On Creating a schematic for an RFM69HW breakout board

Development Boards Arduino
1

n this post I discuss how I went about designing the schematic and choosing components.

http://bitknitting.wordpress.com/2014/0 … out-board/

I want to start making PCBs. To get started, I designed a RFM69HW breakout board - similar in concept to the cc3000 breakout board but using the RFM69HW for wireless RF. I used kicad because this is what we’re using in a course I am talking (Contextual Electronics).

I thought other folks that are “in the same boat” might be interested in what I learned along the way.

ALSO - I aspire to end up with a PCB populated with components that I have soldered on (seems intimidating right now…but…what the heck, I’ve got my rubber ducky in case I end up in the deep end…after all - just keep swimming!).

I would VERY MUCH LOVE to know how I can improve on the schematic. I also don’t expect feedback - rather cherish it and learn from it when I receive it.

Thank you.

2

Looking through your blog I would say that you are on the right track. Your thought process and design decisions seem thorough. My assumption is that you want to do this design yourself for the learning experience. Good for you! Note however that others have already done breakout boards for the RFM12B and RFM69. If you’d like a pointer to those designs, just ask.

To critique your design I am looking at the screen shots you posted. I use Eagle CAD instead of KiCad and I’d rather not load yet another CAD program onto my computer. The screen shots are a bit hard to read but I’ll comment on what I can make out.

The first thing I see is your power connections. Bypass capacitors go in parallel with the power connection not in series with it. Think about DC current flow. DC current cannot flow thru a capacitor (except for very short periods of time and amounts). You want a configuration that will allow tens of milliamps to flow continuously.

The RFM series components do not appear to share the quirk of the CC3000 on the MISO line so you might consider whether the additional tri-state buffer is really needed. Robustness of design is one consideration. Others might be cost, component counts and/or board size. You have to decide what is most important for your design. The same goes for the '245 buffer. (the '245 costs $0.27 in qty 100, 6 resistors would cost less than $0.05 - not a big difference for a hobbyist making one device but one day you might be working on designs you hope to sell in the millions…)

I can’t read all the signal names on the schematic. Posting higher resolution images would be useful. From what I can see things (other than power) seem to be wired right.

Good luck with your project.

  • Chip
3

  • The bypass caps (normally 100n, not 1u) should not be in series between +3.3V and the Vcc pins on the parts; Vcc should tie to +3.3V , and the caps should be between 3.3V and gnd. For C6 and C7, they should be in parallel

  • I’d use a single-pin component for the testpoints (use TST in the DEVICE library). That way, connectivity is correct without having to resort to named nets. Note that the footprint for the testpoint can have two holes with the same pin number so you can use wire loops on the board.

  • Named wires are considered the same. By having the wire connected to P1 pin 5 called MOSI and U2 pin 17 called MOSI, they are connected by the name. That’s not what you want. I’d name the two nets MOSI_5V and MOSI_3V respectively or something similar

  • The antenna pin is shorted to ground.

  • There’s a wire not connected in the middle of C7

  • U2 pin 1 needs to be connected. Also all unused inputs on U2 should be grounded or pulled down with a resistor.

  • U2 and U3’s values are missing the last few digits

  • It looks better to have the wire entering a ground symbol from above (like U2 pin 10) instead of the side (like U2 pin 19)

/mike

4

Chris and Mike - A HUGE Thank you!!! Your comments are incredibly helpful. I am very grateful.

Chip - re: “RFM series do not appear to share the quirk of the cc3000 on the MISO line.” I agree - I will remove the 74HC1G. Less parts, less soldering!! (The thought process I was having was potentially prototyping the RFM69HW with the cc3000 (instead of Ethernet). In that case, I have run into this with the RFM series…poor RFM chip could not move MISO once the cc3000 floated the traffic lane.)

Chip/Mike - re: 1) bypass capacitors go in parallel (both) 2) caps between 3.3V and GND (Mike). Ach - thank you. I changed the schematic. I decided to get rid of the bypass capacitors that are not near the voltage regulators. This simplifies the schematic and is similar to what other similar schematics I learned from do. However - I am glad I made this mistake here so that I could learn!

Mike - re: change TEST testpoint (which has two pin components) to TST which is single-pin. Done. Updated schematic.

Mike - re: 5V SPI lines (MOSI, CS, CLK from Arduino) to 3.3V SPI from RFM69HW. Your recommendation makes a lot of sense. Done. I renamed MOSI_5V, CS_5V, CLK_5V for net prior to the level shifter and MOSI_3V3, etc. after.

Mike - the antenna pin is shorted to GND. Done - updated schematic.

Mike - there’s a wire not connected in the middle of C7. Fixed by removing the additional bypass capacitors.

Mike - DIR (U2 - level shifter) needs to be connected. DONE. Noted in the “FUNCTION TABLE” (p 2 of data sheet) that ~OE = L and DIR = H is for data going from A bus to B bus. So I connected DIR to 3v3.

Mike - All unused input should be grounded. Done. Schematic updated (I see this is noted in the data sheet on p. 4: “All unused inputs of the device must be held at VCC or GND to ensure proper device operation.”

Mike - U2 and U3’s values are missing the last few digits. DONE. The challenge with longer value names is they appear in Pcbnew (laying out parts). When I was learning Pcbnew, I found the longer names made it more difficult to do the part layout….

Mike - it looks better to have the wire entering a ground symbol from above. Done. I was wondering if putting a gnd symbol flat with the net looked ok…I hadn’t seen other schematics with it, but it seemed reasonable. Does look weird.

Chip - resolution of image. I didn’t realize I could plot the schematic to the clipboard. hopefully, the new image is easier to read (although the resolution is 888 x 435 px…which doesn’t sound like a great resolution to me…).

Both - again THANK YOU very much.

5

You really do need the bypass caps. Rule of thumb (unless the data sheet says otherwise, like the RFM69 does) is to have one 100n (0.1uF) bypass capacitor per power pin of each device. When laying out the board, these caps are located right next to the power pin.

It looks like the antenna wire is still shorted to ground; I see a connection dot where it crosses the vertical wire going to U3 pin 11

/mike

6

Again - thank you Mike.

re: bypass caps → I added a .1uF in parallel to the 3.3V line of the RFM69HW. I also added in parallel a 10uF. My thought with the 10uF is to have additional charge located close to the RFM69HW when it transmits in “burst mode” requiring 130mA of (what I believe the correct term is) transient charge.

Q: does the 10uF reasoning make sense? Or is the 10uF near the voltage regulator “good enough”?

re: antenna. my insistence on shorting to ground underscores my misunderstanding about GND and RF transmission (related to using GND). I took the symbol for the hole I was using so that the copper wire that I solder on (where the copper wire acts as a monopole antenna) out of the schematic.

Q: I assume the antenna needs to be grounded. But are the grounds different ground planes? How do I represent the antenna hole in kicad (please see the image below which is what I believe needs to be done…here it looks like the antenna’s ground is same as the circuit’s ground…which got me connecting the antenna’s ground to the circuit’s…which has started to confuse me)? Perhaps this will help me better understand the “copy and paste” part of the circuit I used from excellent work on an RFM69HW arduino shield done by plutonomore (his files are found on this forum post: http://jeelabs.net/boards/6/topics/2934 … ssage-3537 but I can’t reach this post today - something wrong with my connection to the jee abs forum).

What I want to do is connect a hole to the ANA pin (so that I can solder a copper wire to it in order to act as a monopole). Then improve the likelihood the antenna will work best it can by anchoring it to ground (this shows my lack of RF knowledge).

This is what plutonomore did with the antenna in his (Eagle) schematic:

7

Your changes look good.

Regarding antenna: I am by no means an antenna expert but you are not trying to do anything complex. A dipole antenna is basically two wires running in opposite directions. One wire is connected to the signal. The other wire is connected to ground. The two wires are not connected to each other. The critical factor that makes the antenna work is the length of the wire(s). The length is set to create a resonance that allows the signal to efficiently radiate.

Drastically simplified, a monopole antenna is just the dipole antenna minus the ground wire side. Or if you prefer the ground plane of the circuit board is substituting for the other half of the antenna. This is not as efficient but works adequately as long as you are not trying to squeeze out the last bit of range or signal sensitivity. The monopole is not connected to ground, but is still making use of the circuit ground from a radiation standpoint.

Therefore your antenna connection needs to match the kind of antenna you will use. A single hole (like your test points) a short distance from and connected to the ANA pin would serve just fine as the connection to a single wire monopole antenna. Two holes (or maybe pads for a U.FL connector like this one https://www.sparkfun.com/products/9144), one connected to ANA, the other connected to ground, would be for a dipole antenna or a coax to an external antenna.

  • Chip
8

Thank you very much Chip.

I hope you will indulge me a follow on question regarding the monopole antenna. My reading up on monopole antennas leads me to believe that the antenna needs to be connected to ground (acting as a mirror such that the piece of wire works “best” at 90 degrees from the PCB) BUT not as I foolishly and clearly did not understand - in the path of the circuit. Just to system ground (a ground plane). SO I believe I now understand what plutonomore did (image above)- connect the hole that has the copper wire acting as the monopole antenna to ground…make a few connections to provide more ground.

My questions: 1) does the above paragraph make sense? 2) can the ground plane used for the antenna be the same ground plane as the ground plane used for the circuit’s path? I think this is fine because it is not picking up the current from the circuit. Although would there be more chance for interference if there is one ground plane instead of a two - one for the circuit and one for the antenna?

thank you!

9

Sorry, no your description is not clear to me. The wire (the piece of wire that is of the correct length and gets soldered into the PCB and connected to ANA) should not be connected to ground. If you connect ANA to ground you will short out the transmitted signal and nothing will get radiated by the antenna. However the electromagnetic field that radiates from that wire is affected by the circuit ground.

So in some sense the antenna is (radiantly) connected to ground, but the wire connected to ANA is not. Many times a PCB has a ground plane (a copper pour connected to ground) on one side. This is adequate for the antenna to work. The ground plane is the common ground of the circuit it does not need to be separate. You do not need to do anything special to the ground plane it works just because of its presence.

The site is back up and I am able to look at the reference you provided. In that example the ANA signal is brought to a connector for an external antenna. That connector has two contacts, one for the ANA signal the other for ground. The ground is used by those antennas (e.g. dipole) that need it. Again, the ANA signal is not connected to ground.

Is this getting any clearer? I think that part of the problem is the lazy use of “antenna” for the wire that gets soldered to ANA. While that wire is a part of the antenna it is not the entire thing. The wire together with the “ground” (either the circuit ground or more remotely the actual earth below the wire) make up the antenna.

Where is that online whiteboard when we need it? :slight_smile:

  • Chip
10

Hey Chip,

Thank you very much for your help and insights. It has really helped improve my knowledge (although as you can see from my head scratching regarding the antenna i can be quite dense, I apologize for this). If I haven’t frustrated you - is the below correct?

TERMS

ANA - it is the pin on the RFM69HW that sends out a current which generates an electromagnetic field that gets picked up by the…

Wire - a piece of copper that is soldered onto a connector that copies the current and radiates it so that another RFM69HW with a ANA/wire combo can receive the info in the current.

The two together form an antenna (the job of ANA is to send out a current, the job of copper wire is to radiate the current).

The challenge I have is perhaps with the term “Ground plane” —as pointed out in this wikiepedia entry:http://en.wikipedia.org/wiki/Ground_plane

In antenna theory, a ground plane is a conducting surface large in comparison to the wavelength, such as the Earth, which is connected to the transmitter’s ground wire and serves as a reflecting surface for radio waves. In printed circuit boards, a ground plane is a large area of copper foil on the board which is connected to the power supply ground terminal and serves as a return path for current from different components on the board.

So your comment: “the antenna is (radiantly) connected to ground” makes sense. Just having a ground plane on the PCB - and if using a monopole having the connected wire be at 90 degrees so that the ground plan can act as a mirror - serves the purpose of “ground” for the antenna. If the ANA was connected to GND, then a return path in the circuit is created - which is not what we want since the ANA is not drawing current it is pulsing the 1’s and 0’s which the wire picks up.

I updated the schematic to reflect this: https://github.com/BitKnitting/RFM69Bre … tBoard.pdf

11

“By Jove, I think he’s got it!” :clap:

I might word things a bit differently, but you have the basic idea correct. Most importantly the schematic is no longer shorting the ANA signal to ground.

I would change the following (this is just making the wording more accurate).

TERMS

ANA - it is the pin on the RFM69HW that sends out a current to the…

Wire - a piece of copper of the appropriate length that is soldered onto a connector that conducts the current. The wire in proximity to a ground plane forms an antenna that generates a shaped electromagnetic field (radiates) so that another RFM69HW with an antenna connected to its ANA pin can pick up the field and receive the info in the current.

The wire and ground plane together form the antenna (the job of ANA is to send out a current, the job of the antenna is to radiate the current).

Onward to the board layout part of the project.

  • Chip
12

Hi Chip,

MOST EXCELLENT , THANK YOU!

Just one small correction…it should read “…I think she’s got it!” :slight_smile:

Much gratitude to you. And yes…onward. Right now I am associating parts to the symbols, bumbling through digikey to get footprints…and then…yuk…making footprints for those nasty ICs that just don’t like being standard sizes.

13

BTW, now that we have the theory and basic connections correct…

See the various photos on LowPowerLab.com and JeeLabs.com that show the wire antenna. In many cases the wire is coiled or otherwise bent up to fit in an enclosure. Other times the wire is NOT at 90 degrees to the ground plane (for example see the picture below).

https://dl.dropboxusercontent.com/u/362 … G_5882.jpg

Although these antennas violate the prescribed definition of a monopole, they all seem to work sufficiently well.

There is theory and then there is engineering. 8)

  • Chip
14

Just one small correction…it should read “…I think she’s got it!” :slight_smile:

LOL Fair enough.

  • Chip
15

Again - thank you. I have added a section in my blog post about antennas and credited you with your amazing willingness to help me stop banging my head against the wall: http://bitknitting.wordpress.com/2014/0 … out-board/

16

The schematic is coming along nicely. On R2. the right side should connect to ground, not to CS_3V3.

The regulator data sheet has some notes about possible instability with output capacitors larger than 22uF. If that turns out to be an issue, you may need to drop that 47uF cap down to 10uF, so make sure the footprint you choose for the PCB can take either one.

/mike

17

I believe that the wiring of R2 is intentional. The LED will light only when the board is selected and the clock is high, doubly ensuring that the LED means board activity. It also lowers average LED current. The '245 has more than enough drive to sink the current. Kind of clever actually.

  • Chip