Simulating a variable resistance input with LTSpice?
in [Design]
|
Prev: unexpected delay in a TWT
Next: memristors
From: Jim Thompson on 13 Apr 2010 16:20 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? Sorry, Joerg, I misread your need. It's actually quite simple, IF you can describe the TC with coefficients of T and T^2... make your own resistor model: Resistor General form R<name> <(+) node> <(-) node> [model name] <value> + [TC = <TC1> [,<TC2>]] TC1, and TC2 are the linear and squared coefficients, respectively. See the LTspice manual for clarity (the above was pasted from PSPCREF.pdf) ...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: Helmut Sennewald on 13 Apr 2010 17:08 "John Larkin" <jjlarkin(a)highNOTlandTHIStechnologyPART.com> schrieb im Newsbeitrag news:sfd9s511ormdiedjk9o725omcntmkttgpq(a)4ax.com... > 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? > > Do you need a voltage to resistance converter? That's easy if you have > a multiplier. Interestingly, LT Spice doesn't provide a multiplier > component. > > John Hello John, LTspice has B-deviecs. They can do a lot of math. * ** power / divide sin tanh exp See the help pages for B-devices. The B-device is the best device to implement a NTC-resistor with it's exponential resistance versus temperature function. The LTspice Yahoo group provides examples. Best regards, Helmut
From: Joerg on 13 Apr 2010 18:10 Jim Thompson 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? > > Sorry, Joerg, I misread your need. It's actually quite simple, IF you > can describe the TC with coefficients of T and T^2... make your own > resistor model: > > Resistor > > General form > > R<name> <(+) node> <(-) node> [model name] <value> > + [TC = <TC1> [,<TC2>]] > > TC1, and TC2 are the linear and squared coefficients, respectively. > > See the LTspice manual for clarity (the above was pasted from > PSPCREF.pdf) > In the current case it's a whole lot uglier than that, see under "Inverse of the equation": http://en.wikipedia.org/wiki/Steinhart%E2%80%93Hart_equation T (Temperature) must be scooted. I think LTSpice will have a cow when I try this. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
From: John Larkin on 13 Apr 2010 20:03 On Tue, 13 Apr 2010 23:08:23 +0200, "Helmut Sennewald" <helmutsennewald(a)t-online.de> wrote: >"John Larkin" <jjlarkin(a)highNOTlandTHIStechnologyPART.com> schrieb im >Newsbeitrag news:sfd9s511ormdiedjk9o725omcntmkttgpq(a)4ax.com... >> 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? >> >> Do you need a voltage to resistance converter? That's easy if you have >> a multiplier. Interestingly, LT Spice doesn't provide a multiplier >> component. >> >> John > > >Hello John, > >LTspice has B-deviecs. They can do a lot of math. >* >** power >/ divide >sin >tanh >exp > >See the help pages for B-devices. >The B-device is the best device to implement a NTC-resistor >with it's exponential resistance versus temperature function. > >The LTspice Yahoo group provides examples. > >Best regards, >Helmut > > > Sure, but a canned multiplier component would be handy, without a bunch of typing. As would an ideal diode. At least they have ideal opamps. John
From: Jim Thompson on 13 Apr 2010 20:14
On Tue, 13 Apr 2010 15:10:51 -0700, Joerg <invalid(a)invalid.invalid> wrote: >Jim Thompson 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? >> >> Sorry, Joerg, I misread your need. It's actually quite simple, IF you >> can describe the TC with coefficients of T and T^2... make your own >> resistor model: >> >> Resistor >> >> General form >> >> R<name> <(+) node> <(-) node> [model name] <value> >> + [TC = <TC1> [,<TC2>]] >> >> TC1, and TC2 are the linear and squared coefficients, respectively. >> >> See the LTspice manual for clarity (the above was pasted from >> PSPCREF.pdf) >> > >In the current case it's a whole lot uglier than that, see under >"Inverse of the equation": > >http://en.wikipedia.org/wiki/Steinhart%E2%80%93Hart_equation > >T (Temperature) must be scooted. I think LTSpice will have a cow when I >try this. Then use a resistance vs temperature table... trivial in PSpice, probably so in LTspice. Besides, that smells like unnecessary obfuscation :-) What kind of NTC? They're usually spec's as R = Ro*e^(beta*(1/T-1/To)) ...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 |