Hobby radar design

[sckzor]

That is a really cool board.  Thank you for letting me know about it, if I ever need anything that is accurate and reliable I will seriously consider that system.

My goal with this project though was to get a grip on RF and analog electrical engineering both of which have appeared as dark sorcery to me for a while.  I have done some digital things like embedded Linux and micro controllers but I never had a good grip on analog electronics.  I find that I learn best by jumping in an trying things, only issue is that it gets pretty expensive pretty fast.

[sckzor]

I received the attenuators yesterday, they came in late due to some shipping delays (I am assuming winter related).  Once I had them I did some testing and it appears that your hunch is correct radar_macgyver.  It looks like something is going wrong with the RF mixing.  I have once again attached labeled images from my testing.  I also tried the circuit with the coupling capacitor disconnected and the results were almost identical.  Unfortunately I forgot to take a photo of it and I do not want to disconnect it again unnecessarily.

My next step in troubleshooting would be to make sure that it is the mixer causing issues.  My best guess for how to do that with the limited resources I have would be to disconnect the RF from the receive signal amplifier and connect it to the LO signal on the mixer using a small bodge wire. By doing that the output off the mixer should be close to DC, otherwise the mixer is having issues.  This is probably not the best option ever because of impedance matching an whatnot but without a full blown RF lab I cannot think of a better method that would get close enough to at least tell me if I am entirely wrong.  I don't see why a test like this would hurt the RF mixer so at the very least I feel like it is worth a shot.

The only other explanation I can think of for this behavior would be the circuit traces for the ramp (which is clearly seems to be somehow mixed in with one of the signals) run about .7 mm from the received RF signal after amplification.  I suppose that the ramp trace could be inducing a current into the trace that carries RF to the mixer, causing it to behave strangely, however, I would think that the ramp would have to be oscillating much faster to create that kind of change current in that trace because the mixer is mixing different frequencies not amplitudes.  The difference in frequency between the ramp and the RF signal is enough that the change in frequency would look basically like a small, constantly changing DC offset as far as the mixer is concerned.  I could be wrong though.

I don't know if I mentioned this before, but I do believe the mixer is working to some extent because in the past the upper and lower lobes on the output with the antennas connected (highlighted in yellow and teal respectively on the corresponding image) predictably changed when I changed the distance of a surface from the radar.

Hopefully this information gives some more ideas...

Thanks again for any and all help.

[radar_macgyver]

The pix don't mention of the conditions that the measurements were made under. Is the mixer IF port terminated? It should be. With the TX looped back to RX, aside from a DC shift, the mixer output and video amp output seem fairly well aligned. The DC shift is due to the coupling capacitor, and is required since if you note the mixer output is negative-going with respect to ground. The video amp design gets around this using the coupling capacitor, and the amplifier end is tied to +5V. This seems to tell me that the video amp is working OK, though the last picture shows it saturating with the antenna connected. Note how the part highlighted in teal is showing up at the video amp output, but the part in yellow gets clamped to the upper rail. The video amp's first stage includes a gain control (RV2 in the schematic), does adjusting it help prevent the saturation from occurring?

I may have missed it, but did you post the board layout? On any RF board, that's kinda critical. From the one pic in reply #19, it looks like everything's 'spread out' over the board which makes me think that the traces are going to be lossy. Since you seem to be somewhat new to RF, consider replicating the MIT-OCW setup with connectorized parts first before taking a stab at doing it on a PCB. Without test instruments, this is going to be difficult to debug. Consider getting a USB receiver that can be used as a spectrum analyzer (Analog Devices Pluto, for example).

Having said that, I think you have a nearly working radar, just needs a couple of tweaks to make it usable.

[sckzor]

Firstly, thanks for your encouraging words.

I should have been more clear about this, but the photo that you mentioned with the video amp saturating was an old image I posed earlier, I have since fixed it, I just wanted to show the lobes that change with distance in the image and I believe they were the most prominent in that photo.  It no longer saturates when connected to the antennas or the attenuators.  The mixer IF is 50 ohm terminated into the video amp like before, nothing changed there.

I have attached an image of the board layout.  The whole board is very nearly the width of a standard credit card (85 mm) and a little bit shorter than one.  I read a bunch of different materials and was under the impression that so long as the traces were less than the wave length of the signal (i.e 300/2.4 = 125mm) then things would be generally okay (probably not super great but still okay).  I believe that the longest trace on the board is the one that runs from the power divider to the transmit antenna at 71ish mm.  I also remember reading that you do not really need to worry about traces being angular at 2.4 GHz and you can just route them like normal.  All of the traces are 50 ohm impedance controlled.

Please let me know if you see any issue with the board.  I could order another one if you think that it is a likely cause of the interference, although, even if the traces are wrong I would think that the interference would not look like it does.  Alternatively, could the mixer possibly be heat damaged or something? I did have to reheat the board because the first revision had a footprint error, I think the mixer was one of the last components to come off which means it was on my somewhat poorly temperature controlled soldering plate for probably upwards of 5 minutes.  I don't know if these parts are generally super sensitive?

I am very new to RF, this is my first from-scratch project.  I seriously considered trying the MIT OCW approach with the mini-circuits parts, however, after some consideration, I came to the conclusion that I see the mini-circuits route like I see building a desktop computer, it is interesting and you will almost certainly end up with something that works well but there isn't all that much to be gained from doing it learning wise.  It is building expensive legos, definitely cool and I understand why MIT would do it that way, but I think I get the same value from watching their series about it as I would from doing it myself (I did watch their whole video series about it before starting this project.)  I would have tried it both ways, comparing the results (I think some UC Davis students did this) but I don't have a whole lot of money to work with, a max of about $400 USD so I can't really afford to do both.  I figured if I did it the mini-circuits way I would get something that works and a little bit of extra learning value.  If I did it the PCB way I might end up with a cool looking, expensive paper weight but I would learn a whole lot about how RF systems are designed in the real world either way.  To me, it was worth the risk of the expensive paper weight to have the ability to learn a lot more about this.

[radar_macgyver]

Here's the saturation I was referring to:


Note how the rest of it looks like a scaled version of the mixer output. Try adjusting the gain control to see if you can lower the video amp gain to eliminate this effect.

As for the layout, yeah there are certainly some issues. The RF traces are long, and run parallel to other traces, what you have then is a coupler (see for example the three traces under 'R17'). As a rule of thumb, they should be as short as possible, so in your case, the VCO and mixer should be close to the antenna connectors, rather than on the other side of the board. There are also way too few vias to the ground plane around, for example, the VCO - it has so many ground pads for a reason.

tggzzz had posted a link to  https://hforsten.com/, take a look there for examples of a more typical RF layout. Sure, his FMCW radar has a lot more parts than yours, but much of it is bringing the signal processing on board; the basic design is almost identical. See also his discussion on the video amp design.

[sckzor]

My apologies for again taking forever to respond to this thread.  Things again got unexpectedly extremely busy for me toward the holidays and the beginning of the new year.  I did some further testing with some bodge wires on the PCB and I think that the interference explanation that radar_macgyver gave is still the most likely to be the case in this instance.  To solve this problem I redesigned the PCB with a lot more grounding and I moved the components much closer to one another.  I have not yet done impedance control on the traces (because I might switch PCB houses for some reasons) but barring that I think this design is much better.  I have both attached photos of the design and made them available at https://github.com/sckzor/RadarProject/tree/master/AnalogRadar/MkII if you would like to load them into kicad (sorry if there are random extraneous files I am rapidly running out of time to work on this).  If others think it is good too I will send it into production and hopefully make this radar work much better.

Thanks to all that have helped (especially radar_macgyver),

sckzor

[Berni]

All i know is that i need to put "Behold my latest fire hazard" on more of my boards.

[radar_macgyver]

Much better layout, things are more compact. I would get rid of the 'thermal spokes' connecting the surface-mount pads to the ground plane, if you have a suitably rated soldering iron (or a board preheater) because it will make the soldering operations a pain. If you're going to stick with JLC's 7628 process, consider using a transmission line calculator program to design a 50 ohm microstrip (or coplanar waveguide) for all the traces that carry RF.

It does look like you're using some rather large passives, 0805 maybe? Their pads will present a large parasitic capacitor to the nearby ground plane. If you can, drop the size to the smallest one you can. Ideally, one would pick a stackup and transmission line geometry whose trace width is very close to or equal to the passives used, so there's very little impedance mismatch when the traces meet a passive components' pads. With coplanar waveguide (CPW), one can tweak the trace width (by adjusting the spacing to the nearby ground plane) without changing the stackup. CPW does have some drawbacks - mainly that there can be multiple propagation modes depending on the spacing and width chosen. This is minimized by not deviating too far from the width used for microstrip.

Finally, if you're open to a bit more layout tweaking, what I found is that laying out RF boards is a bit different in that one lays out the parts to minimize jogs and turns in the traces - everything's straight lines or 90 degree turns. Take a look at Henrik's boards for inspiration - note how all the RF parts are lined up neatly so the traces are all straight lines. He went the extra mile and made the 90 degree turns use miters to avoid impedance mismatches - I prefer to use swept (curved) traces instead. The pic below shows his implementation of a Wilkinson power divider:



He also placed a solder mask opening over the the transmission lines so that the solder mask doesn't change the Z_o of the line.

All i know is that i need to put "Behold my latest fire hazard" on more of my boards.

Haha, I might just do that on the one I'm working on now (48V/10A H-bridge)

[buta]

Given from datasheet:
VCO, U5, Crystek has a lower output than Raltron, 0, 3, 6 dBm (min, typ, max)
Attenuator, U1, AT0603T03ECATD, -3 dB, assume constant
LNA, U3, BGU8052, gain, 17, 18.5, 20, dB
LNA, U3, BGU8052, output power at 1dB gain compression PL(1dB), 18 dBm typ

Calculate:
LNA, U3, BGU8052, output power, 14, 18.5, 23, dBm

Concern:
The LNA may operate in the nonlinear area as output power > PL(1dB), it may generate additional harmonics, noise or ....

[sckzor]

I took your advice radar_macgyver and added a calibrated co-planar wave guide for the RF, and I swept all of the trace corners and removed the solder mask.  I tried to make the CPW larger to match the size of the component pads but according to the calculator I used, the JLC stack up has pre-preg that is too thin to make the trace much larger than it is right now.  I think I will use JLC again as I did all of the calculations and setup based on their stack up and they still seem to have the best price.

I don't really want to change my SMD component sizes.  I already have everything in 0805 size and I don't want to order new parts unless you think this will present a big issue later.  Additionally, I am not the best at soldering and I start to struggle soldering anything smaller than 0805s with an iron.  If I need to do any rework it is nice to be able to use an iron.  If you think this is a big problem I will bite the bullet and change it but like I said, I don't want to.

Finally, I made the thermal reliefs smaller to make the soldering easier.

I attached more images of the new layout.

Thank you for pointing out that discontinuity buta, I think I will just accept that it could be an issue and carry on unless it will completely break everything.

Thanks

sckzor

Haha, I might just do that on the one I'm working on now (48V/10A H-bridge)

Last time I built an h-bridge one of the transistors I was using got overloaded and blew up in my face lol

[radar_macgyver]

@buta: the calculations don't include the LO to IF isolation of the mixer. The mixer, being double-balanced, will have some isolation between LO and IF ports. This will be degraded somewhat by coupling between the traces, but will still be higher than 0 dB.

@sckzor: Sorry if this is coming in a bit late, but your layout looks much better with good coupling between ground planes. Consider rotating U6 so that the LO port (pin 2) faces up towards the board's TX port. This will eliminate a couple of bends from the RF traces. I would say that if you had to pick one part only for size reduction, it would be the RF coupling capacitors. You could easily make these 0402 or even 0603, with enough room around the parts, these aren't too hard to hand solder or rework. You could also drop the value to 1 nF or lower and make sure they are C0G dielectric, to minimize losses. On the layout surrounding U3 and U4 (the RF amps), you have a short stub on the RF traces connecting the amplifier outputs to the biasing inductor. You could make these "inline" to avoid the stub. Check out NXP's AN11902 to see how they designed a board for this part. AN11416 also has more detail on the completed board, look closely at how the inductor is placed relative to the part. Also note the BOM shows the exact parts used.

[buta]

@buta: the calculations don't include the LO to IF isolation of the mixer. The mixer, being double-balanced, will have some isolation between LO and IF ports. This will be degraded somewhat by coupling between the traces, but will still be higher than 0 dB.

The calculation considers the TX path not the RX path, it shows the LNA U3 (use as a TX amplifier) operates close or above to its 1dB compression point in typ and max conditions.  The TX signal will be distorted and will contain additional harmonics, noise or ...
Usually amplifiers should operate few dB's below the 1dB compression point.

[radar_macgyver]

Oops - missed that you were only looking at TX. The OP could replace U1 with a different part to bring down the gain. Then again, it's FMCW, so the amplifier can operate into saturation without sacrificing performance other than generating more harmonics.

[sckzor]

You are not too late @radar_macgyver.  I am still dealing with a tremendous amount of work and have stalled continued design unfortunately.  If you think smaller coupling caps and inductors would be better I can probably spare the funds to replace them, and while I am at it I can order the larger attenuator.  Later this week, probably Saturday or Sunday I will get around to making further revisions the PCB and and parts list and post about them.

At the risk of redundancy, thank you again @buta and @radar_macgyver this would not be possible without your help.