L
LM
There are many kinds of them for instance from NXP.
-
Categories
-
Platforms
-
Content
T
Tom Del Rosso
Jim said:
The program must be worth the money. Most software is never effortless no
matter how much you master it.
L
LM
I have the "original crispy" MicroSim flavor of schematic capture
So easy to use that OrCAD, then Cadence, chose to crush it.
...Jim Thompson
--
| James E.Thompson, CTO | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon athttp://www.analog-innovations.com| 1962 |
I love to cook with wine. Sometimes I even put it in the food.
True. It cant be totally impossible because there are models at NXP. I
quess I have to start with Yahoo.
About old simulators. I had in an old 286 machine some similation
program, Microsim perhaps. It ran about as fast as this windows
version. LT spice should be about a thousand times faster that it.
What can do I do with a BF998.prm? (other than perhaps delete)
M
Martin Riddle
Jim Thompson said:
It does seem vague, just a few lines of Help on the subject. But it's
straight forward with a little practice.
Cheers
H
Helmut Sennewald
Jim Thompson said:
Hello Jim,
Open the symbol editor.
Place 4 pins.
Right-click on each pin to edit the netlist order to the order in the
..subckt-line.
Draw some nice graphic around it.
Write BFXXX into attribute "Value". Edit -> attributes
Save.
Place this symbol in the schematic.
Change BFXXX to BF998
Include the model file with a SPICE-directive
..lib name_of_file
Wire the complete circuit.
RUN the simulation.
I have used BFXXX in the symbol, because I had in mind to use it for BF996,
BF999, BF???.
If I had used BF998 in the symbol editor, I wouldn't have to change it
later in the schematic of course.
It's also possible to make a symbol only for the BF998.
Last but not least you can already specify the model file in the symbol too.
Best regards,
Helmut
R
Robert Macy
I have the "original crispy" MicroSim flavor of schematic capture
So easy to use that OrCAD, then Cadence, chose to crush it.
...Jim Thompson
--
| James E.Thompson, CTO | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice
| E-mail Icon athttp://www.analog-innovations.com| 1962 |
I love to cook with wine. Sometimes I even put it in the food.
MicroSim was so good I even sprang for the $100+ manual to go with the
'student' version.
As you may know, paying for ANY software rankles me to no end. But
PSpice was so good, I both rewarded MicroSim by buying the book and
enabled me to create models.
R
Robert Macy
I've been doing PSpice so far back that I ran it under DOS, drew
schematics on paper, numbered the nodes, the entered the netlist with
some klutzy text editor. My oldest son wrote me a version controller,
so that every new netlist and DAT file could be tracked.
...Jim Thompson
--
| James E.Thompson, CTO | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice
| E-mail Icon athttp://www.analog-innovations.com| 1962 |
I love to cook with wine. Sometimes I even put it in the food.
I still have AND USE my DOS version. Why? because it has the ability
to plot BH Curves directly
BHCURVE - GENERATES A BH CURVE FOR A CORE
* model uses MKS and CGS units of cm and cm^2 for input
* plot converts to Gauss and Oersteds for output
* to plot, set Y = B(K1) and X = H(K1)
..TRAN 1 6 0 1000uS
..OPTIONS ITL5=0
I1 0 1 SIN(0 .1 1 1)
I2 0 1 SIN(0 .2 1 2)
I3 0 1 SIN(0 .8 1 3)
R1 1 0 1
L1 1 0 200
K1 L1 .9999 KBREAK
..model KBREAK CORE(AREA=3.27156 PATH=12.90399 GAP=0
+K=100 MS=97772.47 A=500 C=0.2)
..PROBE
..END
wish LTspice did something like that.
drew it on paper?! memory slipping? just left to right like playing
chess in your mind.
J
Jamie
You can't do the hysteric core model based on a model first proposed inRobert said:
by John Chan ? It's supported in Ltspice. The problem is that mechanical
data has to be supplied.
I've been playing with that the last couple of days working with a
regenerative oscillator, only because I can't figure out how to set the
turn ratio on the coupled inductors which kinds of screws up my tank
circuit for a real world example.
Jamie
L
LM
There are many kinds of them for instance from NXP.
NXP has some low noise dg fets. They are probably easier to use at UHF/
VHF than a hot 10+GHz XXXfet.
Most are gone.
NXP has some low noise dg fets. They are probably easier to use at UHF/
VHF than a hot 10+GHz XXXfet.
R
Robert Macy
Apologies to OP, seemed to have hijacked your thread, but please bear
with us here...
You missed the syntax of K1 and the ease of plotting BH Curve.
Although I laud LTspice for using MKS units it can get confusing,
going back and forth...
Hc = 1.251 Oe = 99.55 A/m
Bs = 1.202e3 G = .1202 T
Br = 85.14 G = .008514 T
Area = 3.27156 = 327.156e-6 sq m
Path = 12.90399 = .129039 m
Gap = 0 = 0 ??
B from Gauss to Tesla divide by 1e4
H from Oersted to Amp/m multiply by 79.57747
then in LTspice you must plot the following 'formulas' to get the BH
Curve:
H=NI/pathlength = 1550*I/1A
Bup = (.1202*(1550*I(L1)+99.55)/(abs(1550*I(L1)+99.55)+99.55*13.12) +
1.94779e-3*I(L1))/1A
Bdn = (.1202*(1550*I(L1)-99.55)/(abs(1550*I(L1)-99.55)+99.55*13.12) +
1.94779e-3*I(L1))/1A,
,or both, but doesn't work so well
Bmag = (.1202*(1550*I(L1)+99.55)/(abs(1550*I(L1)+99.55)+99.55*13.12) +
1.94779e-3*I(L1) + .1202*(1550*I(L1)-99.55)/
(abs(1550*I(L1)-99.55)+99.55*13.12) + 1.94779e-3*I(L1))/2A
Can't remember if those are ceneric constants, or constants just for
THIS model. I either get the 'going up' side or the 'going down side'
but nothing like I used to get with PSpice DOS version.
By the way, you'll find that LTspice's curve fit for the Chan model is
excellent! PSpice's Jiles-Atherton model used to make hour glass
shaped hysteresis curves that were incredibly difficult to make
square. But, LTspice does fairly well, by just supplying two terms
Bsat and the Br [where it hits the axis] and you get a decent looking
curve.
R
Robert Macy
I think LTspice can do the same thing. Just think your way thru
parameterization.
...Jim Thompson
--
| James E.Thompson, CTO | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice
| E-mail Icon athttp://www.analog-innovations.com| 1962 |
I love to cook with wine. Sometimes I even put it in the food.
Jim, THAT's uncharacteristically vague.See the reply to Jamie for the
way to make LTspice do similar plot to what PSpice DOS version used to
do. I say 'similar' because I have not been able to get the ends of
the curve to touch each other, get close, but no cigars..
R
Robert Macy
FOUND IT! this runs on LTspice
BHCURVE - GENERATES A BH CURVE FOR K528T500_3C8 CORE
* Plot results as V(12)/1V or V(22)/1V or V(32)/1V vs V(20)/1V
..TRAN 1 6 0 10uS
..OPTIONS ITL5=0
* constant absolute permeability = 4pi*1e-7
..param uo=1.256637e-6
* 3C8 material parameters in MKS units
* Note derived from inspection of Microsim PSpice results
..param Hc1=167.1127
..param Bs1=.49
..param Br1=.4575
* Specific core parameters in MKS units
..param Lm1=.1290396
..param A1=327.1756e-6
..param Lg1=0
..param N1=20
*
I1 0 1 SIN(0 .1 1 1)
I2 0 1 SIN(0 .2 1 2)
I3 0 1 SIN(0 .8 1 3)
I4 0 1 SIN(0 1.6 1 4)
R1 1 0 1
L1 1 0 Hc={Hc1} Bs={Bs1} Br={Br1} A=327.1756e-6 Lm={Lm1}
Lg={Lg1} N={N1}
*
* From LTspice manual on page 130 and 131 Use B sources to plot
results:
Bup 12 0 V={(Bs1*(N1*I(L1)/Lm1+Hc1)/(abs(N1*I(L1)/Lm1+Hc1)+Hc1*(Bs1/
Br1-1)) + uo*N1*I(L1)/Lm1)/1A}
Bdn 22 0 V={(Bs1*(N1*I(L1)/Lm1-Hc1)/(abs(N1*I(L1)/Lm1-Hc1)+Hc1*(Bs1/
Br1-1)) + uo*N1*I(L1)/Lm1)/1A}
Bmag 32 0 V={(V(12)+V(22))/2}
* assuming flux is contained in the core, H = N1*I(L1)/Lm1
B_H 20 0 V={N1*I(L1)/Lm1/1A}
..PROBE
..END
then, plot V(12) and V(22) vs V(20) and you get the hysteresis curve,
but the ends don't connect.
enjoy
R
Robert Macy
found it! see the reply to myself to Jamie.
M
Martin Riddle
John Larkin said:
You can define the subckt for the Symbol after you place it. Just right
Click on the symbol and Change the 'SpiceModel' Line to your subckt
name.
Not the same as editing the Attributes for the model file in the Symbol
editor.
Cheers
