Pcb realization info

[Giuseppe]

Hi I'm making a pcb with a radio module HC-12 100mW Max of 433Mhz power and a Pic.
I initially placed both the pic and hc-12 on the top of the board.
Then later thinking about it I thought that RF could create problems on the inputs of the pic.
At this point, is it better for you to put hc-12 on the top and the pic with the various entrance tracks on the botton?

[Mapo]

Hi Giuseppe,
I made various PCBs with HM-TRP 868 without problems and the PIC, the radio module and all the components in the same side.

[Giuseppe]

Hello Mappa
I looked for the module you used for your project is a 868Mhz 100mW of power. Searching for the images in google came out a module welded on a pcb that has around it like a perimeter of the screen, I think you have also used this system of realization?
Also in your project does the microcontroller you used also have ports set as input?
I also wanted to ask you if you are using your module at maximum 100mW power?
Thank you

[Craig]

Hi Guiseppe

I have done a lot of designs using RFM 100Mw and 1Watt Devices and I have never had a problem with putting all the components on the same side and having a good ground plane (2 Layer PCB). I have obviously placed the RF at the Edge of the PCB and the PIC further down with a good ground plane between. It is always very good practice to place as many VIAS through the PCB layers around the Antennae Path From Top Layer Ground plane area to your bottom Ground Plane following on both sides of the Antennae plane and keeping the Antennae Trace as Short as possible and @ 50_Ohms.

See MICHAEL OSSMANN Simple RF Circuit Design - Video it is very well presented.

https://www.youtube.com/watch?v=TnRn3Kn_aXg

Regards
Craig

[charliecoutas]

I have a PCB where the coiled aerial for the HC-12 lies along the 18F26K22 28 pin DIP. No problem.

Charlie

[Mapo]

Ciao Giuseppe
in the project I did not use any particular shielding devices, the module needs a good decoupling, it works at 3.3v, and I use it at maximum power. Only advice, at maximum power you must use a real antenna, with a connector mounted on a metal base, otherwise the high RF blocks the antenna switch.
I am attaching a part of the pcb

[Giuseppe]

Hello Mappa
I saw your pcb. By bringing the antenna away from the pcb with the coaxial cable, you have reduced any problems due to RF.
Now on my 2-layer pcb I used several connection ways with 0.3mm holes, distributing them several on the ends of the pcb but also inside. I put about 60 connecting ways between the 2 faces. Very informative the video of Craig.
The distance between the channels must be at most 1/10 of the wavelength of the frequency used.
Now from what I have read usually using only 2 faces on one you have to put the ground plane and on the other the tracks.
In my case I was unable to put all the tracks on one side. On the side exposed to rf I put the power tracks and the outputs of the mcu while underneath I placed mcu more input tracks. Let's see how the system behaves I'll let you know.
Thanks again everyone.

[John Drew]

To minimise local RF and maximise signal you should make the board traces to the antenna socket either very short or better create a transmission line of the same value as the output impedance and the antenna- usually 50 ohms but not always. Check the data sheets.

A transmission stripline is built using a trace of a certain width surrounded by ground plane top and bottom. Thickness and type of board are part of the calculations.
Alternatively, run a length of very thin 50 ohm coax to the socket.

If you don't need the absolutely best results just do as suggested by previous posters and keep your trace short and at least 2mm wide with ground plane either side.

RF is tricky.
Cheers
John

[JonW]

If you are using Fr4 as a dielectric then try to use a controlled impedance pcb stackup, they are cheap and perform very well.  Don't read too much into adding lots of vias as its not needed unless you need good isolation to another adjacent RF circuits or are not using microstrip.  If you start varying grounding and mixing the transmission line modes then you run the risk of seriously impacting the return loss and your 100mW can easily be 10mW or less destroying your EIRP or RX sensitivity.
 As the substrate thickness increases the trace width increases hence why many controlled impedance boards use a thinner conductor to gnd spacing to realise thinner RF traces that are good for single ended and differential tracing over good distances without destroying return loss and introducing ripple etc.  Most controlled impedance designs use a layer thickness of around 0.2mm to 0.4mm for Fr4 (dk around 4.7) for microstrip. this 0.2 mm layer thickness will yield a 50R trace width of 0.35mm and the Quasi-TEM modes will be well balanced, giving optimal return loss and low loss easily beyond 10GHz.  I have used Fr4 in mass production beyond 15GHz with 3 GHz bandwidths or more with no problems using 0.2 to 0.3mm layer thickness. If you increase the substrate thickness to say 0.8mm on FR4 then a 50R line (for microstrip) needs to be 1.4mm and for 1.6mm layer thickness it rises to 2.8mm for 50R, at this thickness the  Width to Height ratio introduces many issues >500MHz.  If you start placing ground layers onto the top layer and via stitching then the impedance will again change throughout the design and you may again see poor return losses as your circuit interface changes from Microstrip to Coax to Coplanar.  For basic RF sub GHz stick to microstrip and controlled impedance substrate stack-ups or keep the substrate below 0.5mm. 

What you have done using the Coax is a good solution and works well into the GHz range, also consider using UFL connectors as these are very low cost and work well.  If you want to use a pin as an RF feedthrough then you need to again be careful as this is essentially coax so careful consideration is needed for the interface to keep the return loss to better than 10dB. 

J

[JonW]

For low volume this 7628 controlled impedance stack is hard to beat for most designs. 
https://cart.jlcpcb.com/impedance
https://cart.jlcpcb.com/impedanceCalculation

If you need to use printed filters and antennas then you really need a substrate with a specified and tight tolerance dielectric constant (DK).  The Rogers or Sheng Ye substrates are great for this and we produce millions of LNB using these substrates.  You can get access to the materials in very low volumes now and some of the fast turn PCB houses in China have these laminates as stock items.  If you need anymore help then PM me and I can help you out and run some EM simulations for you so you can get the most from your RF circuits

J