my design, and go from that point with
    the complete design.

    I should not be too affraid of mismatch, a few ohms will hardly be noticed
    in terms of signal loss.

    There are free programs availible for me to simulate a strip design, and I
    should not be affraid to use them.

    I should ask my boardhouse for info/assistance on getting my impedance

    My strip is only ment to get the RF part from under the modem to a place I
    can put my RF connector, Because the modem has Ground and power connections
    near (<1.5mm) the antenna connection, my idea was that a CPW would shield my
    strip alot better then a microstrip design would.

    The issues posed in the Greentape poem [1], tell me to not place any via's
    at 1/2 or 1/4 wavelenght appart. Or have any "lose" copper around. Does this
    also apply to the surrounding groundplanes?

    I think I have sufficient info now to start my workh, and will first
    simulate my design. Again, thank you all very much!


  9. Chris Jones

    Chris Jones Guest

    If there is significant coupling from the RF trace to any other structures
    on the board then it would be safer to avoid resonances by making sure that
    the vias are significantly closer together than in the resonant structures
    in the poem. If you're really unlucky then the box in which the PCB is
    installed can also resonate, but at lower frequencies like 900MHz, it is
    not as likely to be a problem as with "real" microwaves. Sometimes you see
    resistive material attached to the inside of the metal casing for microwave
    equipment to damp these resonances, but I doubt you'll have any problem.

  10. Then I will place the via's as close as possible to each other,

    I will most likely use an ABS or PC enclosure, so I assume this has no or
    very little influence on the signal.


Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day