Forums

Colpitts kick-start in LT Spice

Started by Unknown November 11, 2019
jlarkin@highlandsniptechnology.com wrote:

> On Tue, 12 Nov 2019 07:43:06 -0600, John S <Sophi.2@invalid.org> > wrote: > >>On 11/11/2019 9:28 PM, jlarkin@highlandsniptechnology.com wrote: >>> On Tue, 12 Nov 2019 01:36:13 -0000 (UTC), Steve Wilson <no@spam.com> >>> wrote: >>> >>>> John Larkin <jlarkin@highland_atwork_technology.com> wrote: >>>> >>>>> On Mon, 11 Nov 2019 12:19:12 -0800 (PST), Klaus Kragelund >>>>> <klauskvik@hotmail.com> wrote: >>>> >>>>>> Wow, 1 Henry and multiply farad caps, why are you not using real >>>>>> values? >>>> >>>>> It's normalized. Why not? >>>> >>>>>> AFAIR you need to have conditions for oscillation covered, >>>>>> specifically the gain setting of C1 and C2 >>>> >>>>> It's a perfectly fine oscillator with lots of gain. It just never >>>>> starts. >>>> >>>> Your model is broken. Use the PSPICE model. It self-starts. >>> >>> If any oscillator of this kind starts in simulation, something is >>> indeed broken. >>> >>> 0 multiplied exponentially is still 0. >>> >> >> >>In your sim, Remove the kickstart. Then set .tran 0 15000 0. >>It begins self-start at about 5k and reached full amplitude at about 8k.
>>You need more patience. It takes a while for an oscillator to start.
> With one set of values, the voltage at the top of the tank is -4 fV > and is absolutely flat.
The 2N7002 model can be different for each user. It is broken. Use the 2N7000 model from PSPICE.
On Tue, 12 Nov 2019 09:29:59 -0600, John S <Sophi.2@invalid.org>
wrote:

>On 11/12/2019 9:11 AM, jlarkin@highlandsniptechnology.com wrote: >> On Tue, 12 Nov 2019 07:43:06 -0600, John S <Sophi.2@invalid.org> >> wrote: >> >>> On 11/11/2019 9:28 PM, jlarkin@highlandsniptechnology.com wrote: >>>> On Tue, 12 Nov 2019 01:36:13 -0000 (UTC), Steve Wilson <no@spam.com> >>>> wrote: >>>> >>>>> John Larkin <jlarkin@highland_atwork_technology.com> wrote: >>>>> >>>>>> On Mon, 11 Nov 2019 12:19:12 -0800 (PST), Klaus Kragelund >>>>>> <klauskvik@hotmail.com> wrote: >>>>> >>>>>>> Wow, 1 Henry and multiply farad caps, why are you not using real values? >>>>> >>>>>> It's normalized. Why not? >>>>> >>>>>>> AFAIR you need to have conditions for oscillation covered, specifically >>>>>>> the gain setting of C1 and C2 >>>>> >>>>>> It's a perfectly fine oscillator with lots of gain. It just never >>>>>> starts. >>>>> >>>>> Your model is broken. Use the PSPICE model. It self-starts. >>>> >>>> If any oscillator of this kind starts in simulation, something is >>>> indeed broken. >>>> >>>> 0 multiplied exponentially is still 0. >>>> >>> >>> >>> In your sim, Remove the kickstart. Then set .tran 0 15000 0. >>> It begins self-start at about 5k and reached full amplitude at about 8k. >>> >>> You need more patience. It takes a while for an oscillator to start. >> >> With one set of values, the voltage at the top of the tank is -4 fV >> and is absolutely flat. >> > >You're doing something wrong. Try this... > >Version 4 >SHEET 1 1348 680 >WIRE 896 -144 672 -144 >WIRE 672 -80 672 -144 >WIRE 896 -32 896 -144 >WIRE 464 0 304 0 >WIRE 624 0 464 0 >WIRE 464 80 464 0 >WIRE 304 112 304 0 >WIRE 896 128 896 48 >WIRE 896 128 816 128 >WIRE 816 160 816 128 >WIRE 464 192 464 144 >WIRE 576 192 464 192 >WIRE 672 192 672 16 >WIRE 672 192 576 192 >WIRE 464 240 464 192 >WIRE 672 256 672 192 >WIRE 896 256 896 128 >WIRE 304 400 304 192 >WIRE 464 400 464 304 >WIRE 464 400 304 400 >WIRE 672 400 672 336 >WIRE 896 400 896 336 >WIRE 896 400 672 400 >WIRE 464 432 464 400 >FLAG 464 432 0 >FLAG 816 160 0 >FLAG 576 192 SRC >SYMBOL ind 288 96 R0 >WINDOW 0 54 39 Left 2 >WINDOW 3 60 70 Left 2 >SYMATTR InstName L1 >SYMATTR Value 1 >SYMBOL cap 448 80 R0 >WINDOW 0 51 20 Left 2 >WINDOW 3 59 54 Left 2 >SYMATTR InstName C1 >SYMATTR Value 1 >SYMBOL cap 448 240 R0 >WINDOW 0 51 20 Left 2 >WINDOW 3 59 54 Left 2 >SYMATTR InstName C2 >SYMATTR Value 5 >SYMBOL nmos 624 -80 R0 >WINDOW 0 90 24 Left 2 >WINDOW 3 70 58 Left 2 >SYMATTR InstName M1 >SYMATTR Value 2N7002 >SYMBOL res 656 240 R0 >WINDOW 0 61 43 Left 2 >WINDOW 3 60 78 Left 2 >SYMATTR InstName R1 >SYMATTR Value 500 >SYMBOL voltage 896 -48 R0 >WINDOW 0 49 45 Left 2 >WINDOW 3 48 80 Left 2 >SYMATTR InstName V1 >SYMATTR Value 20 >SYMBOL voltage 896 240 R0 >WINDOW 0 53 37 Left 2 >WINDOW 3 57 72 Left 2 >SYMATTR InstName V2 >SYMATTR Value 20 >TEXT -192 376 Left 2 !.tran 0 15000 0 >TEXT -192 272 Left 2 ;Colpitts Kick-Start >TEXT -168 312 Left 2 ;JL Nov 9 2019
You removed my time step. Set it to 1 ms and wait, very patiently, to see a beautiful bizarre startup that doesn't oscillate. With an unspecified time step, LT Spice LC tank frequencies are not very accurate. -- John Larkin Highland Technology, Inc lunatic fringe electronics
jlarkin@highlandsniptechnology.com wrote:

> On Tue, 12 Nov 2019 09:29:59 -0600, John S <Sophi.2@invalid.org> > wrote: > >>On 11/12/2019 9:11 AM, jlarkin@highlandsniptechnology.com wrote: >>> On Tue, 12 Nov 2019 07:43:06 -0600, John S <Sophi.2@invalid.org> >>> wrote: >>> >>>> On 11/11/2019 9:28 PM, jlarkin@highlandsniptechnology.com wrote: >>>>> On Tue, 12 Nov 2019 01:36:13 -0000 (UTC), Steve Wilson <no@spam.com> >>>>> wrote: >>>>> >>>>>> John Larkin <jlarkin@highland_atwork_technology.com> wrote: >>>>>> >>>>>>> On Mon, 11 Nov 2019 12:19:12 -0800 (PST), Klaus Kragelund >>>>>>> <klauskvik@hotmail.com> wrote: >>>>>> >>>>>>>> Wow, 1 Henry and multiply farad caps, why are you not using real >>>>>>>> values? >>>>>> >>>>>>> It's normalized. Why not? >>>>>> >>>>>>>> AFAIR you need to have conditions for oscillation covered, >>>>>>>> specifically the gain setting of C1 and C2 >>>>>> >>>>>>> It's a perfectly fine oscillator with lots of gain. It just never >>>>>>> starts. >>>>>> >>>>>> Your model is broken. Use the PSPICE model. It self-starts. >>>>> >>>>> If any oscillator of this kind starts in simulation, something is >>>>> indeed broken. >>>>> >>>>> 0 multiplied exponentially is still 0. >>>>> >>>> >>>> >>>> In your sim, Remove the kickstart. Then set .tran 0 15000 0. >>>> It begins self-start at about 5k and reached full amplitude at about >>>> 8k. >>>> >>>> You need more patience. It takes a while for an oscillator to start. >>> >>> With one set of values, the voltage at the top of the tank is -4 fV >>> and is absolutely flat. >>> >> >>You're doing something wrong. Try this... >> >>Version 4 >>SHEET 1 1348 680 >>WIRE 896 -144 672 -144 >>WIRE 672 -80 672 -144 >>WIRE 896 -32 896 -144 >>WIRE 464 0 304 0 >>WIRE 624 0 464 0 >>WIRE 464 80 464 0 >>WIRE 304 112 304 0 >>WIRE 896 128 896 48 >>WIRE 896 128 816 128 >>WIRE 816 160 816 128 >>WIRE 464 192 464 144 >>WIRE 576 192 464 192 >>WIRE 672 192 672 16 >>WIRE 672 192 576 192 >>WIRE 464 240 464 192 >>WIRE 672 256 672 192 >>WIRE 896 256 896 128 >>WIRE 304 400 304 192 >>WIRE 464 400 464 304 >>WIRE 464 400 304 400 >>WIRE 672 400 672 336 >>WIRE 896 400 896 336 >>WIRE 896 400 672 400 >>WIRE 464 432 464 400 >>FLAG 464 432 0 >>FLAG 816 160 0 >>FLAG 576 192 SRC >>SYMBOL ind 288 96 R0 >>WINDOW 0 54 39 Left 2 >>WINDOW 3 60 70 Left 2 >>SYMATTR InstName L1 >>SYMATTR Value 1 >>SYMBOL cap 448 80 R0 >>WINDOW 0 51 20 Left 2 >>WINDOW 3 59 54 Left 2 >>SYMATTR InstName C1 >>SYMATTR Value 1 >>SYMBOL cap 448 240 R0 >>WINDOW 0 51 20 Left 2 >>WINDOW 3 59 54 Left 2 >>SYMATTR InstName C2 >>SYMATTR Value 5 >>SYMBOL nmos 624 -80 R0 >>WINDOW 0 90 24 Left 2 >>WINDOW 3 70 58 Left 2 >>SYMATTR InstName M1 >>SYMATTR Value 2N7002 >>SYMBOL res 656 240 R0 >>WINDOW 0 61 43 Left 2 >>WINDOW 3 60 78 Left 2 >>SYMATTR InstName R1 >>SYMATTR Value 500 >>SYMBOL voltage 896 -48 R0 >>WINDOW 0 49 45 Left 2 >>WINDOW 3 48 80 Left 2 >>SYMATTR InstName V1 >>SYMATTR Value 20 >>SYMBOL voltage 896 240 R0 >>WINDOW 0 53 37 Left 2 >>WINDOW 3 57 72 Left 2 >>SYMATTR InstName V2 >>SYMATTR Value 20 >>TEXT -192 376 Left 2 !.tran 0 15000 0 >>TEXT -192 272 Left 2 ;Colpitts Kick-Start >>TEXT -168 312 Left 2 ;JL Nov 9 2019
> You removed my time step. Set it to 1 ms and wait, very patiently, to > see a beautiful bizarre startup that doesn't oscillate.
Doesn't start. 2N7002 models are bad. Here's the error log: Questionable use of curly braces in ".model sir870adp vdmos(rg=3 vto=2.9 rd=3.2m rs=1.5m rb={m} kp=100 mtriode=1.85 cgdmax=1.4n cgdmin=70p cgs=2.9n cjo=3.6n m=.4 a=.7 vj=.7 lambda=20m is=3p ksubthres=.08 mfg=siliconix vds= 100 ron=5.5m qg=53.5n)" Error: undefined symbol in: "[m]" Circuit: * C:\0DNLOAD\1.ASC Direct Newton iteration for .op point succeeded. Date: Tue Nov 12 12:22:34 2019 Total elapsed time: 150.536 seconds. tnom = 27 temp = 27 method = modified trap totiter = 30000048 traniter = 30000040 tranpoints = 15000021 accept = 15000021 rejected = 0 matrix size = 9 fillins = 2 solver = Normal Matrix Compiler1: off [1.9]/3.8/2.3 Matrix Compiler2: off [2.0]/3.2/22.1
On Monday, November 11, 2019 at 5:15:37 PM UTC-8, John Larkin wrote:

[about a Spice-model of oscillator]

> It's a perfectly fine oscillator with lots of gain. It just never > starts.
> It shouldn't start at all. There's no reason why it would prefer to > swing positive or negative to get going.
The REAL oscillator has thermal noise to start it. Even a wire has some Johnson noise. SPICE isn't equipped to handle that, in transient analysis.
whit3rd <whit3rd@gmail.com> wrote:

> On Monday, November 11, 2019 at 5:15:37 PM UTC-8, John Larkin wrote:
> [about a Spice-model of oscillator]
>> It's a perfectly fine oscillator with lots of gain. It just never >> starts.
>> It shouldn't start at all. There's no reason why it would prefer to >> swing positive or negative to get going.
> The REAL oscillator has thermal noise to start it. Even a wire > has some Johnson noise. SPICE isn't equipped to handle that, > in transient analysis.
JL is using the 2N7002 model, which is defective. If you use the 2N7000 model from PSPICE, it starts fine. LTspice supplies the initial conditions, and it runs from there. Version 4 SHEET 1 2804 680 WIRE 976 -144 816 -144 WIRE 816 -80 816 -144 WIRE 976 -32 976 -144 WIRE 368 0 320 0 WIRE 640 0 480 0 WIRE 688 0 640 0 WIRE 768 0 688 0 WIRE 368 80 368 0 WIRE 640 80 640 0 WIRE 320 96 320 0 WIRE 480 112 480 0 WIRE 976 128 976 48 WIRE 976 128 896 128 WIRE 896 160 896 128 WIRE 640 192 640 144 WIRE 688 192 640 192 WIRE 816 192 816 16 WIRE 816 192 688 192 WIRE 640 240 640 192 WIRE 816 256 816 192 WIRE 976 256 976 128 WIRE 320 400 320 176 WIRE 480 400 480 192 WIRE 480 400 320 400 WIRE 640 400 640 304 WIRE 640 400 480 400 WIRE 816 400 816 336 WIRE 976 400 976 336 WIRE 976 400 816 400 WIRE 640 432 640 400 FLAG 688 0 OSC FLAG 640 432 0 FLAG 896 160 0 FLAG 688 192 SRC FLAG 368 80 0 SYMBOL ind 464 96 R0 WINDOW 0 54 39 Left 2 WINDOW 3 60 70 Left 2 SYMATTR InstName L1 SYMATTR Value 1 SYMATTR SpiceLine Rser=1m SYMBOL cap 624 80 R0 WINDOW 0 51 20 Left 2 WINDOW 3 59 54 Left 2 SYMATTR InstName C1 SYMATTR Value 1 SYMBOL current 320 176 R180 WINDOW 0 63 41 Left 2 WINDOW 3 -214 220 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName I1 SYMATTR Value PULSE(0 1 100 1m 1m 50m) SYMBOL cap 624 240 R0 WINDOW 0 51 20 Left 2 WINDOW 3 59 54 Left 2 SYMATTR InstName C2 SYMATTR Value 5 SYMBOL nmos 768 -80 R0 WINDOW 0 90 24 Left 2 WINDOW 3 70 58 Left 2 SYMATTR InstName M1 SYMATTR Value 2N7000 SYMBOL res 800 240 R0 WINDOW 0 61 43 Left 2 WINDOW 3 60 78 Left 2 SYMATTR InstName R1 SYMATTR Value 500 SYMBOL voltage 976 -48 R0 WINDOW 0 49 45 Left 2 WINDOW 3 48 80 Left 2 SYMATTR InstName V1 SYMATTR Value 20 SYMBOL voltage 976 240 R0 WINDOW 0 53 37 Left 2 WINDOW 3 57 72 Left 2 SYMATTR InstName V2 SYMATTR Value 20 TEXT 456 -136 Left 2 !.tran 0 20 0 1m TEXT 456 -168 Left 2 ;'2N7000 Colpitts Self-Start TEXT 328 464 Left 2 !* PWRMOS.LIB \n* NOT SPICE 2G.6 Compatible. FOR USE WITH MICROSIM PSPICE\n.model 2n7000 NMOS(Level=3 Gamma=0 Delta=0 Eta=0 Theta=0 Kappa=0.2 Vmax=0 Xj=0 Phi=.6 Kp=1.073u W=.12 L=2u Rs=20m Vto=1.73 Rd=.5489 Rds=48MEG Cgso=73.61p Cgdo=6.487p Cbd=74.46p Mj=.5 Pb=.8 Fc=.5 Rg= 546.2 Is=10f N=1 Rb=1m) [Transient Analysis] { Npanes: 1 { traces: 1 {524291,0,"V(osc)"} X: (' ',0,0,2,20) Y[0]: ('p',0,-1e-009,2e-010,1e-009) Y[1]: ('_',0,1e+308,0,-1e+308) Volts: ('p',0,0,1,-1e-009,2e-010,1e-009) Log: 0 0 0 GridStyle: 1 } }
On 11/12/2019 10:48 AM, jlarkin@highlandsniptechnology.com wrote:

> You removed my time step. Set it to 1 ms and wait, very patiently, to > see a beautiful bizarre startup that doesn't oscillate.
Why?
> With an unspecified time step, LT Spice LC tank frequencies are not > very accurate.
What kind of not accurate? Frequency, voltage, etc? Please specify. And how do you know about very accurate? Have you built them to verify? I showed you that your own model self-starts in LTSpice without a kickstart. You said it never would, but it does. You never mentioned accuracy. Build one and bench test it. Report back here with your results. Be honest and don't change the stream in the middle of a horse.
On Tue, 12 Nov 2019 14:04:56 -0600, John S <Sophi.2@invalid.org>
wrote:

>On 11/12/2019 10:48 AM, jlarkin@highlandsniptechnology.com wrote: > >> You removed my time step. Set it to 1 ms and wait, very patiently, to >> see a beautiful bizarre startup that doesn't oscillate. > >Why? > >> With an unspecified time step, LT Spice LC tank frequencies are not >> very accurate. > >What kind of not accurate? Frequency, voltage, etc? Please specify.
Frequency.
>And how do you know about very accurate? Have you built them to verify?
Built? I compare the LT spice frequency to the calculated value. Even bare LCs are a bit wrong at the default settings.
> >I showed you that your own model self-starts in LTSpice without a >kickstart. You said it never would, but it does. You never mentioned >accuracy. Build one and bench test it. Report back here with your >results. Be honest and don't change the stream in the middle of a horse.
The issue isn't bench testing, it is the hazards of LT Spice, and the general weirdness of numerical simulation of physical systems. It used to be that LT Spice wouldn't allow you to run if one end of a capacitor was open, or if you have two caps in series. Now it does. -- John Larkin Highland Technology, Inc picosecond timing precision measurement jlarkin att highlandtechnology dott com http://www.highlandtechnology.com
On 12/11/19 10:51 pm, Jeroen Belleman wrote:
> A real oscillator will start up just fine, but a simulation may or > may not. Either way, it would be wrong to take this as a model of > reality. You *must* kick-start an oscillator simulation.
I have both simulated and built quite a few oscillators using LTSpice, allowing them to start by amplifying the noise in the models. Anything reasonable seems to start in LTSpice and in real life, once you get the gain and phase right. I've never used a kick-start in any case.
John Larkin <jlarkin@highland_atwork_technology.com> wrote:

> On Tue, 12 Nov 2019 14:04:56 -0600, John S <Sophi.2@invalid.org> > wrote: > >>On 11/12/2019 10:48 AM, jlarkin@highlandsniptechnology.com wrote: >> >>> You removed my time step. Set it to 1 ms and wait, very patiently, to >>> see a beautiful bizarre startup that doesn't oscillate. >> >>Why? >> >>> With an unspecified time step, LT Spice LC tank frequencies are not >>> very accurate. >> >>What kind of not accurate? Frequency, voltage, etc? Please specify. > > Frequency. > >>And how do you know about very accurate? Have you built them to verify? > > Built? I compare the LT spice frequency to the calculated value. Even > bare LCs are a bit wrong at the default settings.
If you are referring to the test you did on July, 2015, you compared the amplitudes of a shocked LC circuit and a generated sine wave. you ignored the fact that the inductor ESR defaults to 1 milliohm unless you specify otherwise. As you ran the sym, the LC amplitude decayed. You took the difference in amplitudes between the LC and generated sine waves and found a difference. How you translated that into a percentage frequency error I'll never know. Also, you have to set an appropriate timestep. If you don't specify any timestep, the sym produces garbage. Here is your statement from July, 2015:
> LT Spice goes for sim speed, so it tends to use coarse time steps. If > you shock a simple LC and let it ring, at default settings the > resonant frequency will be off by percentages. Similarly, oscillator > sims will be unrealistic.
This is in "SPICE tarnsient analysis of oscillators - sampling time" https://groups.google.com/forum/?hl=en#! searchin/sci.electronics.design/steve$20wilson$20larkin$20lc$20accuracy% 7Csort:date/sci.electronics.design/4cScUlUOldk/3zQjf2pFAwAJ I posted a LTspice file with an appropriate inductor ESR and timestep that showed the frequency error is in the parts per billion. It is difficult to measure. And you still go around spouting false information. LTspice can give very accurate answers if you give it correct data. GIGO. Here is the sym: Version 4 SHEET 1 880 680 WIRE 224 -192 64 -192 WIRE 416 -192 224 -192 WIRE 480 -192 416 -192 WIRE 64 -112 64 -192 WIRE 416 -32 336 -32 WIRE 480 -32 416 -32 WIRE 336 -16 336 -32 WIRE 224 0 224 -192 WIRE 288 0 224 0 WIRE 64 16 64 -32 WIRE 288 48 224 48 WIRE 224 112 224 48 WIRE 224 112 64 112 WIRE 320 112 224 112 WIRE 416 112 320 112 WIRE 480 112 416 112 WIRE 64 160 64 112 WIRE 320 160 320 112 WIRE 224 176 224 112 WIRE 64 288 64 240 WIRE 224 288 224 240 WIRE 320 288 320 240 FLAG 224 288 0 FLAG 320 288 0 FLAG 64 288 0 FLAG 64 16 0 FLAG 336 64 0 FLAG 416 -32 DIFF FLAG 416 -192 IDEAL FLAG 416 112 LC SYMBOL ind 304 144 R0 WINDOW 0 46 29 Left 2 WINDOW 3 50 62 Left 2 SYMATTR InstName L1 SYMATTR Value 0.1591549430918953357688837634 SYMATTR SpiceLine Rser=1u Cpar=1p SYMBOL cap 208 176 R0 WINDOW 0 24 -3 Left 2 WINDOW 3 -84 189 Left 2 SYMATTR InstName C1 SYMATTR Value 0.1591549430918953357688837634 SYMATTR SpiceLine Rser=1n Lser=1p SYMBOL current 64 160 R0 WINDOW 0 -70 50 Left 2 WINDOW 3 -165 99 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName I1 SYMATTR Value PULSE(1 0 0.5) SYMBOL voltage 64 -128 R0 WINDOW 0 -109 61 Left 2 WINDOW 3 -188 104 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V1 SYMATTR Value SINE(0 1 1 0.5) SYMBOL e 336 -32 R0 WINDOW 0 60 40 Left 2 WINDOW 3 53 74 Left 2 SYMATTR InstName E1 SYMATTR Value -1 TEXT 16 -232 Left 2 !.tran 0 1000 0 100u TEXT 16 -264 Left 2 ;'LTSpice Compare LC Frequencies Larkin July 2015 TEXT 592 -232 Left 2 !.options numdgt=15 TEXT 264 -168 Left 2 ;Can't tell if frequency is changing or\ntank amplitude is dropping. A frequency\ndifference will case a linear ramp. Exponential\ndecay due to Q will cause an exponential rise. Here is the PLT file: [Transient Analysis] { Npanes: 3 Active Pane: 1 { traces: 1 {524292,0,"V(ideal)"} X: ('K',3,2304,3,2334) Y[0]: (' ',1,-1,0.2,1) Y[1]: ('_',0,1e+308,0,-1e+308) Volts: (' ',0,0,1,-1,0.2,1) Log: 0 0 0 GridStyle: 1 }, { traces: 1 {268959746,0,"V(lc)"} X: ('K',3,2304,3,2334) Y[0]: ('&#2013266101;',0,-0.0008,0.0001,0.0008) Y[1]: ('_',0,1e+308,0,-1e+308) Volts: ('&#2013266101;',0,0,0,-0.0008,0.0001,0.0008) Log: 0 0 0 GridStyle: 1 }, { traces: 1 {268959747,0,"V(diff)"} X: ('K',3,2304,3,2334) Y[0]: (' ',0,-100,20,100) Y[1]: ('_',0,1e+308,0,-1e+308) Volts: (' ',0,0,0,-100,20,100) Log: 0 0 0 GridStyle: 1 } }
Steve Wilson <no@spam.com> wrote:

> Here is the sym:
Rats. Line wrap kills the file. Here is the fixed version: Version 4 SHEET 1 880 680 WIRE 224 -192 64 -192 WIRE 416 -192 224 -192 WIRE 480 -192 416 -192 WIRE 64 -112 64 -192 WIRE 416 -32 336 -32 WIRE 480 -32 416 -32 WIRE 336 -16 336 -32 WIRE 224 0 224 -192 WIRE 288 0 224 0 WIRE 64 16 64 -32 WIRE 288 48 224 48 WIRE 224 112 224 48 WIRE 224 112 64 112 WIRE 320 112 224 112 WIRE 416 112 320 112 WIRE 480 112 416 112 WIRE 64 160 64 112 WIRE 320 160 320 112 WIRE 224 176 224 112 WIRE 64 288 64 240 WIRE 224 288 224 240 WIRE 320 288 320 240 FLAG 224 288 0 FLAG 320 288 0 FLAG 64 288 0 FLAG 64 16 0 FLAG 336 64 0 FLAG 416 -32 DIFF FLAG 416 -192 IDEAL FLAG 416 112 LC SYMBOL ind 304 144 R0 WINDOW 0 46 29 Left 2 WINDOW 3 50 62 Left 2 SYMATTR InstName L1 SYMATTR Value 0.1591549430918953357688837634 SYMATTR SpiceLine Rser=1u Cpar=1p SYMBOL cap 208 176 R0 WINDOW 0 24 -3 Left 2 WINDOW 3 -84 189 Left 2 SYMATTR InstName C1 SYMATTR Value 0.1591549430918953357688837634 SYMATTR SpiceLine Rser=1n Lser=1p SYMBOL current 64 160 R0 WINDOW 0 -70 50 Left 2 WINDOW 3 -165 99 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName I1 SYMATTR Value PULSE(1 0 0.5) SYMBOL voltage 64 -128 R0 WINDOW 0 -109 61 Left 2 WINDOW 3 -188 104 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V1 SYMATTR Value SINE(0 1 1 0.5) SYMBOL e 336 -32 R0 WINDOW 0 60 40 Left 2 WINDOW 3 53 74 Left 2 SYMATTR InstName E1 SYMATTR Value -1 TEXT 16 -232 Left 2 !.tran 0 1000 0 100u TEXT 16 -264 Left 2 ;'LTSpice Compare LC Frequencies Larkin July 2015 TEXT 592 -232 Left 2 !.options numdgt=15
> Here is the PLT file: > > [Transient Analysis] > { > Npanes: 3 > Active Pane: 1 > { > traces: 1 {524292,0,"V(ideal)"} > X: ('K',3,2304,3,2334) > Y[0]: (' ',1,-1,0.2,1) > Y[1]: ('_',0,1e+308,0,-1e+308) > Volts: (' ',0,0,1,-1,0.2,1) > Log: 0 0 0 > GridStyle: 1 > }, > { > traces: 1 {268959746,0,"V(lc)"} > X: ('K',3,2304,3,2334) > Y[0]: ('&#2013266101;',0,-0.0008,0.0001,0.0008) > Y[1]: ('_',0,1e+308,0,-1e+308) > Volts: ('&#2013266101;',0,0,0,-0.0008,0.0001,0.0008) > Log: 0 0 0 > GridStyle: 1 > }, > { > traces: 1 {268959747,0,"V(diff)"} > X: ('K',3,2304,3,2334) > Y[0]: (' ',0,-100,20,100) > Y[1]: ('_',0,1e+308,0,-1e+308) > Volts: (' ',0,0,0,-100,20,100) > Log: 0 0 0 > GridStyle: 1 > } > } >