Simulating a variable resistance input with LTSpice?
in [Design]
|
Prev: unexpected delay in a TWT
Next: memristors
From: Joerg on 13 Apr 2010 15:30 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? > > Get this file... > > VVR.zip VOLTAGE VARIABLE RESISTOR SYMBOL/SUBCIRCUIT > > On the Subcircuits and Symbols Page of my website. > > It's just a text file... all you care about is the "Template" line. > Thanks, will check it out. Got the circuit pretty much done by now but some day if I get more of those little temp sense projects I want to pour the Steinhart-Hart equation in there. Then I'd have a true temperature-variable resistor. LTSpice has the nice feature of being able to read in a WAV table. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
From: Joerg on 13 Apr 2010 15:33 Fred Bartoli wrote: > Joerg a �crit : >> 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? >> > > The way I'd do it is with a B current source (OK, sink). > Basically you measure voltage across the NL resistor nodes (a,b) and > sink a current between these nodes which is your NL function of V(a,b). > That's a good idea. Right now I map a variable voltage source into a resistor. Works, but leaves one weirdness: kiloohms on the horizontal scale are labeled kilovolts. > That also better handles the R=0 pathological case, because you're less > tempted to allow infinite current flow :-) > I always wondered if there'd be a way to inlude a phssst ... *POOF* function in LTSpice, with audio effects, sirens and all. That would be nice to have during a design review :-) -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
From: Jim Thompson on 13 Apr 2010 15:44 On Tue, 13 Apr 2010 12:30:03 -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? >> >> Get this file... >> >> VVR.zip VOLTAGE VARIABLE RESISTOR SYMBOL/SUBCIRCUIT >> >> On the Subcircuits and Symbols Page of my website. >> >> It's just a text file... all you care about is the "Template" line. >> > >Thanks, will check it out. Got the circuit pretty much done by now but >some day if I get more of those little temp sense projects I want to >pour the Steinhart-Hart equation in there. Then I'd have a true >temperature-variable resistor. LTSpice has the nice feature of being >able to read in a WAV table. Read up on behavioral modeling techniques... lots of simulation power there. ...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: Fred Bartoli on 13 Apr 2010 15:50 Joerg a �crit : > Fred Bartoli wrote: >> Joerg a �crit : >>> 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? >>> >> >> The way I'd do it is with a B current source (OK, sink). >> Basically you measure voltage across the NL resistor nodes (a,b) and >> sink a current between these nodes which is your NL function of V(a,b). >> > > That's a good idea. Right now I map a variable voltage source into a > resistor. Works, but leaves one weirdness: kiloohms on the horizontal > scale are labeled kilovolts. > > >> That also better handles the R=0 pathological case, because you're >> less tempted to allow infinite current flow :-) >> > > I always wondered if there'd be a way to inlude a phssst ... *POOF* > function in LTSpice, with audio effects, sirens and all. That would be > nice to have during a design review :-) > Some XSPICE simulators allow you to monitor values during simulation and do almost whatever you want. The one I use handles wave files, so maybe :-) -- Thanks, Fred.
From: Jim Thompson on 13 Apr 2010 15:53
On Tue, 13 Apr 2010 11:26:12 -0700, John Larkin <jjlarkin(a)highNOTlandTHIStechnologyPART.com> 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? > >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 Loosen up them thar spats, the multiplier "element" is "*" :-) As in... Emult Outnode1 Outnode2 Value = {(Vinnode1,0)*(Vinnode2,0)} [Snicker :-] ...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 |