Simulating a variable resistance input with LTSpice?
in [Design]
|
Prev: unexpected delay in a TWT
Next: memristors
From: Joerg on 14 Apr 2010 16:13 Helmut Sennewald wrote: > "Joerg" <invalid(a)invalid.invalid> schrieb im Newsbeitrag > news:82mkahF8k0U1(a)mid.individual.net... >> qrk wrote: >>> On Wed, 14 Apr 2010 10:23:14 -0700, Jim Thompson >>> <To-Email-Use-The-Envelope-Icon(a)On-My-Web-Site.com> wrote: >>> >>>> On Wed, 14 Apr 2010 10:14:33 -0700, qrk <SpamTrap(a)spam.net> wrote: >>>> >>>>> On Tue, 13 Apr 2010 10:58:03 -0700, Joerg <invalid(a)invalid.invalid> >>>>> wrote: >>>>> >>>>>> Hello Folks, >>>>>> >>>>>> Got stuck when trying to simulate an NTC. This temperature-variant >>>>>> resistor will be the only variable input so ".STEP" and stuff do not >>>>>> cut it because that only overlays multiple curve in an AC or DC >>>>>> simulation. I want just one curve: Output of my circuit versus varying >>>>>> NTC resistor value. >>>>>> >>>>>> Tried to make a voltage dependent resistor this way: >>>>>> >>>>>> http://www.electro-tech-online.com/attachments/general-electronics-chat/40714d1269571000-sine-variable-resistor-ltspice-d2.png >>>>>> >>>>>> It works but is incredibly slow. Any better ideas? >>>>> Here's a couple NTC subcircuits I made up for PSpice. LTspice is >>>>> compatible with PSpice syntax, so these should work. These respond to >>>>> the temperature parameter in Spice. Easiest to use the Beta equation >>>>> approximation, but Steinhart-Hart equation is a bit more accurate. >>>>> >>>>> ************************************************** >>>>> * NTC resistor using the Beta equation: * >>>>> * R = Ro * EXP(B*(1/T - 1/298.15)) * >>>>> * Requires resistor value at 25 deg C and Beta * >>>>> * which can be set in this subcircuit or passed * >>>>> * thru the X instantiation. e.g. * >>>>> * X1 1 0 THERMISTORntcB PARAMS: Ro=100k B=4300 * >>>>> * Schematics component: RntcB * >>>>> * By: Mark 26 March 2003 * >>>>> ************************************************** >>>>> * +------------------- NTC resistor terminals >>>>> * | >>>>> * | +-------- Resistance at 25 deg C >>>>> * | | +- Beta value >>>>> .SUBCKT THERMISTORntcB 1 2 PARAMS: Ro=10k B=4300 >>>>> ETHERM 1 3 VALUE={ I(VSENSE)*Ro*EXP(B*(1/(TEMP+273.15)-1/298.15)) } >>>>> VSENSE 3 2 DC 0 >>>>> .ENDS THERMISTORntcB >>>>> >>>>> ********************************************************* >>>>> * NTC resistor using the Steinhart-Hart equation: * >>>>> * 1/T = A + B*ln(R) + C*ln(R)**3 (ugly solution for R) * >>>>> * Requires equation coefficients which can be * >>>>> * set in this subcircuit or passed thru the * >>>>> * X instantiation. e.g. * >>>>> * X1 1 0 THERMISTORntcS PARAMS: A=8.215E-4 B=2.111E-4 C=6.716E-8 * >>>>> * See Thermistor_Calculator.mcd for coefficient gen * >>>>> * Schematics component: RntcS * >>>>> * By: Mark 26 March 2003 * >>>>> ********************************************************* >>>>> * +-------------------NTC resistor terminals >>>>> * | +------+------+- equation coeffs >>>>> coefficients >>>>> .SUBCKT THERMISTORntcS 1 2 PARAMS: A=8E-4 B=2E-4 C=7E-8 >>>>> .PARAM D={ ((1/(TEMP+273.15))-A)/(2*C) } >>>>> .PARAM E={ (B/(3*C))**3 } >>>>> .PARAM F={ SQRT(D**2+E) } >>>>> .PARAM G={ EXP(PWRS(D-F,1/3)+PWRS(D+F,1/3)) } >>>>> ETHERM 1 3 VALUE={ I(VSENSE)*G } >>>>> VSENSE 3 2 DC 0 >>>>> .ENDS THERMISTORntcS >>>>> >>>>> >>>>> >>>>> Regards, >>>>> Mark >>>> Hi Mark, That's the same _standard_ equation I posted, but Joerg >>>> seems to think he has to use Steinhart-Hart... he's fond of generating >>>> 3-place simulation "accuracy" from a 2-place data sheet ;-) >>>> >>>> ...Jim Thompson >>> If he wants to use Steinhart-Hart equation, I probably have a solver >>> for the coefficients using Mathcad somewhere. I think I pulled that >>> off an app note. The beta and S-H equations are pretty close to >>> another if I recall correctly. That's why I have two different PSpice >>> components - to please the inner "place". >>> >> If I need it again I'll probably pour it into one large WAV file and feed >> that into SPICE. I know that sounds like cheating but then the PC doesn't >> have to crunch so much on every run. One value for every 0.5C or so should >> suffice. >> >> >>> Coefficients calculation given in this note: >>> http://www.cornerstonesensors.com/reports/AboutEquation.pdf >>> >>> Excel solver: >>> http://www.ilxlightwave.com/appnotes/AN%204%20REV02%20Thermistor%20Calibration%20and%20Steinhart%20Hart.pdf >>> >> Thanks, for all the info, Mark. I'll take a look, but this small circuit >> had to be done quickly and is now finished. >> >> -- >> Regards, Joerg >> >> http://www.analogconsultants.com/ >> >> "gmail" domain blocked because of excessive spam. >> Use another domain or send PM. > > > Hello Joerg, > > I have sent you an email with an example using the models from Mark.. > It's for LTspice of course. > Thanks, Helmut, got it and will try it out this weekend. It was a little off when I sent the stuff to the client. The method with the formula in the resistor (controlled via voltage source) that I used yesterday did the trick but it does leave one weirdness: The x-axis of the plot is now labeled in kilovolts instead of kiloohms :-) -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
From: Helmut Sennewald on 14 Apr 2010 16:18 "Joerg" <invalid(a)invalid.invalid> schrieb im Newsbeitrag news:82mlvpFi0bU1(a)mid.individual.net... > Helmut Sennewald wrote: >> "Joerg" <invalid(a)invalid.invalid> schrieb im Newsbeitrag >> news:82mkahF8k0U1(a)mid.individual.net... >>> qrk wrote: >>>> On Wed, 14 Apr 2010 10:23:14 -0700, Jim Thompson >>>> <To-Email-Use-The-Envelope-Icon(a)On-My-Web-Site.com> wrote: >>>> >>>>> On Wed, 14 Apr 2010 10:14:33 -0700, qrk <SpamTrap(a)spam.net> wrote: >>>>> >>>>>> On Tue, 13 Apr 2010 10:58:03 -0700, Joerg <invalid(a)invalid.invalid> >>>>>> wrote: >>>>>> >>>>>>> Hello Folks, >>>>>>> >>>>>>> Got stuck when trying to simulate an NTC. This temperature-variant >>>>>>> resistor will be the only variable input so ".STEP" and stuff do not >>>>>>> cut it because that only overlays multiple curve in an AC or DC >>>>>>> simulation. I want just one curve: Output of my circuit versus >>>>>>> varying NTC resistor value. >>>>>>> >>>>>>> Tried to make a voltage dependent resistor this way: >>>>>>> >>>>>>> http://www.electro-tech-online.com/attachments/general-electronics-chat/40714d1269571000-sine-variable-resistor-ltspice-d2.png >>>>>>> >>>>>>> It works but is incredibly slow. Any better ideas? >>>>>> Here's a couple NTC subcircuits I made up for PSpice. LTspice is >>>>>> compatible with PSpice syntax, so these should work. These respond to >>>>>> the temperature parameter in Spice. Easiest to use the Beta equation >>>>>> approximation, but Steinhart-Hart equation is a bit more accurate. >>>>>> >>>>>> ************************************************** >>>>>> * NTC resistor using the Beta equation: * >>>>>> * R = Ro * EXP(B*(1/T - 1/298.15)) * >>>>>> * Requires resistor value at 25 deg C and Beta * >>>>>> * which can be set in this subcircuit or passed * >>>>>> * thru the X instantiation. e.g. * >>>>>> * X1 1 0 THERMISTORntcB PARAMS: Ro=100k B=4300 * >>>>>> * Schematics component: RntcB * >>>>>> * By: Mark 26 March 2003 * >>>>>> ************************************************** >>>>>> * +------------------- NTC resistor terminals >>>>>> * | >>>>>> * | +-------- Resistance at 25 deg C >>>>>> * | | +- Beta value >>>>>> .SUBCKT THERMISTORntcB 1 2 PARAMS: Ro=10k B=4300 >>>>>> ETHERM 1 3 VALUE={ I(VSENSE)*Ro*EXP(B*(1/(TEMP+273.15)-1/298.15)) } >>>>>> VSENSE 3 2 DC 0 >>>>>> .ENDS THERMISTORntcB >>>>>> >>>>>> ********************************************************* >>>>>> * NTC resistor using the Steinhart-Hart equation: * >>>>>> * 1/T = A + B*ln(R) + C*ln(R)**3 (ugly solution for R) * >>>>>> * Requires equation coefficients which can be * >>>>>> * set in this subcircuit or passed thru the * >>>>>> * X instantiation. e.g. * >>>>>> * X1 1 0 THERMISTORntcS PARAMS: A=8.215E-4 B=2.111E-4 C=6.716E-8 * >>>>>> * See Thermistor_Calculator.mcd for coefficient gen * >>>>>> * Schematics component: RntcS * >>>>>> * By: Mark 26 March 2003 * >>>>>> ********************************************************* >>>>>> * +-------------------NTC resistor terminals >>>>>> * | +------+------+- equation coeffs >>>>>> coefficients >>>>>> .SUBCKT THERMISTORntcS 1 2 PARAMS: A=8E-4 B=2E-4 C=7E-8 >>>>>> .PARAM D={ ((1/(TEMP+273.15))-A)/(2*C) } >>>>>> .PARAM E={ (B/(3*C))**3 } >>>>>> .PARAM F={ SQRT(D**2+E) } >>>>>> .PARAM G={ EXP(PWRS(D-F,1/3)+PWRS(D+F,1/3)) } >>>>>> ETHERM 1 3 VALUE={ I(VSENSE)*G } >>>>>> VSENSE 3 2 DC 0 >>>>>> .ENDS THERMISTORntcS >>>>>> >>>>>> >>>>>> >>>>>> Regards, >>>>>> Mark >>>>> Hi Mark, That's the same _standard_ equation I posted, but Joerg >>>>> seems to think he has to use Steinhart-Hart... he's fond of generating >>>>> 3-place simulation "accuracy" from a 2-place data sheet ;-) >>>>> >>>>> ...Jim Thompson >>>> If he wants to use Steinhart-Hart equation, I probably have a solver >>>> for the coefficients using Mathcad somewhere. I think I pulled that >>>> off an app note. The beta and S-H equations are pretty close to >>>> another if I recall correctly. That's why I have two different PSpice >>>> components - to please the inner "place". >>>> >>> If I need it again I'll probably pour it into one large WAV file and >>> feed that into SPICE. I know that sounds like cheating but then the PC >>> doesn't have to crunch so much on every run. One value for every 0.5C or >>> so should suffice. >>> >>> >>>> Coefficients calculation given in this note: >>>> http://www.cornerstonesensors.com/reports/AboutEquation.pdf >>>> >>>> Excel solver: >>>> http://www.ilxlightwave.com/appnotes/AN%204%20REV02%20Thermistor%20Calibration%20and%20Steinhart%20Hart.pdf >>>> >>> Thanks, for all the info, Mark. I'll take a look, but this small circuit >>> had to be done quickly and is now finished. >>> >>> -- >>> Regards, Joerg >>> >>> http://www.analogconsultants.com/ >>> >>> "gmail" domain blocked because of excessive spam. >>> Use another domain or send PM. >> >> >> Hello Joerg, >> >> I have sent you an email with an example using the models from Mark.. >> It's for LTspice of course. >> > > Thanks, Helmut, got it and will try it out this weekend. It was a little > off when I sent the stuff to the client. The method with the formula in > the resistor (controlled via voltage source) that I used yesterday did the > trick but it does leave one weirdness: The x-axis of the plot is now > labeled in kilovolts instead of kiloohms :-) > > -- > Regards, Joerg Hello Joerg, I assumed you want simulate resistance versus temperature. Do you need it the other way? Temperature(resistance)? Best regards, Helmut > > http://www.analogconsultants.com/ > > "gmail" domain blocked because of excessive spam. > Use another domain or send PM.
From: Joerg on 14 Apr 2010 16:25 Helmut Sennewald wrote: > "Joerg" <invalid(a)invalid.invalid> schrieb im Newsbeitrag > news:82mlvpFi0bU1(a)mid.individual.net... >> Helmut Sennewald wrote: >>> "Joerg" <invalid(a)invalid.invalid> schrieb im Newsbeitrag >>> news:82mkahF8k0U1(a)mid.individual.net... >>>> qrk wrote: >>>>> On Wed, 14 Apr 2010 10:23:14 -0700, Jim Thompson >>>>> <To-Email-Use-The-Envelope-Icon(a)On-My-Web-Site.com> wrote: >>>>> >>>>>> On Wed, 14 Apr 2010 10:14:33 -0700, qrk <SpamTrap(a)spam.net> wrote: >>>>>> >>>>>>> On Tue, 13 Apr 2010 10:58:03 -0700, Joerg <invalid(a)invalid.invalid> >>>>>>> wrote: >>>>>>> >>>>>>>> Hello Folks, >>>>>>>> >>>>>>>> Got stuck when trying to simulate an NTC. This temperature-variant >>>>>>>> resistor will be the only variable input so ".STEP" and stuff do not >>>>>>>> cut it because that only overlays multiple curve in an AC or DC >>>>>>>> simulation. I want just one curve: Output of my circuit versus >>>>>>>> varying NTC resistor value. >>>>>>>> >>>>>>>> Tried to make a voltage dependent resistor this way: >>>>>>>> >>>>>>>> http://www.electro-tech-online.com/attachments/general-electronics-chat/40714d1269571000-sine-variable-resistor-ltspice-d2.png >>>>>>>> >>>>>>>> It works but is incredibly slow. Any better ideas? >>>>>>> Here's a couple NTC subcircuits I made up for PSpice. LTspice is >>>>>>> compatible with PSpice syntax, so these should work. These respond to >>>>>>> the temperature parameter in Spice. Easiest to use the Beta equation >>>>>>> approximation, but Steinhart-Hart equation is a bit more accurate. >>>>>>> >>>>>>> ************************************************** >>>>>>> * NTC resistor using the Beta equation: * >>>>>>> * R = Ro * EXP(B*(1/T - 1/298.15)) * >>>>>>> * Requires resistor value at 25 deg C and Beta * >>>>>>> * which can be set in this subcircuit or passed * >>>>>>> * thru the X instantiation. e.g. * >>>>>>> * X1 1 0 THERMISTORntcB PARAMS: Ro=100k B=4300 * >>>>>>> * Schematics component: RntcB * >>>>>>> * By: Mark 26 March 2003 * >>>>>>> ************************************************** >>>>>>> * +------------------- NTC resistor terminals >>>>>>> * | >>>>>>> * | +-------- Resistance at 25 deg C >>>>>>> * | | +- Beta value >>>>>>> .SUBCKT THERMISTORntcB 1 2 PARAMS: Ro=10k B=4300 >>>>>>> ETHERM 1 3 VALUE={ I(VSENSE)*Ro*EXP(B*(1/(TEMP+273.15)-1/298.15)) } >>>>>>> VSENSE 3 2 DC 0 >>>>>>> .ENDS THERMISTORntcB >>>>>>> >>>>>>> ********************************************************* >>>>>>> * NTC resistor using the Steinhart-Hart equation: * >>>>>>> * 1/T = A + B*ln(R) + C*ln(R)**3 (ugly solution for R) * >>>>>>> * Requires equation coefficients which can be * >>>>>>> * set in this subcircuit or passed thru the * >>>>>>> * X instantiation. e.g. * >>>>>>> * X1 1 0 THERMISTORntcS PARAMS: A=8.215E-4 B=2.111E-4 C=6.716E-8 * >>>>>>> * See Thermistor_Calculator.mcd for coefficient gen * >>>>>>> * Schematics component: RntcS * >>>>>>> * By: Mark 26 March 2003 * >>>>>>> ********************************************************* >>>>>>> * +-------------------NTC resistor terminals >>>>>>> * | +------+------+- equation coeffs >>>>>>> coefficients >>>>>>> .SUBCKT THERMISTORntcS 1 2 PARAMS: A=8E-4 B=2E-4 C=7E-8 >>>>>>> .PARAM D={ ((1/(TEMP+273.15))-A)/(2*C) } >>>>>>> .PARAM E={ (B/(3*C))**3 } >>>>>>> .PARAM F={ SQRT(D**2+E) } >>>>>>> .PARAM G={ EXP(PWRS(D-F,1/3)+PWRS(D+F,1/3)) } >>>>>>> ETHERM 1 3 VALUE={ I(VSENSE)*G } >>>>>>> VSENSE 3 2 DC 0 >>>>>>> .ENDS THERMISTORntcS >>>>>>> >>>>>>> >>>>>>> >>>>>>> Regards, >>>>>>> Mark >>>>>> Hi Mark, That's the same _standard_ equation I posted, but Joerg >>>>>> seems to think he has to use Steinhart-Hart... he's fond of generating >>>>>> 3-place simulation "accuracy" from a 2-place data sheet ;-) >>>>>> >>>>>> ...Jim Thompson >>>>> If he wants to use Steinhart-Hart equation, I probably have a solver >>>>> for the coefficients using Mathcad somewhere. I think I pulled that >>>>> off an app note. The beta and S-H equations are pretty close to >>>>> another if I recall correctly. That's why I have two different PSpice >>>>> components - to please the inner "place". >>>>> >>>> If I need it again I'll probably pour it into one large WAV file and >>>> feed that into SPICE. I know that sounds like cheating but then the PC >>>> doesn't have to crunch so much on every run. One value for every 0.5C or >>>> so should suffice. >>>> >>>> >>>>> Coefficients calculation given in this note: >>>>> http://www.cornerstonesensors.com/reports/AboutEquation.pdf >>>>> >>>>> Excel solver: >>>>> http://www.ilxlightwave.com/appnotes/AN%204%20REV02%20Thermistor%20Calibration%20and%20Steinhart%20Hart.pdf >>>>> >>>> Thanks, for all the info, Mark. I'll take a look, but this small circuit >>>> had to be done quickly and is now finished. >>>> >>>> -- >>>> Regards, Joerg >>>> >>>> http://www.analogconsultants.com/ >>>> >>>> "gmail" domain blocked because of excessive spam. >>>> Use another domain or send PM. >>> >>> Hello Joerg, >>> >>> I have sent you an email with an example using the models from Mark.. >>> It's for LTspice of course. >>> >> Thanks, Helmut, got it and will try it out this weekend. It was a little >> off when I sent the stuff to the client. The method with the formula in >> the resistor (controlled via voltage source) that I used yesterday did the >> trick but it does leave one weirdness: The x-axis of the plot is now >> labeled in kilovolts instead of kiloohms :-) >> >> -- >> Regards, Joerg > > Hello Joerg, > > I assumed you want simulate resistance versus temperature. > Do you need it the other way? Temperature(resistance)? > I had to simulate the output of my circuit versus stepped temperature, IOW the temperature would have been the stimulus. Since I hadn't poured in the whole equation I instead stepped the resistance and plotted the electrical output. In real life it will be the opposite. The software will have to calculate temperature from the voltage it sees. That requires the inverse Steinhart-Hart which gets sort of ugly. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
From: Jim Thompson on 14 Apr 2010 18:18 On Wed, 14 Apr 2010 11:47:57 -0700, qrk <SpamTrap(a)spam.net> wrote: >On Wed, 14 Apr 2010 10:23:14 -0700, Jim Thompson ><To-Email-Use-The-Envelope-Icon(a)On-My-Web-Site.com> wrote: > >>On Wed, 14 Apr 2010 10:14:33 -0700, qrk <SpamTrap(a)spam.net> wrote: >> >>>On Tue, 13 Apr 2010 10:58:03 -0700, Joerg <invalid(a)invalid.invalid> >>>wrote: >>> >>>>Hello Folks, >>>> >>>>Got stuck when trying to simulate an NTC. This temperature-variant >>>>resistor will be the only variable input so ".STEP" and stuff do not cut >>>>it because that only overlays multiple curve in an AC or DC simulation. >>>>I want just one curve: Output of my circuit versus varying NTC resistor >>>>value. >>>> >>>>Tried to make a voltage dependent resistor this way: >>>> >>>>http://www.electro-tech-online.com/attachments/general-electronics-chat/40714d1269571000-sine-variable-resistor-ltspice-d2.png >>>> >>>>It works but is incredibly slow. Any better ideas? >>> >>>Here's a couple NTC subcircuits I made up for PSpice. LTspice is >>>compatible with PSpice syntax, so these should work. These respond to >>>the temperature parameter in Spice. Easiest to use the Beta equation >>>approximation, but Steinhart-Hart equation is a bit more accurate. >>> >>>************************************************** >>>* NTC resistor using the Beta equation: * >>>* R = Ro * EXP(B*(1/T - 1/298.15)) * >>>* Requires resistor value at 25 deg C and Beta * >>>* which can be set in this subcircuit or passed * >>>* thru the X instantiation. e.g. * >>>* X1 1 0 THERMISTORntcB PARAMS: Ro=100k B=4300 * >>>* Schematics component: RntcB * >>>* By: Mark 26 March 2003 * >>>************************************************** >>>* +------------------- NTC resistor terminals >>>* | >>>* | +-------- Resistance at 25 deg C >>>* | | +- Beta value >>>.SUBCKT THERMISTORntcB 1 2 PARAMS: Ro=10k B=4300 >>> ETHERM 1 3 VALUE={ I(VSENSE)*Ro*EXP(B*(1/(TEMP+273.15)-1/298.15)) } >>> VSENSE 3 2 DC 0 >>>.ENDS THERMISTORntcB >>> >>>********************************************************* >>>* NTC resistor using the Steinhart-Hart equation: * >>>* 1/T = A + B*ln(R) + C*ln(R)**3 (ugly solution for R) * >>>* Requires equation coefficients which can be * >>>* set in this subcircuit or passed thru the * >>>* X instantiation. e.g. * >>>* X1 1 0 THERMISTORntcS PARAMS: A=8.215E-4 B=2.111E-4 C=6.716E-8 * >>>* See Thermistor_Calculator.mcd for coefficient gen * >>>* Schematics component: RntcS * >>>* By: Mark 26 March 2003 * >>>********************************************************* >>>* +-------------------NTC resistor terminals >>>* | +------+------+- equation coeffs >>>coefficients >>>.SUBCKT THERMISTORntcS 1 2 PARAMS: A=8E-4 B=2E-4 C=7E-8 >>> .PARAM D={ ((1/(TEMP+273.15))-A)/(2*C) } >>> .PARAM E={ (B/(3*C))**3 } >>> .PARAM F={ SQRT(D**2+E) } >>> .PARAM G={ EXP(PWRS(D-F,1/3)+PWRS(D+F,1/3)) } >>> ETHERM 1 3 VALUE={ I(VSENSE)*G } >>> VSENSE 3 2 DC 0 >>>.ENDS THERMISTORntcS >>> >>> >>> >>>Regards, >>>Mark >> >>Hi Mark, That's the same _standard_ equation I posted, but Joerg >>seems to think he has to use Steinhart-Hart... he's fond of generating >>3-place simulation "accuracy" from a 2-place data sheet ;-) >> >> ...Jim Thompson > >If he wants to use Steinhart-Hart equation, I probably have a solver >for the coefficients using Mathcad somewhere. I think I pulled that >off an app note. The beta and S-H equations are pretty close to >another if I recall correctly. That's why I have two different PSpice >components - to please the inner "place". > >Coefficients calculation given in this note: >http://www.cornerstonesensors.com/reports/AboutEquation.pdf > >Excel solver: >http://www.ilxlightwave.com/appnotes/AN%204%20REV02%20Thermistor%20Calibration%20and%20Steinhart%20Hart.pdf Mark, It occurs to me, since I think, as an electrical engineer, in Ohms, rather than L/W, I twisted XFAB's resistor equations thusly... * ---------------------------------------------------------------------- * TYPICAL MEAN CONDITION * ---------------------------------------------------------------------- * NOTE: TNOM = 27 deg C * NOTE: Recommended minimum numbers of squares L/W > 5 * NOTE: Contact resistance with maximum number of contacts is appr. * resrc={rcont/ncont/m} * ncont1=(1+((w-2*0.5e-06)/1.2e-06-0.499)) calculated, * but can exactly specified with parameter ncont * ncont=int(1+((w-2*0.5e-06)/1.2e-06-0.499)) * VARIABLES: w,l=device width and length ; m, par1 = multiplier * ..SUBCKT RPOLYH N1 N2 PARAMS: R=15K W=3u ;L=10u ..PARAM M=1 NCONT=1000 ;PAR1=1 ..PARAM RSH=3.5K ..PARAM RSH0=3.5K ..PARAM NCONT1={1+((W-2*0.5E-06)/1.2u-0.499)} ..PARAM NCONT2={MIN(NCONT1,NCONT)} ..PARAM NCONT3={MAX(1,NCONT2)} ..PARAM RESRC={115/NCONT3/M} ..PARAM RESRC0={115/NCONT3/M} ..PARAM L={(R-2*RESRC0)*(W-0.12u)/RSH0} RC1 N1 NA {RESRC} TC=-0.95m,0.3u R1 NA NB {(3.5K*(L-(0.0))/(W-(0.12u)))/M} TC=-3.30m,10.9u RC2 NB N2 {RESRC} TC=-0.95m,0.3u C1 NA 0 {(5.40E-05*0.5*(W-(0.12u))*(L-(0.0))+3.80E-11*(L-(0.0)))*M} C2 NB 0 {(5.40E-05*0.5*(W-(0.12u))*(L-(0.0))+3.80E-11*(L-(0.0)))*M} ..ENDS RPOLYH * ---------------------------------------------------------------------- Thus I can do do a fit of Steinhart-Hart, with three point-pairs: R1, T1; R2, T2; R3, T3; then work backwards as you did, using PSpice's or LTspice's behavior language, to get to a standard subcircuit declaration. Good mind teasing! Thanks, Mark! ...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:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | The only thing bipartisan in this country is hypocrisy
From: neddie on 16 Apr 2010 08:46
On Apr 13, 7:58 pm, Joerg <inva...(a)invalid.invalid> wrote: > Hello Folks, > > Got stuck when trying to simulate an NTC. This temperature-variant > resistor will be the only variable input so ".STEP" and stuff do not cut > it because that only overlays multiple curve in an AC or DC simulation. > I want just one curve: Output of my circuit versus varying NTC resistor > value. > > Tried to make a voltage dependent resistor this way: > > http://www.electro-tech-online.com/attachments/general-electronics-ch... > > It works but is incredibly slow. Any better ideas? > > -- > Regards, Joerg > > http://www.analogconsultants.com/ > > "gmail" domain blocked because of excessive spam. > Use another domain or send PM. ..step temp 0 100 10 , with simulation command set to DC op point or am I missing something here. Rob |