Needing more than a spark test?

[homebrewed]

As I recall, you designed this structure in SCAD?

Yes. If you want the script, just let me know.

 

[homebrewed]

Yes - I came to the same conclusion about tilting. The 52° I came up with was built around the constraint of having the lead shield cylinder around the PIN photodiode, the sources arranged around, also shielded from radiating backwards or sideways, and how close one could get consistent with physically fitting the sources around the detector.

Re: the low count. Is the advice to squeeze in 8 instead of 6 sources?
Are we saying we should max out with more rows of sources?
I can imagine a circular support about 75mm diameter, a shielded PIN diode in the middle, and all the remaining area packed with sources!

My current setup is using 8 sources. A big reason why I've got lead sheet inside the box!

 

[homebrewed]

Hi Mark
Just to get me clear on the LMC662. Is it always operated with negative power input grounded, and positive power input at 9V?
Also, is the LMC662 on the signal conditioner board also like that?

The pocket geiger uses a single-ended power supply. There's a voltage divider string between +9 and ground that generates a virtual ground for the LMC662's noninverting inputs and a couple of voltages that serve as "reference voltages" to the comparators. This of course means that the analog output is sitting above ground. For that reason, I AC coupled the signal going to my signal conditioning board.

Examination of the divider string indicates that it isn't designed to generate Vcc/2 for the virtual ground, it's noticeably higher than that. At this point I'm not quite sure why that is. While pulses coming out of the TIA will be negative-going (so the divider string design sort of makes sense), the second amplifier in the chain, which has substantial gain as well, also is an inverting design: so its dynamic range will be reduced. Hmm, hmm. Scratching my head over this one.

Since I have enough lab supplies to manage the power supply requirements, I designed my signal conditioning board so it uses balanced +/- 10V supplies. That does have its drawbacks because there's the possibility of pulling the Teensy's ADC input below ground if something goes awry. Something to think about when designing the final version, if something like that is needed.

Your question has prompted me to consider the possibility that my modified pocket geiger board's TIA and filter block may not be all that happy. The reason being: I yanked the LMC662 off and replaced it with an Analog Devices part (because it has better noise specifications). BUT that part has a reduced power supply range, maxing out at 5.5V. I took care of that issue by swapping out the 9V linear regulator with its 5V cousin: but, since I didn't change the divider string that MIGHT be causing some problems in other places. Time to make some measurements.... and look more carefully at some opamp data sheets.

 

[WobblyHand]

Yes. If you want the script, just let me know.

I would like a copy of the script. I believe FreeCAD can import SCAD. If not, I'll install it. From that I can get a better idea of what to do.

I ordered 8 sources from China. About $1.54 each plus shipping.

 

[graham-xrf]

The pocket geiger uses a single-ended power supply. There's a voltage divider string between +9 and ground that generates a virtual ground for the LMC662's noninverting inputs and a couple of voltages that serve as "reference voltages" to the comparators. This of course means that the analog output is sitting above ground. For that reason, I AC coupled the signal going to my signal conditioning board.

My apologies in advance. This is a bit of a trawl through exactly what the PocketGeiger does that I had to do, to satisfy myself about what it does, and let me feel OK about cutting through it with a Junior hacksaw to just have the PIN diode.

OK - call me nerd, but here I have a little something that might save a lot of measurement time initially, and may help make some decisions.
@WobblyHand also just might soon be messing with a PocketGeiger board, and we need to have him catch up on what you and I have been "changing".

In the end, I discover that what is on the Pocket Geiger is not ideal, but with some simple changes, can become workable, and if one changes the first op-amp, and power rails, it gets potentially useful.

Examination of the divider string indicates that it isn't designed to generate Vcc/2 for the virtual ground, it's noticeably higher than that. At this point I'm not quite sure why that is. While pulses coming out of the TIA will be negative-going (so the divider string design sort of makes sense), the second amplifier in the chain, which has substantial gain as well, also is an inverting design: so its dynamic range will be reduced. Hmm, hmm. Scratching my head over this one.

I get it that you have replaced the LMC662 with another opamp, and changed power rail volts, but just temporarily, I stay with the LMC662.
Also - we start out with Rf=66MΩ and Cf=1pF.
Important to note that 1pF is OK with the 66MΩ for stability, and it is part of why the negative going output pulse settles in about 340uS.

If lower gain (440K) is chosen here, and gain as needed put downstream, one needs Cf = 6.8pF to yield much better performance, and (I think) better noise figure.

The first bias
The first divider chain in the PocketGeiger tries to make the opamp work at halfway point between 0V and 9V
The divider puts 802.2mV on the positive input, which along with the 6mV or so Voffset, results in U1A output sitting at 2.04 volts.
The response to the photon pulse is on top of that, negative going, and apparently reasonably fast, amplitude -1.86mV

What happens here is about a huge time constant based around the 66MΩ, the 1pF, and whatever other capacitance it sees.
The output initially goes downward, pretty fast, following the photon pulse current, and then spends the rest of the time leaking that output back through the 66MΩ to settle back to quiescent condition

I do include her the LTSpice simulation models, library for LMC662C (the one with 6mV Vos), and the redrawn opamp symbol, for you and @WobblyHand to use later, but for the moment, I have examples where we step through in stages with the plots, because the upstream ones display too small in Y-axis if later ones are on the same plot.

I get it that we are more interested using own choice of opamps in there, but as it happens, there exists a different gain distribution solution that allows the PocketGeiger LMC662 to deliver a slowed down pulse that might be workable, though I did not fancy the noise performance. V(N007) is the U1A output.



Now move on to what happens at U1B second opamp output V(N007).
Notice that the second opamp has its positive input at 802.2mV, just like the first, but it's output is not at 2.04V.
I would think that this is because of the constant 1.5nA dark current coming from the PIN diode when it is biased -10V, feeding U1A.
The second opamp does not have any constant dark current input, and it's a voltage amplifier anyway.

The U1B output is responding to the slowed down negative going -1.86mV, and attempts to make it's positive-going inverted version.


The Signal Conditioner board
We press on looking at what happens onto the signal conditioner board.
It goes through a 1uF capacitor, and a 10MΩ low-pass RC.
Multiply R x C and throw in the 2π, and find reciprocal, and we have a cut-off frequency 0.0159 Hz
Maybe we should not do that!

The stage that follows amounts to a follower with 1K in the feedback, and has a voltage divider network feeding into the inverting input via a 1MΩ resistor. Technically, it is a non-inverting amplifier with gain 1+1K/1MΩ = 1.001, but that gives a way to set the DC output to halfway between the rails. That's OK. It shifts whole thing downwards about 0.8V, which is useful, though arguably not enough when we look further downstream.


What we have is a 800mV delayed (by about 50uS), and stretched out (to about 250uS) positive going pulse. It does have a similar shape to the original pulse, sort of. We have to believe that this pulse shape, and the area under it, is strongly related to the original photon pulse shape.
The original was also shaped, depending on the charging of a PIN diode capacitance.
This one is shaped based on the CR time constant of a shunted integrator (U1A) charging a 66MΩ Rf, that used the already spread out photon pulse as it's input to work on. Then another (U1B) downstream, doing much the same, but faster, using 10pF and 1MΩ. That one rolls off at 16kHz, so would not make much difference

Since I have enough lab supplies to manage the power supply requirements, I designed my signal conditioning board so it uses balanced +/- 10V supplies. That does have its drawbacks because there's the possibility of pulling the Teensy's ADC input below ground if something goes awry. Something to think about when designing the final version, if something like that is needed.

The labels on the power rails for the signal conditioning board still say "V+10" and "V-10". As soon as I saw that, I knew it was beyond the 16V allowed for the LMC662. I changed V5 and V6 to be 5V each, but I forgot to rename the labels. Your power supply change is taken into account, as is the fact this part of the circuit operates between equal positive and negative rails
It does, of course, crash the rail, because it now has a +5V supply.

Your question has prompted me to consider the possibility that my modified pocket geiger board's TLTspiceXVII/lib/sym/AutoGeneratedIA and filter block may not be all that happy. The reason being: I yanked the LMC662 off and replaced it with an Analog Devices part (because it has better noise specifications). BUT that part has a reduced power supply range, maxing out at 5.5V. I took care of that issue by swapping out the 9V linear regulator with its 5V cousin: but, since I didn't change the divider string that MIGHT be causing some problems in other places. Time to make some measurements.... and look more carefully at some opamp data sheets.

I actually would prefer to be where you are now, actually making measurements.
But - I am behind with it all. Forgive that I am still getting curious with simulations. Its just that the simulations are much faster in taking me to making decisions, whether about bias, or changing op-amp, etc. If you and @WobblyHand (we must try for his name?) find it useful, I post the model here.

NOTES:
1. In the ZIP file, there is a LMC662C.lib. That one is the commercial PMC662 with the 6mV Voffset.
I derived it from the original LMC662B.MOD model from TI, (also supplied here in the TI data pack)
My Linux Mint thinks it's a music file! The data sheet is in there also.
I edited it to change the .SUBCKT name to LMC662C
This file needs to be placed where LTSpice can find it. I simply let it live in the same folder as the model being simulated.
The LTSpice directive .lib LMC662.lib needed to be right-clicked on, and the SPICE .lib directive explicitly selected, instead of the .inc (include) to avoid the netlist seeing duplicate node idents.

2. Hopefully, there is a LMC662C.asy in the ZIP file. This one started out as an auto-generated default, but I edited it to look like a op-amp.
It is supposed to live in the user's documents LTSpice stuff "Documents/LTspiceXVII/lib/sym/AutoGenerated".
If you happen to be using a Linux computer, and running LTSpice under Wine, the program uses a link to the usual home folder.
Mine is in /home/graham/Documents/LTspiceXVII/lib/sym/AutoGenerated

If you are using a Windows computer, I see it in c:\users\user_name\Documents\LTspiceXVII/lib\sym\AutoGenerated\LMC662C.asy
This is the only file you need to actually move or copy into your system
There are other ways to add symbols and models into LTSpice, in the library, but this is what I just threw in, and it worked.

3. Some simulation go nuts when one makes modifications, I have not explored in detail the best settings, but there are some I have discovered.
There are texts on the model schematics that explain.

One thing I would mention. We already have waveforms that will crash the 5V rail, starting out with 2.5nA of photon pulse. That may be correct, because maybe we should expect about 120pA is the "huge" pulse, and 45pA is the "smaller" type. Regardless, the ADC uses 2.048V reference. The "Absolute Maximims" for the ADC are AVDD +0.3V, and AGND -0.3V. If we use +2.5V for the + rail we, then in switched gain settings, we can let the oversized pulses crash the rail, and get ignored, while keeping the ADC safe.

In any event, we never need that the last stage piles on so much gain that it hits 5V less than 30uS into doing it's thing!

So there it is. If anyone finds it useful, that's great.
I am considering getting in the Analog Devices DC2414A evaluation board from Mouser (£26-93), with the possiblity of getting three op-amps in. This competes with the knowledge that I will end up with a self-designed PCB anyway, with ADC and hum filter and switched gain ranges. Even so, knowing how to modify the PocketGeiger lets us have some development practice runs with real electrons doing stuff in there.

 

[graham-xrf]

I would like a copy of the script. I believe FreeCAD can import SCAD. If not, I'll install it. From that I can get a better idea of what to do.

I ordered 8 sources from China. About $1.54 each plus shipping.

Do tell about where you got them from.
I was having thoughts about a 12 or 16 circular array of sources.
Also, some pictures of the tear-down to get at the little button might be nice.

 

[WobblyHand]

Thanks for the write up and your simulation settings. For tough to simulate circuits it's nice to have the settings recorded in the schematic. Spice is one of those programs where you have to use it a bit to keep up with the "tricks" necessary for a good simulation. If I haven't used it in a year or so, I forget those tricks.

@graham-xrf my name is Bruce. It will take me a day to get up to speed on your schematic and simulation. Have to figure out how one adds models to LTSpice, it's been a while.

 

[WobblyHand]

Do tell about where you got them from.
I was having thoughts about a 12 or 16 circular array of sources.
Also, some pictures of the tear-down to get at the little button might be nice.

Found them on AliExpress. Have to go to my main computer to get the link I briefly thought about getting more and decided against it. 8 are within my comfort zone right now. Buying 3 dozen just didn't sound prudent to me.

Edit: Here's the URL for the sources. AliExpress Americium Sources shipping is more than the product, but still cheaper than buying locally.

 

[graham-xrf]

Thanks for the write up and your simulation settings. For tough to simulate circuits it's nice to have the settings recorded in the schematic. Spice is one of those programs where you have to use it a bit to keep up with the "tricks" necessary for a good simulation. If I haven't used it in a year or so, I forget those tricks.

@graham-xrf my name is Bruce. It will take me a day to get up to speed on your schematic and simulation. Have to figure out how one adds models to LTSpice, it's been a while.

That's the point of the ZIP folder.
The model is already there in the library file I supplied. Look at it with a text editor, and look for "SUBCKT", and there you see the part name.

The other thing that it needs is a symbol to have it's pin numbers associated with the circuit you connect it to. That is also there. Of course you can just use a default rectangle with the right number of pins, like I once did in an earlier posting. So, just like anyone creating a part, I edited the symbol, and clicked "save". That file is the only one you have to put in a specific place, unless you want to create your own.

I deliberately provided the photon current source equivalent circuit for the X100-7 PIN diode already built in to the simulation circuits. It uses a contrived exponential pulse to look like those that really would happen. The only thing we might have to do is reduce it's amplitude, so the thing pushes pico-amps instead of nano-amps.

For the moment, just start up LTSpice, get the files that are in the ZIP into the folder you want them to live in. Copy the .asy file into the right place as explained, then drop the simulation .asc file into LTSpice, and click on the "little man running" icon. If it starts messing about, not completing after (say) 10 seconds or so, the push ESC two or three times.

 

[WobblyHand]

@graham-xrf I don't seem to have an Autogenerated subdirectory under sym. I can create this, but is it necessary?
Under home, it is .wine/drive_c/users/bruce/My Documents/LTSpiceXVII/lib/sym as I said, there's no Autogenerated . First folder is ADC. I have display hidden directories ON.