On Fri, 30 May 2014 07:49:46 -0700, RobertMacy wrote:

> As you can see by the 'credits' left in those two, not mine. But thanks  
> for the heads up on shifted sine wave.
> 
> Jim Thompsons touts using tanh. Tried it and now use a multiplying tanh  
> function to 'ramp up' any signals to not upset the initial parts of the  
> .tran analyses. Usng tanh totally solved the startup problem of a slew  
> rate limit analysis, after combining the tanh with the 'delayed recording'

I only see a credit on one of the examples.

Sorry about the rewrap on the subcircuit, BTW. I try not to do that.

-- 
"Design is the reverse of analysis"
                   (R.D. Middlebrook)

On Fri, 30 May 2014 19:35:48 -0700, josephkk wrote:

> OK.  But i would use and ".ic" statement instead.

I must try that. As a guess, I think it will just put a starting offset on
the source. We'll see. The main raison d'&ecirc;tre is to avoid the initial
current surge in an inductor when zero switching. Specifying 90 degrees
shift in the source doesn't do it.

It's caused to the, so-often-forgotten-by-undergrads, "constant of
integration" :-)

-- 
"Design is the reverse of analysis"
                   (R.D. Middlebrook)

On Fri, 30 May 2014 04:17:32 -0700, Fred Abse
<excretatauris@invalid.invalid> wrote:

>On Wed, 28 May 2014 16:20:51 -0700, RobertMacy wrote:
>
>> On Wed, 28 May 2014 15:28:36 -0700, Maynard A. Philbrook Jr.
>> <jamie_ka1lpa@charter.net> wrote:
>>=20
>>=20
>>>
>>>  How do I use John chan L model on the form in Ltspice?
>>>
>>>  I can't seem to find a way to instruct LTspice to use
>>> it over the standard?
>>>
>>>   I looked for a model card to use but I don't see it
>>> what I was looking for?
>>>
>>>  All it shows is how to do it in at the text file level, I
>>> want to do it on the form? Or do I need to write an include file for
>>> that specific L? If so, then I assume when using the mutual =
inductances
>>> (transformer stuff) it'll understand it?
>>>
>>>
>>> Jamie
>>=20
>> watch out for word wraps
>
><LTspice listing snipped>
>
>Hingteresing...
>
>One thing. Specifying a sine voltage at 90 degrees, in Spice, doesn't =
get
>you quite what you think it might (switchon at peak?). Been caught that
>way myself.
>
>To get switchon at a peak, I use this "peaksine" subcircuit:
>
>*Peaksine.sub
>*Params: f - frequency, V - Peak Voltage .subckt peaksine Hi Lo
>V1 N001 Lo SINE(0 {V} {f} 0 0 90) Rser=3D0 S1 Hi N001 N002 Lo Peak
>V2 N002 Lo PULSE(0 1 {1/f} 1n 1n)
>.model Peak sw (Ron=3D1p Roff=3D1t Vt=3D0.5 Vh=3D0) .ends
>
>Try it, it makes a difference.

OK.  But i would use and ".ic" statement instead.

?-)
=20

On Fri, 30 May 2014 04:17:32 -0700, Fred Abse  
<excretatauris@invalid.invalid> wrote:

>> ...snip....
>
> Hingteresing...
>
> One thing. Specifying a sine voltage at 90 degrees, in Spice, doesn't get
> you quite what you think it might (switchon at peak?). Been caught that
> way myself.
>
> To get switchon at a peak, I use this "peaksine" subcircuit:
>
> *Peaksine.sub
> *Params: f - frequency, V - Peak Voltage .subckt peaksine Hi Lo
> V1 N001 Lo SINE(0 {V} {f} 0 0 90) Rser=0 S1 Hi N001 N002 Lo Peak
> V2 N002 Lo PULSE(0 1 {1/f} 1n 1n)
> .model Peak sw (Ron=1p Roff=1t Vt=0.5 Vh=0) .ends
>
> Try it, it makes a difference.
>

As you can see by the 'credits' left in those two, not mine. But thanks  
for the heads up on shifted sine wave.

Jim Thompsons touts using tanh. Tried it and now use a multiplying tanh  
function to 'ramp up' any signals to not upset the initial parts of the  
.tran analyses. Usng tanh totally solved the startup problem of a slew  
rate limit analysis, after combining the tanh with the 'delayed recording'

On Wed, 28 May 2014 16:20:51 -0700, RobertMacy wrote:

> On Wed, 28 May 2014 15:28:36 -0700, Maynard A. Philbrook Jr.
> <jamie_ka1lpa@charter.net> wrote:
> 
> 
>>
>>  How do I use John chan L model on the form in Ltspice?
>>
>>  I can't seem to find a way to instruct LTspice to use
>> it over the standard?
>>
>>   I looked for a model card to use but I don't see it
>> what I was looking for?
>>
>>  All it shows is how to do it in at the text file level, I
>> want to do it on the form? Or do I need to write an include file for
>> that specific L? If so, then I assume when using the mutual inductances
>> (transformer stuff) it'll understand it?
>>
>>
>> Jamie
> 
> watch out for word wraps

<LTspice listing snipped>

Hingteresing...

One thing. Specifying a sine voltage at 90 degrees, in Spice, doesn't get
you quite what you think it might (switchon at peak?). Been caught that
way myself.

To get switchon at a peak, I use this "peaksine" subcircuit:

*Peaksine.sub
*Params: f - frequency, V - Peak Voltage .subckt peaksine Hi Lo
V1 N001 Lo SINE(0 {V} {f} 0 0 90) Rser=0 S1 Hi N001 N002 Lo Peak
V2 N002 Lo PULSE(0 1 {1/f} 1n 1n)
.model Peak sw (Ron=1p Roff=1t Vt=0.5 Vh=0) .ends

Try it, it makes a difference.

-- 
"Design is the reverse of analysis"
                   (R.D. Middlebrook)

In article <op.xgle42o22cx0wh@ajm>, robert.a.macy@gmail.com says...
> >
> >  How do I use John chan L model on the form in Ltspice?
> >
> >  I can't seem to find a way to instruct LTspice to use
> > it over the standard?
> >
> >   I looked for a model card to use but I don't see it
> > what I was looking for?
> >
> >  All it shows is how to do it in at the text file level, I
> > want to do it on the form? Or do I need to write an include
> > file for that specific L? If so, then I assume when using
> > the mutual inductances (transformer stuff) it'll understand it?
> >
> >
> > Jamie
> 
> watch out for word wraps
> 
> Version 4
> 
 Thanks, those two are exactly what I was looking for..

Jamie

On Thursday, May 29, 2014 12:28:36 AM UTC+2, Maynard A. Philbrook Jr. wrote:
> How do I use John chan L model on the form in Ltspice?
> 
>  I can't seem to find a way to instruct LTspice to use 
> it over the standard?   
> 
>   I looked for a model card to use but I don't see it 
> what I was looking for? 
>  
>  All it shows is how to do it in at the text file level, I 
> want to do it on the form? Or do I need to write an include 
> file for that specific L? If so, then I assume when using 
> the mutual inductances (transformer stuff) it'll understand it?

When I checked one of the schematics where I'd used it, this is the line I found in the "inductance" entry in the inductor information.

HC=20. Bs=.49 Br=.18 A=0.00017 Lm=0.07 Lg=0.0017 N=1360

The LTSpice Help entry on inductors - got to "index" then to L. Inductor - spells out what they all mean.

Those figures are for a heavily gapped Epcos RM-14 core (an EPCOS - B65887E0160A087 - N87 core pair, with a 1.9mm gap) and they mostly came off the EPCOS data sheet. N=1360 is actually the number of turns 'd had put on the on the former.

The character string also showed up on the schematic as as one of the Spice directives.

-- 
Bill Sloman, Sydney

On Wed, 28 May 2014 15:28:36 -0700, Maynard A. Philbrook Jr.  
<jamie_ka1lpa@charter.net> wrote:

>
>
>  How do I use John chan L model on the form in Ltspice?
>
>  I can't seem to find a way to instruct LTspice to use
> it over the standard?
>
>   I looked for a model card to use but I don't see it
> what I was looking for?
>
>  All it shows is how to do it in at the text file level, I
> want to do it on the form? Or do I need to write an include
> file for that specific L? If so, then I assume when using
> the mutual inductances (transformer stuff) it'll understand it?
>
>
> Jamie

VERY useful for plotting the B-HCurve to match to your material curves

watch out for word wrap

Version 4
SHEET 1 1704 680
WIRE 144 112 0 112
WIRE 0 144 0 112
WIRE 144 144 144 112
WIRE 464 144 464 112
WIRE 720 144 720 112
WIRE 0 256 0 224
WIRE 144 256 144 224
WIRE 464 256 464 224
WIRE 720 256 720 224
FLAG 144 256 0
FLAG 0 256 0
FLAG 464 256 0
FLAG 144 112 1
FLAG 464 112 B
IOPIN 464 112 BiDir
FLAG 720 256 0
FLAG 720 112 H
IOPIN 720 112 BiDir
SYMBOL ind 128 128 R0
WINDOW 123 -115 209 Left 2
WINDOW 3 -115 181 Left 2
SYMATTR Value2 Lm={Lm} Lg={Lg} N={N}
SYMATTR Value Hc={Hc} Bs={Bs} Br={Br} A={A}
SYMATTR InstName L1
SYMBOL current 0 224 R180
WINDOW 0 24 80 Left 2
WINDOW 3 43 41 Left 2
WINDOW 123 0 0 Left 2
WINDOW 39 0 0 Left 2
SYMATTR InstName I1
SYMATTR Value SINE(0 1 50 0 0 0 0)
SYMBOL bv 464 128 R0
SYMATTR InstName B1
SYMATTR Value V=idt(V(1))/(A*N)
SYMBOL bv 720 128 R0
SYMATTR InstName B2
SYMATTR Value V=N*I(L1)/Lm
TEXT -224 96 Left 2 !.tran 0 50m 0 10u
TEXT -216 -88 Left 2 !.param A = 2.67e-4
TEXT -216 8 Left 2 !.param N = 10
TEXT -120 -408 Left 2 ;B-H curve of a non-linear inductor\n       by ltoth  
- December 2012\n           elklll@uni-miskolc.hu
TEXT -216 -152 Left 2 !.param Bs = 0.4
TEXT -216 -184 Left 2 !.param Hc = 7.328
TEXT -216 -120 Left 2 !.param Br = 0.106
TEXT -216 -56 Left 2 !.param Lm = 0.255
TEXT -216 -24 Left 2 !.param Lg = 0
TEXT 16 -184 Left 2 ;Coersive force [A/m]
TEXT 16 -152 Left 2 ;Magnetic Saturation [T]
TEXT 16 -120 Left 2 ;Residual Magnetism [T]
TEXT 16 -88 Left 2 ;Cross sectional area [m2]
TEXT 16 -56 Left 2 ;Magnetic Length (excl. gap)  [m]
TEXT 16 -24 Left 2 ;Length of gap  [m]
TEXT 16 8 Left 2 ;Number of turns [1]
TEXT -240 -224 Left 2 ;FERROXCUBE - T102/66/15-3C11 - FERRITE CORE,  
TOROID, 3C11
TEXT 512 -80 Left 2 ;Plot V(b)/1V against V(h)/1V
TEXT 200 200 Left 2 ;540uH
TEXT 448 352 Left 2 ;V(1)/d(I(L1))/1s/1ohm
LINE Normal 272 208 448 336 2
LINE Normal 304 240 272 208 2
LINE Normal 320 224 304 240 2
LINE Normal 272 208 320 224 2
RECTANGLE Normal 400 48 -224 -208
RECTANGLE Normal 912 288 400 48 2
RECTANGLE Normal 264 -328 -136 -424 2
RECTANGLE Normal 280 -312 -152 -440 2

On Wed, 28 May 2014 15:28:36 -0700, Maynard A. Philbrook Jr.  
<jamie_ka1lpa@charter.net> wrote:

>
>
>  How do I use John chan L model on the form in Ltspice?
>
>  I can't seem to find a way to instruct LTspice to use
> it over the standard?
>
>   I looked for a model card to use but I don't see it
> what I was looking for?
>
>  All it shows is how to do it in at the text file level, I
> want to do it on the form? Or do I need to write an include
> file for that specific L? If so, then I assume when using
> the mutual inductances (transformer stuff) it'll understand it?
>
>
> Jamie

watch out for word wraps

Version 4
SHEET 1 1188 900
WIRE 96 208 64 208
WIRE 208 208 176 208
WIRE 224 208 208 208
WIRE 400 208 288 208
WIRE 432 208 400 208
WIRE 448 208 432 208
WIRE 544 208 528 208
WIRE 640 208 544 208
WIRE 784 208 704 208
WIRE 64 224 64 208
WIRE 400 224 400 208
WIRE 448 224 448 208
WIRE 528 224 528 208
WIRE 784 224 784 208
WIRE 64 320 64 304
WIRE 400 320 400 304
WIRE 448 320 448 304
WIRE 528 320 528 304
WIRE 784 320 784 304
FLAG 64 320 0
FLAG 784 320 0
FLAG 528 320 0
FLAG 400 320 0
FLAG 448 320 0
FLAG 208 208 i
FLAG 784 208 o
FLAG 432 208 p
FLAG 544 208 s
SYMBOL ind2 384 208 R0
WINDOW 0 0 24 Right 0
WINDOW 3 0 56 Right 0
WINDOW 39 0 88 Right 0
SYMATTR InstName Lp
SYMATTR Value {Lp}
SYMATTR Type ind
SYMATTR SpiceLine Rser=1u
SYMBOL ind2 544 208 M0
WINDOW 0 0 24 Right 0
WINDOW 3 0 56 Right 0
WINDOW 39 0 88 Right 0
SYMATTR InstName Ls
SYMATTR Value {Ls}
SYMATTR Type ind
SYMATTR SpiceLine Rser=1u
SYMBOL voltage 64 208 R0
WINDOW 0 -32 32 Right 0
WINDOW 3 -32 80 Right 0
WINDOW 123 0 0 Left 0
WINDOW 39 -32 112 Right 0
SYMATTR InstName V1
SYMATTR Value SINE(0 {Vp} {f} 0 0 90)
SYMATTR SpiceLine Rser=1m
SYMBOL res 768 208 R0
SYMATTR InstName Ro
SYMATTR Value 260
SYMBOL ind 432 208 R0
WINDOW 0 56 0 Center 0
WINDOW 3 -144 144 Left 0
WINDOW 123 -144 176 Left 0
SYMATTR InstName Lm
SYMATTR Value Hc=0.12 Bs=2.03 Br=.050 A=3m72 Lm=0.671
SYMATTR Value2 Lg=0 N={Np}
SYMBOL voltage 192 208 M270
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V2
SYMATTR Value PWL(0 0 1 1k)
SYMBOL FerriteBead2 256 208 M90
WINDOW 0 -9 0 VBottom 0
WINDOW 3 9 0 VTop 0
WINDOW 39 35 0 VTop 0
SYMATTR InstName LLp
SYMATTR Prefix L
SYMATTR Value {LLp}
SYMATTR SpiceLine Rser={RLp}
SYMBOL FerriteBead2 672 208 R90
WINDOW 0 -9 0 VBottom 0
WINDOW 3 9 0 VTop 0
WINDOW 39 35 0 VTop 0
SYMATTR InstName LLp1
SYMATTR Prefix L
SYMATTR Value {LLp}
SYMATTR SpiceLine Rser={RLp}
TEXT -144 384 Left 0 !.param Vi=380 f=400\n+ Vp=sqrt(2)*Vi
TEXT -144 -112 Left 0 ;Steel = M6 - 29Ga\nA = 2.4" x 2.4" = 5.76in^2  
(0.00372m^2)\nMagnetic Path Length = 26.4" (0.671m)\nBsat = 20300 Gauss  
(2.03T)\nInput Voltage = 380VAC\nInput Frequency = 400Hz\nOutput Voltage =  
6.5KV\nOutput Power = 50KVA\nOther parameters as per .op command
TEXT -144 448 Left 0 !.tran 0 .1 10u 10u uic
TEXT 288 424 Left 0 !.param Np=96 Nsp=6k5/380\n+ Zsp=Nsp**2 Lp=1k  
Ls=Lp*Zsp\n+ LLp=10u LLs=LLp*Zsp\n+ RLp=1m RLs=RLp*Zsp
TEXT 488 160 Center 0 !Kx Lp Ls 1
LINE Normal 480 304 480 224
LINE Normal 496 304 496 224