Simulating a variable resistance input with LTSpice?
in [Design]
|
Prev: unexpected delay in a TWT
Next: memristors
From: Jim Thompson on 17 Apr 2010 15:43 On Sat, 17 Apr 2010 12:38:29 -0700, Joerg <invalid(a)invalid.invalid> wrote: >Jim Thompson wrote: >> On Sat, 17 Apr 2010 08:58:58 -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: >>> >>> [snip] >>>> ********************************************************* >>>> * 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, >>> >>> Saturday morning, time to muse over adding your thermistor equation to >>> my symbol and model libraries, and studying the Steinhart-Hart >>> equations for "R", I wondered why you needed to use "PWRS"? >>> >>> They way I read those equations, "x" is always greater than "y/2", so >>> simply PWR, or even **(1/3) should suffice. >>> >>> Or am I overlooking a trap (like, can B/3C be negative ?:-) >>> >>> Thanks! >>> >>> ...Jim Thompson >> >> And it looks like "standard" data is resistance versus temperature >> tables, rather than specifying A, B & C. Is that typical, or am I not >> looking in the right places? >> > >That is the standard for NTC. Probably because the big market for them >is industrial control and the usual PLC can't do much more than simple >ladder logic. > >Also, those things have large tolerances so there ain't no real >precision. However, if you run a tight PID control with them the table >surely doesn't cut it. > > >> It _would_ be easy enough to specify the subcircuit with parameter >> pairs, R1/T1, R2/T2, R3/T3, then have the behavioral model compute A, >> B & C. >> > >Most of the times when I try this the PC starts to bog down. And heat >the office which is nice these days but not in August :-) I run a _real_ simulator :-) Got a table of values I can try out my model on? My guess is it'll run in seconds. ...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: Joerg on 17 Apr 2010 16:07 Jim Thompson wrote: > On Sat, 17 Apr 2010 12:38:29 -0700, Joerg <invalid(a)invalid.invalid> > wrote: > >> Jim Thompson wrote: >>> On Sat, 17 Apr 2010 08:58:58 -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: >>>> >>>> [snip] >>>>> ********************************************************* >>>>> * 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, >>>> >>>> Saturday morning, time to muse over adding your thermistor equation to >>>> my symbol and model libraries, and studying the Steinhart-Hart >>>> equations for "R", I wondered why you needed to use "PWRS"? >>>> >>>> They way I read those equations, "x" is always greater than "y/2", so >>>> simply PWR, or even **(1/3) should suffice. >>>> >>>> Or am I overlooking a trap (like, can B/3C be negative ?:-) >>>> >>>> Thanks! >>>> >>>> ...Jim Thompson >>> And it looks like "standard" data is resistance versus temperature >>> tables, rather than specifying A, B & C. Is that typical, or am I not >>> looking in the right places? >>> >> That is the standard for NTC. Probably because the big market for them >> is industrial control and the usual PLC can't do much more than simple >> ladder logic. >> >> Also, those things have large tolerances so there ain't no real >> precision. However, if you run a tight PID control with them the table >> surely doesn't cut it. >> >> >>> It _would_ be easy enough to specify the subcircuit with parameter >>> pairs, R1/T1, R2/T2, R3/T3, then have the behavioral model compute A, >>> B & C. >>> >> Most of the times when I try this the PC starts to bog down. And heat >> the office which is nice these days but not in August :-) > > I run a _real_ simulator :-) > For circuit level design I have yet to find anything I need where LTSpice can't do something that PSpice does. Chip design is probably different, I guess there comes a limit in terms of BSIM model support and so on. > Got a table of values I can try out my model on? Here ya go: http://www.epcos.com/inf/50/db/ntc_06/SMD__NiBarrier__0402__B572x1__V2x1.pdf > My guess is it'll run in seconds. > On its own it always does but once it's in the middle of a rather dense concoction of analog parts that quickly changes. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
From: Jim Thompson on 17 Apr 2010 16:13 On Sat, 17 Apr 2010 13:07:25 -0700, Joerg <invalid(a)invalid.invalid> wrote: >Jim Thompson wrote: >> On Sat, 17 Apr 2010 12:38:29 -0700, Joerg <invalid(a)invalid.invalid> >> wrote: [snip] >> >> I run a _real_ simulator :-) >> > >For circuit level design I have yet to find anything I need where >LTSpice can't do something that PSpice does. Chip design is probably >different, I guess there comes a limit in terms of BSIM model support >and so on. > > >> Got a table of values I can try out my model on? > > >Here ya go: > >http://www.epcos.com/inf/50/db/ntc_06/SMD__NiBarrier__0402__B572x1__V2x1.pdf > > >> My guess is it'll run in seconds. >> > >On its own it always does but once it's in the middle of a rather dense >concoction of analog parts that quickly changes. That part should end up all being linear Algebra. Does temperature change in ns ?? ...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: Joerg on 17 Apr 2010 16:44 Jim Thompson wrote: > On Sat, 17 Apr 2010 13:07:25 -0700, Joerg <invalid(a)invalid.invalid> > wrote: > >> Jim Thompson wrote: >>> On Sat, 17 Apr 2010 12:38:29 -0700, Joerg <invalid(a)invalid.invalid> >>> wrote: > [snip] >>> I run a _real_ simulator :-) >>> >> For circuit level design I have yet to find anything I need where >> LTSpice can't do something that PSpice does. Chip design is probably >> different, I guess there comes a limit in terms of BSIM model support >> and so on. >> >> >>> Got a table of values I can try out my model on? >> >> Here ya go: >> >> http://www.epcos.com/inf/50/db/ntc_06/SMD__NiBarrier__0402__B572x1__V2x1.pdf >> >> >>> My guess is it'll run in seconds. >>> >> On its own it always does but once it's in the middle of a rather dense >> concoction of analog parts that quickly changes. > > That part should end up all being linear Algebra. Does temperature > change in ns ?? > No, but once in a while one must monitor temperature pulses or fast trends. Usually to dodge a phut ... *BOOM* situation. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
From: qrk on 18 Apr 2010 11:57
On Sat, 17 Apr 2010 10:42:27 -0700, Jim Thompson <To-Email-Use-The-Envelope-Icon(a)On-My-Web-Site.com> wrote: >On Sat, 17 Apr 2010 08:58:58 -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: >> >>[snip] >>> >>>********************************************************* >>>* 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, >> >>Saturday morning, time to muse over adding your thermistor equation to >>my symbol and model libraries, and studying the Steinhart-Hart >>equations for "R", I wondered why you needed to use "PWRS"? >> >>They way I read those equations, "x" is always greater than "y/2", so >>simply PWR, or even **(1/3) should suffice. >> >>Or am I overlooking a trap (like, can B/3C be negative ?:-) >> >>Thanks! >> >> ...Jim Thompson > >And it looks like "standard" data is resistance versus temperature >tables, rather than specifying A, B & C. Is that typical, or am I not >looking in the right places? > >It _would_ be easy enough to specify the subcircuit with parameter >pairs, R1/T1, R2/T2, R3/T3, then have the behavioral model compute A, >B & C. > > ...Jim Thompson Standard are tables, not the A B C coeffs. I had an app note with the equations on it (too lazy to do arithmetic) which I solved in Mathcad using 3 points, but you can probably use Excel. Seems like a lot of work for PSpice to solve the coefficients. -- Mark |