I want to interface the WISMO218 GPRS chip with an antenna. The antenna lines on the PCB board have to be very specific, otherwise the system won't work. I have uploaded the part of the datasheet that refers to the antenna.

I am going to use an antenna and and a coaxial jack as seen at the links below:



My PCB board is of the type "FR-4", Copper thickness: 35um, Height of the board: 1.6mm

I would like to interface the antenna on the same way as seen at the datasheet.

How can I calculate the line width, and the distance from the ground planes in order to achieve the 50 ohms impedance? Only the top layer is going to used for the antenna.

Remember that this operates in high frequencies.

Thanks in advance

The data sheet states the following:

First part datasheet

Second part datasheet


1 Answer 1


It's called a Coplanar Waveguide With Ground. To find impedance, here is a calculator.

This is a cross-section through the line. The red is the RF track, the blue is ground. The dotted blue lines are vias, you should put them every 5 to 10 mm along the sides of the ground.
CPW Ground

If I assume you have a two-layer board,
Er= 4.2 (good guess for FR4 if you don't know better)
Board= 1.5 mm
Track= 2.1 mm
Gap = 0.5 mm

You will have a 50 ohm line. There will be other solutions with wider tracks.

Deviations of 10% from 50 Ohms will not matter in this application. But as they say in the datasheet, keep the track short! If I recall correctly, at 900 MHz, the attenuation is 3 dB in just 5 or 10 cm. 1800 MHz is be worse.

Don't forget to put plenty of vias down the sides of the CPW, to the ground plane underneath.

  • \$\begingroup\$ Thank you for your answer. I have designed the PCB board with the WISMO chip and with the antenna at EAGLE. In order to do this, I have calculated the impedance using the values as seen at the picture. !Calculations. Then I designed the antenna part as seen at the picture below. !Antenna PCB. The whole circuit looks like this !whole PCB board. What do you think? Does this look right to you? \$\endgroup\$ Commented Apr 14, 2015 at 16:52
  • \$\begingroup\$ @DimitriosTorssøn The line looks good as designed. Perhaps put in two more vias right next to the module, either side of the line. Secondly, unless you have some RF test equipment, you should follow the manufacturer's recommendations for the antenna mounting quite carefully. To me it looks too close to the GSM module, and maybe too far from the edge of the board. And with an on-board antenna, the corners of the board will have some RF voltages on them. I don't see any filters or bypass caps on the lines leaving the board, they might be good, especially if you are planning to use it for voice. \$\endgroup\$
    – tomnexus
    Commented Apr 14, 2015 at 18:30
  • \$\begingroup\$ I use that system in order to send only simple SMS text messages. I am in doubt about how exactly antenna should be mounted. In the data sheet, it says that it should be mounted at the edge of the board (and they tried it to an FR-4 board. This type of board is way too thick for that PCB connector to fit there. Do you have any suggestions? It seems like that I have to create manually some pockets on the PCB board. I do not see a way to do that in EAGLE. Do you know if there is a way in EAGLE to do that? or maybe do you know an other way? (I am only a 2nd semester student BTW :-( ) \$\endgroup\$ Commented Apr 14, 2015 at 18:55
  • \$\begingroup\$ Ah ok, I'm sorry I didn't read, I assumed you were using a chip antenna. No that connector won't work, it needs to slip over the edge of a board. This type of connector is what you need. Five thru plated holes. Keep the same sort of clearance as you had from track to ground, under the connector. Keep the pad on the bottom very small. Notice that the connector pins have little shoulders, so the body doesn't touch the track; if you get one without these, solder it 0.5 mm up. \$\endgroup\$
    – tomnexus
    Commented Apr 14, 2015 at 19:55
  • \$\begingroup\$ We have not the option of using an other connector since our teachers ordered that one because it was cheaper... But if we manage to create the pockets and solder it at the edge of the board, will it work then? Why you say that it won't work at all? what is wrong with the connector apart from the part that it does not fit the FR 4 board and that we have to find a way to create pockets so it can fit? \$\endgroup\$ Commented Apr 14, 2015 at 20:02

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.