 |
 | Home | Contact Us | FAQ | Search & Site Map | Link to Us |
 | Sign In | Join | Other 45 Sites in Network |
| HomeDiscussion GroupsElectronicsBasicsRepairDesignCADComponentsEquipmentElectrical Engineering ElectronicsKB.com Contact UsLink To UsSearch & Site Map |
Electronics Forum / CAD / March 2004SPICE (LT): determining dissipation by resistors, etc.?
Newbie question: What's the quick and easy way of finding the steady-state power dissipation of resistors and other components in a circuit with SPICE? .op gives me node voltage and device currents and, yep, I could do the simple math. How can I get SPICE to do it?  SignatureMike "Rocket J Squirrel" Elliott Mike, > What's the quick and easy way of finding the steady-state > power dissipation of resistors and other components in a > circuit with SPICE? > > .op gives me node voltage and device currents and, yep, > I could do the simple math. How can I get SPICE to do it? In LTspice, device power is only computed as part of an efficiency calculation in a .tran analysis, but since efficiency is only computed for SMPS's in steady state, it isn't of much use for general simulations. The easiest way to enter the simple math to plot the power dissipation of a resistor in a general simulation in LTspice is to do a .tran analysis and then drag the cross-probe cursor across the resistor so that now the differential voltage is plotted. Then right click on the plot label say, V(a,b), and edit it 1K*V(a,b), or what ever value of resistance you have. --Mike >Mike, > [quoted text clipped - 19 lines] > >--Mike Does LTSpice have "avg" and "avgx" functions like PSpice? If so, you can display the averaged power. ...Jim Thompson | James E.Thompson, P.E. | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona Voice:(480)460-2350 | | | E-mail Address at Website Fax:(480)460-2142 | Brass Rat | | http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food. >Does LTSpice have "avg" and "avgx" functions like PSpice? > >If so, you can display the averaged power. Jim, you need to dump PSpice *immediately* and get a copy of LT. Trust me. I know what I'm talking about. I think. :-) No, seriously! LT is *all* you need. Why pay oodles of dollars when you don't need to? Screw P. :P Signature"Windows [n.], A thirty-two bit extension and GUI shell to a sixteen bit patch to an eight bit operating system originally coded for a four bit microprocessor and produced by a two bit company." >>Does LTSpice have "avg" and "avgx" functions like PSpice? >> [quoted text clipped - 4 lines] >No, seriously! LT is *all* you need. Why pay oodles of dollars when >you don't need to? Graphing. PSpice has a few more graphing goodies than LTSpice offers. I find the Performance Analysis feature in PSpice to be very handy. Node voltage and device current annotation on the schematic. Don't know if LTSpice has this, but this sure is handy when trying to debug stuff. No, I'm not trashing LTSpice. I'm quite partial to LTSpice, especially since Mike is so responsive getting bugs fixed and adding features. When the graphing gets tough, gotta switch to PSpice. Mark >>>Does LTSpice have "avg" and "avgx" functions like PSpice? >>> [quoted text clipped - 17 lines] > >Mark Same here. Some of us have to do this for a living. (Actually LOVE to do this for a living... can't EVER pass up a challenge ;-) ...Jim Thompson | James E.Thompson, P.E. | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona Voice:(480)460-2350 | | | E-mail Address at Website Fax:(480)460-2142 | Brass Rat | | http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food. Mark, Jim, > >>>Does LTSpice have "avg" and "avgx" functions like PSpice? > >>> [quoted text clipped - 18 lines] > Same here. Some of us have to do this for a living. (Actually LOVE > to do this for a living... can't EVER pass up a challenge ;-) Yes, PSpice does still have more plotting features than LTspice, but LTspice has some that PSpice doesn't have. For example, in LTspice, you can sweep a parameter at a single frequency as in this deck: * I1 0 1 ac 1 L1 1 0 100u R1 1 0 100K C1 1 0 {C} .step oct param C 200p 300p 500 .ac list 1Meg .end Similarly, you can plot noise density at a single frequency vs. a parameter. There'll be more plotting features added to LTspice before the end of the year. Also, LTspice handles waveform data in a 64bit address space so the waveform files are unlimited in size. Designers find it more viable for doing full-chip, transistor-level simulations not only because of it's vastly superior solving capabilities over PSpice, but also because of it's improved data-handling for large data sets. --Mike >Yes, PSpice does still have more plotting features than >LTspice, but LTspice has some that PSpice doesn't have. [quoted text clipped - 9 lines] >.ac list 1Meg >.end Is this a new feature, Mike? I wasn't aware that LT had this highly useful capability. Signature"Windows [n.], A thirty-two bit extension and GUI shell to a sixteen bit patch to an eight bit operating system originally coded for a four bit microprocessor and produced by a two bit company." Paul, > >Yes, PSpice does still have more plotting features than > >LTspice, but LTspice has some that PSpice doesn't have. [quoted text clipped - 12 lines] > Is this a new feature, Mike? I wasn't aware that LT had this highly > useful capability. As I remember, it was there as part of the first release of LTspice that supported .step. That became a documented feature on Jan 8, 2002. An example of doing this for in a .noise simulation is in ./examples/Educational/stepnoise.asc. There you can see the diff pair tail resistance that gives the lowest input referenced noise density. --Mike > Mike, > [quoted text clipped - 17 lines] > and edit it 1K*V(a,b), or what ever value of resistance you > have. Hello Mike, something like V(a,b)*V(a,b)/10k is ok for DC, but what if I have a time dependent voltage V(a,b). I will need an integration of P(t) over time. Is there any hidden(not documented) command for integration? I would like something as s(...) . PROBE in PSPICE has this function. Best Regards Helmut Jim wrote: > Does LTSpice have "avg" and "avgx" functions like PSpice? Helmult wrote: > something like V(a,b)*V(a,b)/10k is ok for DC, but what Opps, sorry for the mistake. > if I have a time dependent voltage V(a,b). I will need an > integration of P(t) over time. > Is there any hidden(not > documented) command for integration? After you plot the instanteneous power with I(R1)*V(a,b) then you can integrate it to get the average and rms values by holding down the control key and left clicking on the plot trace's label. You control integration limits with the horizontal zoom of the plot. This Control-click to integrate gives different types of integrations for different analysis types. It will integrate noise in quadrature after a .noise analysis. It will give bandwidths after a .ac analysis. Sorry again about writting 1K*V(a,b) instead of I(R1)*V(a,b) for power. The method can be used for devices with more than two pins. For the power in a bipolar transistor, plot V(b)*Ib(Q1)+V(c)*Ic(Q1)+V(e)*Ie(Q1) Where V(b), V(c), and V(e) are base, collector, and emitter voltages. --Mike > Jim wrote: > [quoted text clipped - 18 lines] > analysis types. It will integrate noise in quadrature after a > .noise analysis. It will give bandwidths after a .ac analysis. Hello Mike, thanks for the tipp. I will remmeber always to try the powerful <control> key in the future if I miss some feature. Best Regards Helmut I miswrote: > ...Then right click on the plot label say, V(a,b), > and edit it 1K*V(a,b), or what ever value of resistance you > have.... Opps, wasn't thinking, you would then edit it to read V(a,b)*I(R1) to get instantaneous power. --Mike > Mike, > [quoted text clipped - 17 lines] > and edit it 1K*V(a,b), or what ever value of resistance you > have. To me, it's surprising that SPICE doesn't generate as a matter of course, the steady-state Pd for parts along with the usual voltage drop and current. But hey! I just want to make sure I order resistors big enough for the job -- I expect that the folks that create SPICEs seldom worry about that, or it would be part of the package. Thanks for the tip! SignatureMike "Rocket J Squirrel" Elliott Hi Mike, In Micro-Cap you plot PD(R1) (PD for power dissipated), where R1 is the name of the resistor. This essentially plots I(R1)^2*R(R1). You can also plot ED(R1) to see the energy dissipated during the run. To see average power you could use the AVG (average) function as in AVG(PD(R1)) You can get a demo version of Micro-Cap at www.spectrumn-soft.com. Cheers, Andy Thompson > Mike, > [quoted text clipped - 19 lines] > > --Mike >Hi Mike, > [quoted text clipped - 10 lines] > >Andy Thompson [snip] Gawwwd! Can't even correctly spell his own website ;-) ...Jim Thompson | James E.Thompson, P.E. | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona Voice:(480)460-2350 | | | E-mail Address at Website Fax:(480)460-2142 | Brass Rat | | http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food. Hi All, The correct web site for the Micro-Cap demo is: www.spectrum-soft.com Thanks to Jim Thompson for noticing this and pointing it out. Cheers, Andy Thompson > >Hi Mike, > > [quoted text clipped - 24 lines] > > I love to cook with wine. Sometimes I even put it in the food. Andy Thompson wrote: > Hi All, Hi Andy > The correct web site for the Micro-Cap demo is: > > www.spectrum-soft.com It's a beautiful site (gotta love your newsletters), but why would any serious designer in their right mind pay thousands of dollars for your software when they can get LTspice with its superior core functionality for free? (not just a rhetorical question, btw) LTspice surely by now must be noticeably eroding your market share and reducing your revenues. What is your strategy for dealing with this? Are you planning price reductions or perhaps cutting a licensing deal so that one of Linear Technology's competitors can offer a free simulator? Maybe National Semiconductor would be interested. > Thanks to Jim Thompson for noticing this and pointing it out. No thanks needed, I'm sure. Pointing out the foibles of others is one of his pleasures. -- analog > Cheers, > > Andy Thompson > Hi Mike, > > In Micro-Cap you plot PD(R1) (PD for power dissipated), where R1 is > the name of the resistor. This essentially plots I(R1)^2*R(R1). You > can also plot ED(R1) to see the energy dissipated during the run. To > see average power you could use the AVG (average) function as in In SuperSpice, you move the mouse over the component, dc power and ave. tran power is shown bottom right of main window. That's it, its all automatic. Oh, also, you just put a test point on the component to plot its power. Kevin Aylward salesEXTRACT@anasoft.co.uk http://www.anasoft.co.uk SuperSpice, a very affordable Mixed-Mode Windows Simulator with Schematic Capture, Waveform Display, FFT's and Filter Design. Mike, > What's the quick and easy way of finding the steady-state power > dissipation of resistors and other components in a circuit with SPICE? There's a new feature in version 2.07a. From a schematic, you can now plot the instantaneous power dissipation in a device. This is accessed by Alt-Left clicking on a symbol. It's computed as an expression of voltages and currents that are already in the data set. For example, if you Alt-click on a transistor, the trace you add might look like "V(N001,N003)*Ic(Q1)+V(N002,N003)*Ib(Q1)" Average power dissipation can be found by control clicking on this trace label to integrate. --Mike > Mike, > [quoted text clipped - 10 lines] > power dissipation can be found by control clicking > on this trace label to integrate. Awwww -- and it even comes with a cute little bulb thermometer symbol! Extremely handy addition, Mike. Many thanks! SignatureMike "Rocket J Squirrel" Elliott >> Mike, >> [quoted text clipped - 14 lines] > >Extremely handy addition, Mike. Many thanks! Reminds me of a simulation program from way back - Analog Artistry, I think. When the simulated component dissipation exceeded the part rating, a curl of smoke was displayed on the screen next to the part. > Reminds me of a simulation program from way back - Analog Artistry, >I think. > When the simulated component dissipation exceeded the part rating, >a curl of smoke was displayed on the screen next to the part. What an amusing and innovative idea! Signature"I expect history will be kind to me, since I intend to write it." - Winston Churchill >> Reminds me of a simulation program from way back - Analog Artistry, >> I think. >> When the simulated component dissipation exceeded the part rating, >> a curl of smoke was displayed on the screen next to the part. > > What an amusing and innovative idea! Amusing yes, innovative no. Innovative is a term to describe things that are reasonably new or unexpected. Since real components do smoke, the idea to have them do this on a schematic is trivially obvious. It was one I rejected a long time a go as a silly gimmick. Kevin Aylward salesEXTRACT@anasoft.co.uk http://www.anasoft.co.uk SuperSpice, a very affordable Mixed-Mode Windows Simulator with Schematic Capture, Waveform Display, FFT's and Filter Design. http://www.anasoft.co.uk/replicators/index.html Understanding, is itself an emotion, i.e. a feeling. Emotions or feelings can only be "understood" by consciousness. "Understanding" consciousness can therefore only be understood by consciousness itself, therefore the "hard problem" of consciousness, is intrinsically unsolvable. Physics is proven incomplete, that is, no understanding of the parts of a system can explain all aspects of the whole of such system. >Kevin Aylward >salesEXTRACT@anasoft.co.uk [quoted text clipped - 15 lines] >understanding of the parts of a system can >explain all aspects of the whole of such system. Kev, your sig appears to be a tad over the 4-line limit. Any chance of trimming it in the interests of saving B/W? Thanks. Signature"I expect history will be kind to me, since I intend to write it." - Winston Churchill : Mike, : > What's the quick and easy way of finding the steady-state power : > dissipation of resistors and other components in a circuit with SPICE? : There's a new feature in version 2.07a. From a schematic, : you can now plot the instantaneous power dissipation in a [quoted text clipped - 5 lines] : power dissipation can be found by control clicking : on this trace label to integrate. An axix labels with "Watts" would be usefull. Thanks for the feature! SignatureUwe Bonnes bon@elektron.ikp.physik.tu-darmstadt.de ======================================================= Free software means: Contribute nothing, expect nothing ======================================================= >Newbie question: > >What's the quick and easy way of finding the steady-state power >dissipation of resistors and other components in a circuit with SPICE? Here's a handy little trick I've used a couple of times. Use the arb. voltage source to multiply I*V then feed that into an RC model of the thermal characteristics of the heatsinking. The result is a nice plot of the temperature rise vs time when the circuit pulses on. Signature-- kensmith@rahul.net forging knowledge >>Newbie question: >> [quoted text clipped - 5 lines] >thermal characteristics of the heatsinking. The result is a nice plot of >the temperature rise vs time when the circuit pulses on. In CircuitMaker you just move the probe to the component until a P pops up (instead of V or I), and the power is shown automatically. SignatureTerry Pinnell Hobbyist, West Sussex, UK >>In article <zyyob.438$Bf7.374091@news1.news.adelphia.net>, >>Mike Rocket J. Squirrel Elliott [...] >>Here's a handy little trick I've used a couple of times. Use the arb. >>voltage source to multiply I*V then feed that into an RC model of the [quoted text clipped - 3 lines] >In CircuitMaker you just move the probe to the component until a P >pops up (instead of V or I), and the power is shown automatically. Yes but it doesn't plot the temperature rise. Signature-- kensmith@rahul.net forging knowledge > In article <zyyob.438$Bf7.374091@news1.news.adelphia.net>, > Mike Rocket J. Squirrel Elliott [quoted text clipped - 4 lines] >> dissipation of resistors and other components in a circuit with >> SPICE? In SuperSpice, simply move the mouse pointer over the component and power will be immediately displayed in a text field in the docked window, bottom right. Both bias power and transient power is displayed. Kevin Aylward salesEXTRACT@anasoft.co.uk http://www.anasoft.co.uk SuperSpice, a very affordable Mixed-Mode Windows Simulator with Schematic Capture, Waveform Display, FFT's and Filter Design. http://www.anasoft.co.uk/NewBeginning.mp3 "quotes with no meaning, are meaningless" - Kevin Aylward. >> In article <zyyob.438$Bf7.374091@news1.news.adelphia.net>, >> Mike Rocket J. Squirrel Elliott [quoted text clipped - 8 lines] >power will be immediately displayed in a text field in the docked >window, bottom right. Both bias power and transient power is displayed. In LT., simply multiply the voltage across the resistor by the current flowing through it. :-) SignatureThe BBC: Licensed at public expense to spread lies. >>>> What's the quick and easy way of finding the steady-state power >>>> dissipation of resistors and other components in a circuit with [quoted text clipped - 5 lines] >>> result is a nice plot of the temperature rise vs time when the >>> circuit pulses on. >>In SuperSpice, simply move the mouse pointer over the component and >>power will be immediately displayed in a text field in the docked >>window, bottom right. Both bias power and transient power is displayed. > >In LT., simply multiply the voltage across the resistor by the current >flowing through it. :-) I think Ken's point of his late post to the thread was that he got temperature vs time. But if you just want component dissipation in LTspice, you can Alt-Left click on a component to plot instantaneous dissipation of the component(The mouse cursor icon will turn into a thermometer when you're pointing at a plotable power dissipation). Then the waveform integrator can be used get the average dissipation over a period of the simulation. --Mike [...] >I think Ken's point of his late post to the thread was that he got >temperature vs time. Yes, exactly, that was the whole point. Using this trick you can model the temperature of a heatsink when there is a pulsed load. Often in a switcher, there is a part of the circuit that only needs to provide power for a short time when the circuit is switched on. Once the main section is up and going, a secondary takes over the load. Signature-- kensmith@rahul.net forging knowledge >>Newbie question: >> [quoted text clipped - 5 lines] > thermal characteristics of the heatsinking. The result is a nice plot of > the temperature rise vs time when the circuit pulses on. But how to convert a device + heatsink's thermal specs into an appropriate RC circuit? (Puzzle 1 for me.) And how to translate the simulation data into the device's junction temperature? (Puzzle 2 for me.) I'm lazy and hate doing thermal calcs by hand. SignatureMike "Rocket J Squirrel" Elliott 71 VW Type 2 -- the Wonderbus (AKA the Saunabus in summer) >But how to convert a device + heatsink's thermal specs into an >appropriate RC circuit? (Puzzle 1 for me.) And how to translate the >simulation data into the device's junction temperature? (Puzzle 2 for >me.) I'm lazy and hate doing thermal calcs by hand. Mike, what's your favourite Pizza topping? SignatureThe BBC: Licensed at public expense to spread lies. >>But how to convert a device + heatsink's thermal specs into an >>appropriate RC circuit? (Puzzle 1 for me.) And how to translate the >>simulation data into the device's junction temperature? (Puzzle 2 for >>me.) I'm lazy and hate doing thermal calcs by hand. > > Mike, what's your favourite Pizza topping? I'm pretty much a cheese guy. Cheese, tomato sauce, basil -- "Margherita" pizza just about does all I need. But artichoke hearts are good, too. SignatureMike "Rocket J Squirrel" Elliott 71 VW Type 2 -- the Wonderbus (AKA the Saunabus in summer) [.. modeling heat sinking ..] >But how to convert a device + heatsink's thermal specs into an >appropriate RC circuit? (Puzzle 1 for me.) And how to translate the >simulation data into the device's junction temperature? (Puzzle 2 for >me.) I'm lazy and hate doing thermal calcs by hand. The thermal resistance is in Watts per degree C. These you just call Ohms. The thermal mass looks like a capacitor with C = degree/J. Heat into the sink is just a current equal to I*V in the component. The outdoor temperature is just a voltage source at the far end of the circuit. Signature-- kensmith@rahul.net forging knowledge > [.. modeling heat sinking ..] > >>But how to convert a device + heatsink's thermal specs into an >>appropriate RC circuit? (Puzzle 1 for me.) And how to translate the >>simulation data into the device's junction temperature? (Puzzle 2 for >>me.) I'm lazy and hate doing thermal calcs by hand. Okay, looking at a standard part, like Aavid's 533522b02552 ( http://www.aavidthermalloy.com/bin/stdisp.pl?Pnum=533522b02552 ) It's spec'ced thermal resistance is 2.7 degree C / Watt. > The thermal resistance is in Watts per degree C. These you just call > Ohms. So R = the inverse of thermal resistance? With thermal resistance of 2.7 C/W, then R = 1/2.7 ohm: 0.37 ohm, yes? > The thermal mass looks like a capacitor with C = degree/J. Degree /Joule? I'm a bit simple -- this one I don't get. Does a heatsink data sheet provide sufficient information to calculate this number? > Heat into the sink is just a current equal to I*V in the component. The > outdoor temperature is just a voltage source at the far end of the > circuit. 25 degrees C ambient would be . . . 25 volts? SignatureMike "Rocket J Squirrel" Elliott 71 VW Type 2 -- the Wonderbus (AKA the Saunabus in summer) >> The thermal resistance is in Watts per degree C. These you just call >> Ohms. > >So R = the inverse of thermal resistance? With thermal resistance of 2.7 >C/W, then R = 1/2.7 ohm: 0.37 ohm, yes? Sorry I either (A) had brain lock or (B) had beer. I should have said that the heat sink makers usually give you Watts per degree. From that you calculate the resistance in Degrees per Watt. >> The thermal mass looks like a capacitor with C = degree/J. > >Degree /Joule? I'm a bit simple -- this one I don't get. Does a heatsink >data sheet provide sufficient information to calculate this number? Brain trouble here too. If you use an alluminum heat sink each gram of metal is good for 0.9uF For copper or brass, a gram is about 0.38uF. >25 degrees C ambient would be . . . 25 volts? This one I got right. Signature-- kensmith@rahul.net forging knowledge I obviously am having an advanced case of brain lock or too much beer. After checking my notes here's the right answers (I hope): [.. I wrote ..] >> The thermal resistance is in Watts per degree C. These you just call >> Ohms. > >So R = the inverse of thermal resistance? With thermal resistance of 2.7 >C/W, then R = 1/2.7 ohm: 0.37 ohm, yes? No I meant to say that the data sheet I'd looked at gave you Watts per degree. The Degrees per Watt is the right form to do resistance. >> The thermal mass looks like a capacitor with C = degree/J. > >Degree /Joule? I'm a bit simple -- this one I don't get. Does a heatsink >data sheet provide sufficient information to calculate this number? Another mistake, it is C=J/degree. I measured degree/J because that is the easy way to make the measurement and then inverted. The capacitor looks like 0.9F per gram if it is alluminum. Copper and brass are more like 0.38F per gram. >25 degrees C ambient would be . . . 25 volts? Yes. Signature-- kensmith@rahul.net forging knowledge > I obviously am having an advanced case of brain lock or too much beer. > After checking my notes here's the right answers (I hope): [quoted text clipped - 23 lines] > > Yes. Hey -- I figured one out myself! Thanks for going back over this and clearing things up. So if a fellow wanted to know the junction temperature of a power device mounted on a heatsink, all he'd need to so is stick in a second R in series with the RC network, and give it the value of the device's specified junction-to-mounting surface thermal resistance. I'm going to play with this a bit and see how it works. In LTspice it should be easy to create a heatsink symbol for use on the schematic. Easy for some -- Mike, Helmut and analogspiceman could slam-dunk it. Me, I'll slog at it. BTW: where did the capacitor numbers for aluminum and copper/brass come from? SignatureMike "Rocket J Squirrel" Elliott 71 VW Type 2 -- the Wonderbus (AKA the Saunabus in summer) [...] >> the easy way to make the measurement and then inverted. The capacitor >> looks like 0.9F per gram if it is alluminum. Copper and brass are more >> like 0.38F per gram. [...] >BTW: where did the capacitor numbers for aluminum and copper/brass come >from? The value for C is the "specific heat" of the material times its mass. The CRC list Al having a specific heat of 0.215 in cal/(gK) units. You multiply cal by 4.184 to get J so 0.215 * 4.184=0.89956 or 0.9. Signature-- kensmith@rahul.net forging knowledge > > I obviously am having an advanced case of brain lock or too much beer. > > After checking my notes here's the right answers (I hope): [quoted text clipped - 37 lines] > BTW: where did the capacitor numbers for aluminum and copper/brass come > from? Hello Mike, I have looked for some literature with Google about thermal transistor and heatsink models. http://www.iisb.fraunhofer.de/en/arb_geb/powersys_thermmod_gb_fhg.pdf http://www.infineon.com/cmc_upload/migrated_files/document_files/Appli cation_Notes/mmpn_eng.pdf http://www.fairchildsemi.com/an/AN/AN-7533.pdf http://www.irf.com/technical-info/designtp/temp002.pdf http://www.irf.com/product-info/datasheets/data/100bgq045.pdf They are all based on the equation Tfinal=Pv*Rth with an exponential temperature rise from Tamb to Tfinal. The most important question now is, how can we influence the transistor(NPN, MOS) during a simulation run. My understanding about(LT,P-)SPICE is, that there is no chance to do that with the basic transistor models. What I have seen in the above articles is that they build more or less complex circuits around the basic transistor models. Is that the only way to get temperature dependent transistor behaviour with SPICE transistor models in a .TRAN simulation? Best Regards, Helmut >> > I obviously am having an advanced case of brain lock or too much beer. >> > After checking my notes here's the right answers (I hope): [quoted text clipped - 68 lines] >Best Regards, >Helmut What is lacking in Spice is that the thermal model will not affect the TA that the device model sees :-( ...Jim Thompson | James E.Thompson, P.E. | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona Voice:(480)460-2350 | | | E-mail Address at Website Fax:(480)460-2142 | Brass Rat | | http://www.analog-innovations.com | 1962 | "Will you love me when I'm sixty-four?" > >Newbie question: > > [quoted text clipped - 5 lines] > thermal characteristics of the heatsinking. The result is a nice plot of > the temperature rise vs time when the circuit pulses on. Hi Ken, very interesting stuff but I am confused. Above you state, "a voltage source to drive the RC model". Should not that be a current source as the heat generating driving element? The current output would be the power dissipated. 25amps = 25watts. Regards Harry >> In article <zyyob.438$Bf7.374091@news1.news.adelphia.net>, >> Mike Rocket J. Squirrel Elliott [quoted text clipped - 18 lines] > source as the heat generating driving element? The current output > would be the power dissipated. 25amps = 25watts. One use a Thevenin or Norton equivalent circuit. Putting a current source into a series RC circuit will result in an infinite temperature (voltage) in steady state!!! Kevin Aylward salesEXTRACT@anasoft.co.uk http://www.anasoft.co.uk SuperSpice, a very affordable Mixed-Mode Windows Simulator with Schematic Capture, Waveform Display, FFT's and Filter Design. http://www.anasoft.co.uk/NewBeginning.mp3 "quotes with no meaning, are meaningless" - Kevin Aylward. > >> In article <zyyob.438$Bf7.374091@news1.news.adelphia.net>, > >> Mike Rocket J. Squirrel Elliott [quoted text clipped - 24 lines] > > Kevin Aylward But, but doesn't this current flow thru the thermal resistances and finally end at a voltage source which is the ambient temperature or infinite heat sink? It may get slowed down along the way by shunt capacity (thermal mass). Regards Harry [.. RC model of thermal ..] > But, but doesn't this current flow thru the thermal resistances and >finally end at a voltage source which is the ambient temperature or infinite >heat sink? It may get slowed down along the way by shunt capacity (thermal >mass). Yes, the current (heat) flows through the resistance (thermal r) to go to a voltage (outside temperature). Capacitance does the thermal mass. Signature-- kensmith@rahul.net forging knowledge [...] >> Here's a handy little trick I've used a couple of times. Use the arb. >> voltage source to multiply I*V then feed that into an RC model of the >> thermal characteristics of the heatsinking. The result is a nice plot of >> the temperature rise vs time when the circuit pulses on. [...] > Hi Ken, very interesting stuff but I am confused. Above you state, "a >voltage source to drive the RC model". Should not that be a current source >as the heat generating driving element? The current output would be the >power dissipated. 25amps = 25watts. Sorry about the slight muddle on that. Yes a current source is the right answer if the model you use is a more or less direct model of the real heat sink. If you use resistance to model thermal resistance and capacitance to model thermal mass, you use a current source. If you have just a pre-calculated thermal time constant, you can just use a voltage source and the right RC value to make the right time constant. Signature-- kensmith@rahul.net forging knowledge >>In article <zyyob.438$Bf7.374091@news1.news.adelphia.net>, >>Mike Rocket J. Squirrel Elliott [quoted text clipped - 15 lines] > as the heat generating driving element? The current output would be the > power dissipated. 25amps = 25watts. Harry, I'm glad you saw that. I thought that a voltage source was incorrect, too, but knowing that I rank in the bottom 10 percentile of brainpower for sci.electronics.cad, I doubted myself. Thanks for bringing it up. SignatureMike "Rocket J Squirrel" Elliott 71 VW Type 2 -- the Wonderbus (AKA the Saunabus in summer) "Mike Rocket J. Squirrel Elliott" <j.michael.elliottAT@REMOVETHEOBVIOUSadelphiaDOT.net> wrote in message news:b-> >>kensmith@rahul.net forging knowledge > > Hi Ken, very interesting stuff but I am confused. Above you state, "a > > voltage source to drive the RC model". Should not that be a current source [quoted text clipped - 5 lines] > brainpower for sci.electronics.cad, I doubted myself. Thanks for > bringing it up. Hey Rocket, even a blind squirrel will find some nuts. Harry > "Mike Rocket J. Squirrel Elliott" > <j.michael.elliottAT@REMOVETHEOBVIOUSadelphiaDOT.net> wrote in message [quoted text clipped - 14 lines] > > Hey Rocket, even a blind squirrel will find some nuts. This is probably more akin to chimps and typewriters. SignatureMike "Rocket J Squirrel" Elliott 71 VW Type 2 -- the Wonderbus (AKA the Saunabus in summer) |
Reply to this Message |
 Sign In
 Join
 My Latest Posts My Monitored Threads My Blog My Photo Gallery My Profile My Homepage Start New Thread Enable EMail Alerts Rate this Thread
|
©2009 Advenet LLC Privacy Policy - Terms of Use
This website includes both content owned or controlled by Advenet as well as content owned or controlled by third parties.