Ground plane for a GSM spring antenna with 4 layer PCB

Question

We are looking to build a 2G GSM based device with a helical spring antenna like this.

The work in progress layout is as shown below:

We are using a 4 layer PCB with top layer for signal, inner 1 layer for GND, inner 2 layer for power and bottom layer for signal. The antenna would be mounted on bottom layer.

Questions I have are

1. Is it better to use a microstrip or a co-planar wave guide or a co-planar wave guide with ground plane to connect the antenna with a 50 Ohm line from the GSM module?
2. For a near omni directional antenna pattern, what should the copper pour look like around the antenna in the various layers? Should I cover the entire PCB with copper pour or should I cover only near the line connecting the antenna? If later, to how much distance from the line connecting the antenna?
3. For Q1, which calculator would you recommend I use for figuring out the line width?
4. In these calculators the height from GND plane would be the distance between the top layer and the first inner layer with GND plane according to the stack-up, right?

Thanks!

Answer 1

1. Microstrip is probably easiest, i.e. a continuous ground plane on one layer, and the RF signal-carrying strip on another layer. No other conductors above the signal line, nor between the signal line and ground plane.

2. That "spring" antenna operates in a way that might be unexpected for antenna novices. I regard it as a bent, top-loaded monopole. The strongest radiation will occur from the straight, upright section, which has the highest RF current. The long helically-wound portion mainly serves to make the antenna resonant. Being a monopole, a ground plane is essential to its performance, and ideally, the ground plane should extend at least 1/4 wavelength in all directions from the feedpoint. But GSM operates in both the 850-900 MHz and 1800-1900 MHz ranges. You'd have to have about 8 cm of ground plane in all directions to satisfy that lower frequency range. Even with that, the bent nature of this antenna will make it impossible to get perfect omnidirectionality, or pure vertical polarization either.

3. There are plenty of calculators on the web. I found this one to be OK.

4. Yes, you have the right idea for microstrip "height". You'll also need to enter the dielectric constant of your PCB material.

Answer 2

Adding a couple of points to the answer by Mark Leavitt (not enough rep to comment).

I am assuming that the layer that is visible is the bottom signal layer.

1. Microstrip is the easiest but since there's a power layer between this signal layer and the ground layer, this is not strictly a microstrip line any longer. If using microstrip, I would recommend using the top signal layer for the line and connecting to the antenna with a through hole via. You will have to consider the via length in the impedance match. If using the bottom signal layer, I would recommend a CPWG.
2. Monopoles do not have an omnidirectional pattern - see image and notes here. Assuming you want something like this, yes you will need a large ground plane. For this PCB I would expect to see skewing.
3. LineCalc from Agilent/Keysight is the gold standard. TX-Line is pretty good too.
4. Yes, layer thickness is to nearest full ground plane.

Some good points to consider in here.