Question regarding (RF) microstrip design

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

Colin =^.^=

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.

John

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.

Steve

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.

Robert

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

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.

Cheers, Tom

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 poem:

Chris

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 right.

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 (

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.

Chris

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.

Thanks!

Jasper