Could some electronics guru on this group please help ? I am trying to set up a SPICE simulation for an Armstrong oscillator. The problem seems to be with designing the transformer and/or excitation coil. Are there any good tutorials or related material online. Any hints/ suggestions would be of immense help. Thanks in advance.
Transformer/excitation coil for Armstrong oscillator
Started by ●September 24, 2018
Reply by ●September 25, 20182018-09-25
On Monday, September 24, 2018 at 6:29:25 AM UTC-4, daku...@gmail.com wrote:> Could some electronics guru on this group please help ? I am trying to set up a SPICE simulation for an Armstrong oscillator. The problem seems to be with designing the transformer and/or excitation coil. > Are there any good tutorials or related material online. Any hints/ > suggestions would be of immense help. Thanks in advance.Should be easy. Assuming you are using LTspice, post your ASC file. I'll see if I can help.
Reply by ●September 25, 20182018-09-25
On 24.9.18 13:29, dakupoto@gmail.com wrote:> Could some electronics guru on this group please help ? I am trying to set up a SPICE simulation for an Armstrong oscillator. The problem seems to be with designing the transformer and/or excitation coil. > Are there any good tutorials or related material online. Any hints/ > suggestions would be of immense help. Thanks in advance.Please note that a simulation is often so stable that an oscillator will not start by itself. To make it start, there needs to be a disturbance in the form of an initial condition. -- -TV
Reply by ●September 25, 20182018-09-25
On Tuesday, September 25, 2018 at 1:11:19 PM UTC+5:30, Steve Wilson wrote:> On Monday, September 24, 2018 at 6:29:25 AM UTC-4, daku...@gmail.com wrote: > > Could some electronics guru on this group please help ? I am trying to set up a SPICE simulation for an Armstrong oscillator. The problem seems to be with designing the transformer and/or excitation coil. > > Are there any good tutorials or related material online. Any hints/ > > suggestions would be of immense help. Thanks in advance. > > Should be easy. Assuming you are using LTspice, post your ASC file. I'll see if I can help.I use Ngspice The netlist is below .PARAMS C=1.0E-7 C1=1.0E-6 L0=1.0E-6 L1=0.43E-6 .PARAMS FLLIM=1.0E+4 FHLIM=1.0E+7 AMPL=15.0 F=5.0E+5 .MODEL BC547B NPN(IS=5.5e-16 VAF=112 BF=265 BR=5 IKF=.22 RC=1 CJC=4.5p CJE=12p TR=500n TF=500p RCO=27.65 GAMMA=1.75e-9 VO=2.74) ** THERE ADVANCED MODELS OF BC547B .SUBCKT amplifierceM 1 2 3 ** 1 VCC ** 2 BASE TRIGGER IN ** 3 OUT C0 3 4 {C1} C1 2 5 {C1} C2 6 9 {C1} Q0 4 5 6 BC547B RC 1 4 12.0 RE 6 0 4.0 RB1 1 5 1.0K RB2 5 0 250.0 .ENDS .SUBCKT LCTANK 1 2 ** 1 VCC ** 2 OUT C0 1 0 {C} L0 3 0 {L0} L1 2 0 {L0} k0 L0 L1 0.99 R0 1 3 1.0u .ENDS * TRANSIENT ANALYSIS VCC 1 0 DC {AMPL} AC 0.0 ** OSCILLATOR TEST XCE 1 2 3 amplifierceM XLC 3 2 LCTANK .OPTIONS METHOD=GEAR NOPAGE RELTOL=1m MINBREAK=5ps ** TRANSIENT ANALYSIS .IC V(2)=12.0 V(3)=10 .TRAN 1u 102.05ms 100ms 100n UIC .PRINT TRAN V(2) V(3) .END
Reply by ●September 25, 20182018-09-25
On Tuesday, September 25, 2018 at 5:44:30 AM UTC-4, daku...@gmail.com wrote:> On Tuesday, September 25, 2018 at 1:11:19 PM UTC+5:30, Steve Wilson wrote: > > On Monday, September 24, 2018 at 6:29:25 AM UTC-4, daku...@gmail.com wrote: > > > Could some electronics guru on this group please help ? I am trying to set up a SPICE simulation for an Armstrong oscillator. The problem seems to be with designing the transformer and/or excitation coil. > > > Are there any good tutorials or related material online. Any hints/ > > > suggestions would be of immense help. Thanks in advance. > > > > Should be easy. Assuming you are using LTspice, post your ASC file. I'll see if I can help. > > I use Ngspice The netlist is below >Sorry, I use LTspice. I don't have time to translate your netlist.
Reply by ●September 25, 20182018-09-25
<dakupoto@gmail.com> wrote in message news:7d529c91-326c-4792-b646-98cb0c021df9@googlegroups.com...> I use Ngspice The netlist is below ><snip> This is all backwards. It's also not recommended to use SUBCKTs that don't conserve current (i.e., they are all using the implicit global node 0 for ground, instead of connecting it through a pin). Compare the Armstrong circuit to the netlist, and doublecheck device pin orders if necessary. You also have unused PARAMs, which may be confusing. Tim -- Seven Transistor Labs, LLC Electrical Engineering Consultation and Design Website: https://www.seventransistorlabs.com/
Reply by ●September 25, 20182018-09-25
On 09/25/2018 04:38 AM, Tauno Voipio wrote:> On 24.9.18 13:29, dakupoto@gmail.com wrote: >> Could some electronics guru on this group please help ? I am trying to >> set up a SPICE simulation for an Armstrong oscillator. The problem >> seems to be with designing the transformer and/or excitation coil. >> Are there any good tutorials or related material online. Any hints/ >> suggestions would be of immense help. Thanks in advance. > > > Please note that a simulation is often so stable that > an oscillator will not start by itself. To make it start, > there needs to be a disturbance in the form of an initial > condition. >In LTSpice hitting the switch that makes the power supply voltage start at 0 V and select "skip initial operating point solution" is often enough to get LC oscillators going. If it's still hard to get an LC started after that it will be persnickity in the real world, too, in my experience
Reply by ●September 25, 20182018-09-25
On 25/09/2018 10:44, dakupoto@gmail.com wrote:> On Tuesday, September 25, 2018 at 1:11:19 PM UTC+5:30, Steve Wilson wrote: >> On Monday, September 24, 2018 at 6:29:25 AM UTC-4, daku...@gmail.com wrote: >>> Could some electronics guru on this group please help ? I am trying to set up a SPICE simulation for an Armstrong oscillator. The problem seems to be with designing the transformer and/or excitation coil. >>> Are there any good tutorials or related material online. Any hints/ >>> suggestions would be of immense help. Thanks in advance. >> >> Should be easy. Assuming you are using LTspice, post your ASC file. I'll see if I can help. > > I use Ngspice The netlist is below > > > > > .PARAMS C=1.0E-7 C1=1.0E-6 L0=1.0E-6 L1=0.43E-6 > .PARAMS FLLIM=1.0E+4 FHLIM=1.0E+7 AMPL=15.0 F=5.0E+5 > > .MODEL BC547B NPN(IS=5.5e-16 VAF=112 BF=265 BR=5 IKF=.22 RC=1 CJC=4.5p CJE=12p TR=500n TF=500p RCO=27.65 GAMMA=1.75e-9 VO=2.74) > > ** THERE ADVANCED MODELS OF BC547B > > > .SUBCKT amplifierceM 1 2 3 > ** 1 VCC > ** 2 BASE TRIGGER IN > ** 3 OUT > C0 3 4 {C1} > C1 2 5 {C1} > C2 6 9 {C1} > Q0 4 5 6 BC547B > RC 1 4 12.0 > RE 6 0 4.0 > RB1 1 5 1.0K > RB2 5 0 250.0 > .ENDS > > .SUBCKT LCTANK 1 2 > ** 1 VCC > ** 2 OUT > C0 1 0 {C} > L0 3 0 {L0} > L1 2 0 {L0} > k0 L0 L1 0.99 > R0 1 3 1.0u > .ENDS > > > * TRANSIENT ANALYSIS > VCC 1 0 DC {AMPL} AC 0.0 > > ** OSCILLATOR TEST > XCE 1 2 3 amplifierceM > XLC 3 2 LCTANK > > .OPTIONS METHOD=GEAR NOPAGE RELTOL=1m MINBREAK=5ps > ** TRANSIENT ANALYSIS > .IC V(2)=12.0 V(3)=10 > .TRAN 1u 102.05ms 100ms 100n UIC > .PRINT TRAN V(2) V(3) > .END >I don't know Ngspice, here is a very quick and dirty LTspice Armstrong oscillator completely unoptimised that I put together in just a few minutes, if you can run LT spice then you can have fun playing with it and trying different values etc. You may also find it fun to move the tuned circuit to the collector and feedback winding to the base (that is no longer strictly an Armstrong oscillator and purists would call that a Meissner circuit). Enjoy ... Version 4 SHEET 1 880 680 WIRE 176 -96 -16 -96 WIRE 496 -96 176 -96 WIRE -16 -48 -16 -96 WIRE 176 -32 176 -96 WIRE -16 80 -16 32 WIRE -16 80 -144 80 WIRE -144 128 -144 80 WIRE 496 144 496 -96 WIRE 176 160 176 48 WIRE -16 208 -16 80 WIRE 112 208 -16 208 WIRE -144 224 -144 192 WIRE -144 224 -192 224 WIRE -112 224 -144 224 WIRE -192 272 -192 224 WIRE -112 288 -112 224 WIRE -16 288 -16 208 WIRE 176 288 176 256 WIRE 288 288 176 288 WIRE 176 320 176 288 WIRE 288 336 288 288 WIRE -192 416 -192 352 WIRE -112 416 -112 352 WIRE -112 416 -192 416 WIRE -16 416 -16 368 WIRE -16 416 -112 416 WIRE 176 416 176 400 WIRE 176 416 -16 416 WIRE 288 416 288 400 WIRE 288 416 176 416 WIRE 496 416 496 224 WIRE 496 416 288 416 WIRE 496 464 496 416 FLAG 496 464 0 SYMBOL npn 112 160 R0 SYMATTR InstName Q1 SYMATTR Value BC547B SYMBOL res 160 304 R0 SYMATTR InstName R1 SYMATTR Value 220 SYMBOL res -32 272 R0 SYMATTR InstName R2 SYMATTR Value 10k SYMBOL res -32 -64 R0 SYMATTR InstName R3 SYMATTR Value 10k SYMBOL ind2 160 -48 R0 SYMATTR InstName L1 SYMATTR Value 10µ SYMATTR Type ind SYMBOL ind2 -208 256 R0 SYMATTR InstName L2 SYMATTR Value 2µ SYMATTR Type ind SYMBOL cap -128 288 R0 SYMATTR InstName C1 SYMATTR Value 1n SYMBOL cap 272 336 R0 SYMATTR InstName C2 SYMATTR Value 100n SYMBOL voltage 496 128 R0 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V1 SYMATTR Value 9 SYMBOL cap -160 128 R0 SYMATTR InstName C3 SYMATTR Value 100n TEXT 280 -16 Left 2 !K1 L1 L2 0.95 TEXT -206 488 Left 2 !.tran 500u piglet
Reply by ●September 25, 20182018-09-25
On 24/09/2018 11:29, dakupoto@gmail.com wrote:> Could some electronics guru on this group please help ? I am trying to set up a SPICE simulation for an Armstrong oscillator. The problem seems to be with designing the transformer and/or excitation coil. > Are there any good tutorials or related material online. Any hints/ > suggestions would be of immense help. Thanks in advance. > >Irving Gottlieb wrote a book "Understanding Oscillators" or "Practical Oscillator HandbooK" that explains the various modes very clearly and why the Hartley circuit (of which Armstrong is a type) behaves differently from the other fundamental Colpitts class. Don't know if available online but some libraries should have them. piglet
Reply by ●September 25, 20182018-09-25
piglet <erichpwagner@hotmail.com> wrote:> On 24/09/2018 11:29, dakupoto@gmail.com wrote: >> Could some electronics guru on this group please help ? I am trying >> to set up a SPICE simulation for an Armstrong oscillator. The problem >> seems to be with designing the transformer and/or excitation coil. >> Are there any good tutorials or related material online. Any hints/ >> suggestions would be of immense help. Thanks in advance. >> >> > > Irving Gottlieb wrote a book "Understanding Oscillators" or "Practical > Oscillator HandbooK" that explains the various modes very clearly and > why the Hartley circuit (of which Armstrong is a type) behaves > differently from the other fundamental Colpitts class. Don't know if > available online but some libraries should have them.Here's a link to an online version of the Handbook: https://www.qsl.net/pa2efr/manuals/Doc/Practical%20Oscillator%20Handbook%201997-Irving%20M%20Gottlieb.pdf Here's some links about the Armstrong oscillator: https://duckduckgo.com/?q=armstrong+oscillator+site:qsl.net Thank you, 73, -- Don, KB7RPU There was a young lady named Bright Whose speed was far faster than light; She set out one day In a relative way And returned on the previous night.
