Simple Sinusoidal Oscillators

[mawyatt]

Detector based upon controversial Passive Spectral Radiometry....long story about solving the impossible if someone is interested

Interested?  You must be kidding, not only interested but rather eager to hear more, of course. 

Ok should start another thread.

Best

[RoGeorge]

Ok should start another thread.

Found it, thank you:
https://www.eevblog.com/forum/projects/xm21-remote-sensing-chemical-agent-detector/


Back to the Peltz osc, in my attempts the most beneficial measures against distortions were:
1. - reduce the power supply close to no oscillations (can oscillate with as less as 0.6-0.7V)
2. - increase the R emiter (lower the T current - still oscillates with 50-100k)
3. - lower the Q of the L (add a series resistor - can oscillate with X_L/R ~ 1 or lower)

Any of these also reduces the amplitude, which is essential to do, or else the oscillations will be limited by the V_BC forward, because BC junctions are in parallel with the LC tank.

Adding base resistors as suggested in the Analog Devices lab material didn't help as much as the other 3 measures listed.

What puzzles me is that I couldn't get anywhere near the -65dBc harmonics showed in your latest measurement.  What I see is more like -45dBc.  I will try this weekend an oscillator in the kHz range, so I could measure the distorts with a sound card.

Did you used other tricks than in the ADI lab (in order to get less harmonics)?

[mawyatt]

Back to the Peltz osc, in my attempts the most beneficial measures against distortions were:
1. - reduce the power supply close to no oscillations (can oscillate with as less as 0.6-0.7V)
2. - increase the R emiter (lower the T current - still oscillates with 50-100k)
3. - lower the Q of the L (add a series resistor - can oscillate with X_L/R ~ 1 or lower)

Any of these also reduces the amplitude, which is essential to do, or else the oscillations will be limited by the V_BC forward, because BC junctions are in parallel with the LC tank.

Adding base resistors as suggested in the Analog Devices lab material didn't help as much as the other 3 measures listed.

What puzzles me is that I couldn't get anywhere near the -65dBc harmonics showed in your latest measurement.  What I see is more like -45dBc.  I will try this weekend an oscillator in the kHz range, so I could measure the distorts with a sound card.

Did you used other tricks than in the ADI lab (in order to get less harmonics)?

Didn't use any base resistors or other "tricks", just a couple 2N3904s, L, C, and a 510 resistor. Reducing the collector current should improve results as the incremental gain across the waveform period when integrated must be identically unity in steady state, so higher collector current results in higher "gain" at the waveform mid-section and thus lower compressed gain at the peaks so the average over the waveform cycle is unity. At lower collector currents the gain across the waveform cycle is more uniform and should produce less distortion.

As you mention, the gain "compression" at the peaks is due to the CB junctions which acts as a self limiter, and adding series base resistance allows a larger signal swing and a softer self limiting and may slightly improve the distortion, although haven't tried yet.

Anyway, have fun with this, it' really an interesting little circuit!!

Edit: An important note regarding the waveform cycle unity gain requirement under steady state. An ideal oscillator eventually settles to a sinusoid with constant amplitude or:

Vo = V*{Exp(alpha*t)}Sin(omega*t), where alpha is identically zero under steady state and negative under waveform decay and positive under waveform expanding.

(Need to figure out how to enter proper equations like others use, MathJax or other method!!)

Simulations with many oscillator cycles involve waiting for the oscillator to reach steady state, so then one can get better results, but this imposes a long simulation time frame even on a fast computer. Long ago we ran into all sorts of issues attempting to simulate very high Q oscillators, one thing we did to help with the actual simulation time was utilizing a PWL current source to ignite the oscillations with a PWL current that approximated the desired oscillator output. This caused the oscillator to sort of kick start very close to the final value frequency and amplitude, and a carefully crafted current source could save considerable simulation time. Another issue is that very fact of a simulation creates a sampling effect and subtly imposes the sampling effects upon the oscillator, one of which the sampling function has a "gain" of slightly less than unity. Under steady state the oscillator loop-gain should be identically unity, however the sampling effect reduces this below unity and can cause the oscillator output to decay. This is one reason why some oscillator simulations die out after a kick start and require the time step (sampling period) to be significantly reduced for long simulations with many waveform cycles. With a smaller period between simulation samples the sampling effect more closely approaches unity {sinc function moving towards the origin, and at origin (zero sampling period, or infinite sampling rate) is unity}.

Unfortunately the longer (more) the simulation of oscillator cycles the shorter the simulation time step if one wishes to achieve very accurate sim oscillator results after many cycles. One can run the simulation with a moderate time step with many oscillator cycles, then carefully attempt to recreate the waveform with the mentioned PWL current source, and restart the simulation with the modified PWL current source and much smaller time steps. This should yield a waveform result with more waveform fidelity in fewer cycles under the smaller time steps. Much later Cadence came up with various simulation augmentations to address high Q oscillator simulations, and this improved one's ability to accurately simulate high Q oscillators. Suspect Cadence has some tutorials on such.

Best,

[moffy]

Number resolution can also be an issue. In LTSpice you can turn 'off' compression in the control panel and this will improve any FFTs done on the data.

[RoGeorge]

No idea if QucsStudio is using lossy compression when saving data, like in the LTspice defaults.  Since, by default, QucsStudio only saves data for the specified signals, I suspect QucsStudio doesn't compress the results at all.

Just for the fun of it, attaching an LTspice simulation for 3 distinct Re values.  It was just a draft, I didn't use the behavioural source trick to start the oscillator, only used the LTspice 'uic' option instead.



At first I've simulated with LTspice, but QucsStudio has a very nice feature:  one can simply click on a value to add a live slider for that value, which make QucsStudio the ideal tool to quickly adjust/optimize a schematic (something like seen in this video, unrelated with the Pelts oscillator, only to show how easy is to add tuning sliders:  https://youtu.be/fYs7ZoVyPmM ).

QucsStudio is free to use but not open source, was made for Windows but works in Linux, too, using Wine (should work under Wine for Mac also, but I didn't try).

[gf]

Screenshot_20220708_094621.png

I wonder for which time window of the transient simulation the spectrum is calculated?
At least for this usecase, only the trailing samples should be considered, where steady state is (almost) reached.

[mawyatt]

Number resolution can also be an issue. In LTSpice you can turn 'off' compression in the control panel and this will improve any FFTs done on the data.

Also once you get down to these levels the SPICE parameters such as reltol, abstol, chgtol, and so on can be tweaked to improve simulation fidelity.

Best,

[moffy]

Number resolution can also be an issue. In LTSpice you can turn 'off' compression in the control panel and this will improve any FFTs done on the data.

Also once you get down to these levels the SPICE parameters such as reltol, abstol, chgtol, and so on can be tweaked to improve simulation fidelity.

Best,

They can also make convergence a pain, tweak with care.

[Sengcid]

A bit off topic but jfets work nicely, albeit with a high Q tank cct. I will put more details in another thread.

[PeiCB]

In Wireless Worlds three volumes of "Circuit Designs special Editions" which is available for free download here:

https://worldradiohistory.com/Wireless_World_Magazine.htm

there are a number of similar designs as the Pelz-oscillator described.

Unfortunately I do not remember exactly where but the volumes are so rich in information it is a joy just to browse through them all!

[doktor pyta]

I did't knew the name of the inventor, but back in 2013 i've built 'the shittiest VCO ever' for educational purpose:
https://www.elektroda.pl/rtvforum/topic2548956.html
As it turned out it has some practical uses (but with X7R capacitors).
Thanks for the post mawyatt.

[Kleinstein]

Using X7R capacitors as voltage controlled capacitors is a strange idea. It may work in a PLL loop or similar, but probably not for a stable frequency on it's own.

[mag_therm]

My "entry" is a DDS locked tube Hartley Local Oscillator
https://app.box.com/s/ufytpndvnjm3yljoezz96afiqy2lcqfa
After trying some other methods, this one using the 6BE6 (Mixer tube) signal grid as injection point works best.

The glass tuning scales (re- artworked by Radio Daze)  on the old receiver still work as originally with the DDS deselected in  the app.
There are presets for the DDS in the app, also a lock can be manually entered.

Spect An show that the unlocked 2nd and 3rd Harmonics are about -50 and -45 dB respectively on 20 metre band
There are phase noise sidebands on the L.O. output, I think due to proximity of strong ft8 signals coming in to RF stage

When the DDS is switched in, the harmonics are both reduced by about 5dB.
The noise sidebands are significantly reduced by DDS but I am not sure how to measure noise sidebands on the old analog Spect An.

I presently have the DDS level and negative bias from the 2n2907 set for a lock range of about +/- 3 kHz

There are other mods to upgrade the receiver especially for L.O. stability to receive digital modes.
-Plate and Filamant voltage regulators
-The original 6AV6 is switched out for ssb and ft8 etc  and a Gilbert cell is used as demodulator
-Shaft drives have ball bearings added and the dial cord is replaced with the newer dual core type.
-A temp sensor is added to the variable tuning cap with a PI controller on a variable speed fan.
(The chassis and tuning cap run at about 10 C above ambient due mainly to the losses in the rectifier tube.
This is leveraged so the fan cools more if the temp rise, and slows down if the temp falls.

[mawyatt]

With the Peltz oscilator mentioned we changed L to 10uH (9.017uH) and C to10nF (9.523nF) which should produce ~543KHz waveform with Vee at -1.5VDC.

Here's the results, not bad for a simple oscillator.

Best,

[moffy]

In Wireless Worlds three volumes of "Circuit Designs special Editions" which is available for free download here:

https://worldradiohistory.com/Wireless_World_Magazine.htm

there are a number of similar designs as the Pelz-oscillator described.

Unfortunately I do not remember exactly where but the volumes are so rich in information it is a joy just to browse through them all!

Thanks for the reference, I have downloaded the 3 volumes, used to love Wireless World, so much content.

I feel a little slow in recognising how the Peltz oscillator works so I have redrawn it so the differential pair is a bit more obvious.

[mawyatt]

What are the primary motivating advantages of using the Peltz oscilator as compared to other simple-ish roughly similar BOM size sinusoidal oscillators e.g. Colpitts, Hartley, Clapp, ...?

Here's a few that come to mind, although not sure if these are necessarily "advantages" over the other style sine wave oscillators.

Maybe "features" is a better characteristic.

a) Simplicity, 2 transistors, 1 resistor, 1 inductor and capacitor.

b) Simple biasing, only one resistor.

c) Symmetrical self-limiting, important for low harmonics.

d) Ground reference output, low DC offset when using only negative supply.

e) Low voltage operation, requires only slightly more than Vbe_on (~0.7VDC).

f) Wide supply operation, essentially e) to any available voltage since the emitter resistor limits the available current and the transistors never "see" more than a CB junction drop.

g) See a) !!

Best,

[mag_therm]

It would be useful to do a  high frequency hybrid pi analysis based on Moffy's clarification of the Peltz.

L1 and C1 and L1_R_equiv_parallel and 2*(R_ce_H_pi) all in parallel  give the  circuit Q at a frequency.

That can be compared with a model of Hartley.
Hartley's patent claims include ...tappings ...."at least a portion of" ...full turns.
That seems to include any tap  > 0% to < 100%
 He describes damping instead of present day Q
Lower taps on Hartley will increase the Q

Higher Q in these oscillators will give better harmonic suppression , but I am not sure about effect on phase noise.

[RoGeorge]

...
An important note regarding the waveform cycle unity gain requirement under steady state. An ideal oscillator eventually settles to a sinusoid with constant amplitude or:

Vo = V*{Exp(alpha*t)}Sin(omega*t), where alpha is identically zero under steady state and negative under waveform decay and positive under waveform expanding.

(Need to figure out how to enter proper equations like others use, MathJax or other method!!)

This forum supports MathJax, with formulas delimited by backslash dollar at both the beginning and the end of a formula (for inline formulas), i.e.  \$ V_o = Ve^{\alpha t}\sin(\omega t) \$ or backslash open-square-bracket at the beginning and backslash close-square-brackets at the end for formulas centered on a new line:   \[ V_o = Ve^{\alpha t}\sin(\omega t) \] where t is time ...

There is a small thread with examples of posting math on EEVblog:
https://www.eevblog.com/forum/beginners/how-does-posting-math-notation-work/msg3994178/#msg3994178

The drawback is that MatJax formulas are not rendered at preview, they only show as formulas after posting, which makes editing a pain.  There are online MatJax editors that can live-render formulas, then copy paste from there to here.  There is a trick I've found working to preview MathJax in EEVblog, formulas are rendered when pressing preview from a locally saved reply webpage, like this:
- press the reply button on EEVblog, so to start editing a new reply
- save the reply webpage locally (i.e. with save as from the Firefox web browser file menu)
- open with Firefox the locally saved EEVblog reply page
- type the matjax in the offline saved reply page
- press preview to see the formula rendered

- important - to further edit or to copy the formula, press "Back" page in the browser, to go back to the offline reply page, then preview again and so on.  The formula is only rendered when pressing preview from a locally saved webpage.

Once a formula edited one way or another, copy/paste it in the "live" reply webpage.  Cumbersome and time consuming.



Did some experiments with the Peltz oscillator this weekend, both in simulation and in practice (for the fun of it, mostly out of curiosity, because I was not aware about this type of oscillator before, thank you for bringing it).

As everybody know, "a rainy Sunday afternoon" is best suitable to improve distortions in existing oscillator designs, and yesterday it was a rainy Sunday afternoon.  So I took advantage of that, and reduced even further the distortions for the Peltz oscillator by inventing the  Peltz-Wyatt  oscillator , if I may call it so.  It's a Peltz oscillator with a Wyatt current source instead of the resistor, signal much cleaner now. 

[mawyatt]

...
An important note regarding the waveform cycle unity gain requirement under steady state. An ideal oscillator eventually settles to a sinusoid with constant amplitude or:

Vo = V*{Exp(alpha*t)}Sin(omega*t), where alpha is identically zero under steady state and negative under waveform decay and positive under waveform expanding.

(Need to figure out how to enter proper equations like others use, MathJax or other method!!)

This forum supports MathJax, with formulas delimited by backslash dollar at both the beginning and the end of a formula (for inline formulas), i.e.  \$ V_o = Ve^{\alpha t}\sin(\omega t) \$ or backslash open-square-bracket at the beginning and backslash close-square-brackets at the end for formulas centered on a new line:   \[ V_o = Ve^{\alpha t}\sin(\omega t) \] where t is time ...

There is a small thread with examples of posting math on EEVblog:
https://www.eevblog.com/forum/beginners/how-does-posting-math-notation-work/msg3994178/#msg3994178

Thanks for the information on using MathJax, didn't know how this would be rendered here, now need to spend some time with this.

Did some experiments with the Peltz oscillator this weekend, both in simulation and in practice (for the fun of it, mostly out of curiosity, because I was not aware about this type of oscillator before, thank you for bringing it).

As everybody know, "a rainy Sunday afternoon" is best suitable to improve distortions in existing oscillator designs, and yesterday it was a rainy Sunday afternoon.  So I took advantage of that, and reduced even further the distortions for the Peltz oscillator by inventing the  Peltz-Wyatt  oscillator , if I may call it so.  It's a Peltz oscillator with a Wyatt current source instead of the resistor, signal much cleaner now. 

That's certainly a good use of the Wyatt current source, well done, and please show some of your measurement results 

Another reference for the current source from Harrison's book, Current Sources and Voltage References: A Design Reference for Electronics

https://books.google.com/books?id=03JmxpE39N4C&pg=PA87&lpg=PA87&dq=Wyatt+Current+Source&source=bl&ots=5zevJ8Ypzb&sig=ACfU3U3DvUbu9AotugZ_GWm2zi6zyEj6pA&hl=en&sa=X&ved=2ahUKEwicmoqB9Oj2AhWOSjABHRumDjYQ6AF6BAgYEAM#v=onepage&q=Wyatt%20Current%20Source&f=false

Best,

[RoGeorge]

please show some of your measurement results

This is the Peltz oscillator after adding the Wyatt current source.  The coil is from a former black and white TV (to adjust the vertical linearity IIRC), but I've removed the adjustable ferrite core, now it has ~16.9mH and 138 ohms, no magnetics.



When powered from a single 1.2V battery it measures about -29.7dB (3.39%) distortions at about 3555Hz.  Spectrum and distortions measured with the free baudline v1.08 software and the onboard Creative SoundCore3D audio card sampling at 24bits/96kHz (displayed dB are relative to 1V_RMS):


The hill in the background noise floor for frequencies above 25kHz is internal noise from the soundcard.  I don't know if the displayed THD includes the 50Hz hum and the noise, too, or only the fundamental and its harmonics.


The previous measurements last week were made by eyeballing at the FFT on the screen of my Rigol DS1054z oscilloscope, so not very precise.  With more precise measurement using the soundcard, I see no significant differences in distortions when the differential BJT pair of the Peltz osc is powered through a simple resistor vs a constant current source in their tail (for the same amplitude of the generated signal).

I think I might have measured something wrong last week, when I've observed reduced distortions after replacing the common emiters tail resistor with the current source. 

[mawyatt]

Nice 1.2V oscillator 

Best

[Kleinstein]

The current source instead of a simple resistor would allow to adjust the amplifier gain, e.g. in an loop to regulate the amplitude. This would be expected to also reduce the THD.
It was seen before that less current for the transistors (and thus less gain) gives lower distortion.

Another simple point to improve on the THD may be base resitstor, so that the clamping from the BE/BC diodes is not so hard, but more gradual.

[moffy]

We just had one of the main speakers at my church go silent, was thinking of a small battery test oscillator, I think I might try the Peltz.

[mawyatt]

Just for fun we did an analysis to find the minimum supply voltage to start/sustain oscillations for the Peltz oscillator. We were too lazy to use the Wyatt Current Source with the oscillator as RoGeorge did, and just used a 10K Resistor to the negative Vee supply.

10K Emitter Resistor was selected to allow a finer adjustment since the actual parameter being varied to start/sustain oscillations is the transistor transconductance which is Ic/Vt, where Vt is the thermal voltage kT/q, and by varying the supply voltage the transistor current is varied.

The Peltz oscillator was assembled on a plug-in Proto-Board with jumpers and a pair of 2N3904 transistors with a 100uH Inductor (99.28uH with Rp of 241 ohms at 16.3KHz) and 1uF Polyester Cap (963nF with Rp of 4.68K ohms) for a resonate frequency of ~16.3KHz. Measurement show oscillation start at ~5.75V Vee supply.

The analysis involves computing the supply voltage when the gain around the positive feedback loop formed by Q1 and Q2 equals unity and the solution goes transcendental which requires Netwon's Method or other Numerical Solution algorithms even when simple transistor models are assumed. Here's the solution found (later we'll try and make this nicer with MathJax when we figure out how to use such).

Vee > Vt [ 2 * ( R + Sqrt( R^2 + Z * R)) / Z  + ln {( Vee -Vbe)/(R * Is)} ]

Edit: Trying to use MathJax, shows OK on a interactive editor (see image)!!

\[V_{ee} > V_t \left( 2\cdot\left(\frac{R + \sqrt{R^2 + Z \cdot R}} {Z}\right) + \ln\left(\frac{V_{ee} - V_{be}} {R\cdot I_s}\right)\right)\]

Finally got the equation to render properly with the kind help from RoGeorge!!

Where Vt is the thermal voltage kT/q, Z is the total real impedance "seen" at the parallel resonate LC network and includes board loss, R is the emitter bias resistor, and Vbe is the base emitter voltage of Q1 which is Vt * Ln (Ic/Is), where Is is the bipolar saturation current. As you can see this isn't exactly a simple straight forward solution, and best left for a grad student 

However, a simple assumption can make the solution more amendable if one assumes a fixed value for Vbe, of say 0.65 volts. With this assumption and the values shown above with a small loss to account for board contact losses which makes Z ~ 215 ohms at the oscillator resonate frequency, we calculate a minimum Vee supply voltage of ~5.62 volts and measure ~5.75 volts which is ~ 255ua collector current for each transistor.

Anyway this was a fun exercise while "holding down the fort" here at home this afternoon. This Peltz oscillator is a fun little circuit and great for those folks that like to tinker around with electronics stuff!!!

Best,

[RoGeorge]

Trying to reproduce your formula, using this live rendering webpage:  https://arachnoid.com/latex/
The raw formula typed in the https://arachnoid.com/latex/ webpage was

Code: [Select]

\require{cancel} \xcancel{V_{ee} ~= V_t \cdot 2\left(R + \frac{\sqrt{R^2 + Z \cdot R}} {Z} + \ln\left(\frac{V_{ee} - V_{be}} {R+I_s}\right)\right)}then I've copy pasted it here, and added backslash square brackets at the beginning and at the end, in order to be rendered by the forum in display mode (centered in a new line).  This is how the formula edited live on https://arachnoid.com/latex/ renders here:  \[ \require{cancel} \xcancel{V_{ee} ~= V_t \cdot 2\left(R + \frac{\sqrt{R^2 + Z \cdot R}} {Z} + \ln\left(\frac{V_{ee} - V_{be}} {R+I_s}\right)\right)} \]  Thought, a photo of a handwritten formula on paper is much faster and less prone to typo errors.

As a side note, my Peltz-Wyatt oscillates just fine starting from anything above 0.7-0.8V but the amplitude is very small.  For example at 0.9V the sound card measures -100dBVrms, so about 25uVpp, and the DC level is very jumpy, so I can not use the oscilloscope in averaging mode.  Not sure if the signal jumps because of shot noises or because of the breadboard contacts, I suspect it's not the breadboard.  The attached spectrum is for Vcc = 0.9V, barely visible above the noise floor.

LATER EDIT:
-----------------
Added cross-strikeout because, by mistake, I've messed the parenthesis while editing the formula.  My bad, sorry.