On Tuesday, September 25, 2018 at 5:06:41 PM UTC+5:30, Steve Wilson wrote:
> 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.
That is fine. Both HSpice and Ngspice use text based input
netlists, which allows for efficient and intuitive circuit design. For example, a few weeks ago at work I was using Hspice to do some crosstalk simulations with a basic configuration of
of 3 microstrip lines, where each microstrip line consists of
1024 unit(series inductor, resistor, shunt capacitor, conductance) cells. Took me about 45 minutes to get the first
cut simulation running. I am absolutely sure it would have
taken me several hours with a GUI based simulator. I mean
just wiring up the whole setup would have been a challenge. .
Reply by ●September 27, 20182018-09-27
On Tuesday, September 25, 2018 at 9:00:34 PM UTC+5:30, Tim Williams wrote:
> <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/
Well, I am not sure what you mean by "backwards". I have in
the past used a dedicated ground pin for SUBCKTs both with
HSpice and Ngspice, but I do not think that made any obvious
difference in the performance.
Reply by Don KB7RPU●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.
> 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 bitrex●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 piglet●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 Tim Williams●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 Steve Wilson●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
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.
Reply by Tauno Voipio●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