EDN 1994 Design Idea: Spice does thermal analysis - missing files

[busaboy]

EEVblog member @mawyatt wrote an EDN Design Idea in 1994 titled "Spice does thermal analysis". Unfortunately EDN doesn't provide access to old content and Mike doesn't have the Spice files anymore.

Can anyone help with di1576z.zip?

https://www.edn.com/edn-access-08-18-94-spice-runs-thermal-analysi/

[CatalinaWOW]

What are you looking for?  Values for components?  Only a little that was in use at the time this article was written would be pertinent to todays components.

The idea is simple enough.  Model thermal masses as capacitances and heat conduction paths as resistances.  Heat capacities of common materials are readily available on line, as are conductivities.  Thermal resistance of many packages can be found in data sheets.  Some things need to be fudged.  Radiative and convective heat transfer don't really model simply and are probably best dealt with by a rational approximation to measured data.  And three dimensional heat flow such as lateral flow in a circuit board, or transfer to a large heat sink from a dimensionally small heat source will have to be simplified to a network of thermal resistors.  But when you get that complex it probably makes sense to use more traditional thermal model. 

As always models are simplifications of the real world and need to be validated by comparison with measured data before you really believe the results.

[busaboy]

Looking for the original Spice sub-circuits with formulas.

Trying to add more simulation examples for Qucs-S. I already have examples using the rare Manufacturer supplied "thermal" Spice models. The issue is how to do thermal modeling using old Spice models or the vast majority of power devices that don't come with a thermal Spice model. It's useful for Hobbyists building audio power amplifiers.

https://github.com/ra3xdh/qucs_s/discussions

[RoGeorge]

You started this topic twice. 
Please do not duplicate the same subject (it's one of the rules to keep this forum clean).

If you forgot where did you wrote before, go to "Profile" -> "Summary" -> "Show Posts", or bookmark this link:  https://www.eevblog.com/forum/profile/?area=showposts

It is also possible to edit your own posts, or to move your own topics to another section of the forum (in case you accidentally opened them in a wrong section).


@ in front of a username doesn't work on this forum, so it doesn't send a mention notification.


That simulation looks like it doesn't depend on any specific/custom files or models.  The thermal model is in the topology of the schematic itself, and in the values for the particular thermal R and C.

Should be enough to just redraw the schematic in your preferred simulator.


Spice can do temperature simulations, for example can account for Vbe variations with temperature, or for the thermal coeficients of resistors, etc., but that is something else.

I think the article is not about those spice features, but rather about modeling the thermal effects using an electric analog.  Random link example for an analog of thermal effects using electric circuits:
http://web.mit.edu/16.unified/www/FALL/thermodynamics/notes/node118.html

In a similar way, there is an equivalence between mechanical and electrical circuits, so for example mechanical behavior can be also simulated with a SPICE model:
https://en.wikipedia.org/wiki/Mechanical%E2%80%93electrical_analogies

[iMo]

FYI - https://www.eevblog.com/forum/metrology/lm399-heat-loss-within-a-vacuum/msg4392685/#msg4392685

PS: one of the great issues with Spice (LTspice, etc.) since ever is there is none "on-the fly" feedback of the actual Temperature (the temperature of a particular part) into its intrinsic models.

Having that would be a fundamental breakthrough.

You may easily model a schematics where, for example, a power loss of a 2N2222 transistor will be 100W (and its temperature say 700C) and it still will show nice results. Today LTspice assumes everything in your schematics is "kept" at the set global Temperature, like the default 27degC. You may "step" through temperature, but each individual step means that you change the global temperature to a certain value, and again, all in your schematics is kept at that temperature during the entire simulation run within the set step.. Also you may assign an individual temperature to a certain part, but again, it will stay constant during the entire simulation run.
That is a real world nonsense, of course..

To create an actual temperature of something is easy in the Spice as you may derive it from the power loss which is accessible anytime, but there is none mechanism to feed it back into the intrinsic models (diodes, transistors, resistors, etc.).. Also modeling of the temperature gradients and flows in the Spice is easy even today (provided you have on the actual temperature based behavior of the parts handy, what is not the case today).

I asked on this problem at the ADI's EZone forum (where LTspice developers sit), after a short discussion the guys there indicated "..it would require almost complete rewrite.." of the LTspice.

Btw., there is everything you need in the Spice to do it, as all its intrinsic models ARE ALREADY a function of Temperature (the temperature is an internal variable in the models, like any currents/voltages)..

Thus all what needs to be done is to SIMPLY expose the internal intrinsic model's temperature variable such we may wire it somewhere (where we created the actual temperature value).

So instead of a single global CONSTANT Temperature (as is today) we will have N_x temperature VARIABLES (where N is the number of the LTspice's intrinsic models, perhaps 15-20), applicable to each specific part in the schematics individually (as the part's parameter into which we will wire our temperature_value generating node).
Like Q1_Q_BIP3_temp, Q23_Q_MOS2_temp, D3_D_temp, D6_D_temp, R7_R_temp..
When not wired/set by the user in the schematics the default global Temperature will be used.

I encouraged them to go for it.. 

[mawyatt]

EEVblog member @mawyatt wrote an EDN Design Idea in 1994 titled "Spice does thermal analysis". Unfortunately EDN doesn't provide access to old content and Mike doesn't have the Spice files anymore.

Can anyone help with di1576z.zip?

https://www.edn.com/edn-access-08-18-94-spice-runs-thermal-analysi/

Tom,

Wish we could find the original set of files, but they are long gone!! As mentioned in our message discussion which may be helpful for others, the thermal models we developed back then in 80~90s were based upon measurements.

For various package types (TO3, TO220, TO18, etc) we created models based upon using a device diode or BE junction as an internal temperature sensor. For example, we used a 2N3055 for a TO3 model and used the BE junction at a constant small current and measured the Vbe at room temp, then heating the TO3 to 100C, after awhile and measure Vbe. This gives an assumed linear Vbe response to temperature. Then use this TO3 2N3055 on a massive heatsink at a given power to create a significant temperature delta across the junction to heatsink and measure the Vbe, the TO3 case, and the heatsink temperatures. From this one can glean the thermal impedances of the junction to case, and case to heatsink.

Getting the thermal mass is more involved and requires recording the temperature vs. time profiles of the junction temperature (via Vbe) and the case to ambient, and also another test of junction temperature (Vbe) with case to massive heatsink, under long pulsed responses. From this a curve fit allows the case thermal mass to be estimated.

We did this, actually had grad students & post docs do the work for all the various case types we used and also similar types of measurements for other components where temperature performance was an important parameter.

Later this work led to actual thermal modeling within our custom chip designs and packages which included time domain transient thermal effects. We had created our own custom simulators back then based upon Spice for use with MW/MMW custom chip developments and all this was quite advanced at the time (we even had time domain noise models). Much later IBM introduced second order thermal models for their advanced SiGe BiCMOS IC processes we were using, these included proximity effects and 2nd order thermal dynamics which eventually became supported by Cadence.

Best

[busaboy]

I have thermal simulations for SiC Mosfet, IGBT and GaN devices using Manufacturers supplied thermal models. These models show parameter degradation over temperature (see attached GaN simulation) and will "blow up" when Tj gets too hot. Unfortunately these models are only available for limited devices.

I also have simulations using the LTspice and ngspice simplified VDMOS thermal model. The thermal model adds Rthjc and Cthj to existing Spice files. The simulations do not show parameter degradation over temperature however. My goal is to do similar for BJT devices.

Attached is an experiment in Qucs-S/ngpice to replicate what was done in the EDN Design Idea. (see attached) The "add-on" circuit still needs additional stages and the the conversion formulas.

These simulations are to expose Users to electro-thermal modeling. The simulations are not expected to be accurate. They are useful as teaching aids and for hobbyists.

[busaboy]

I think I got it. Attached is the Author's circuit and my original one.

[mawyatt]

Nice work

Best

[hvogt]

This is my tutorial on electro-thermal simulation with ngspice: https://ngspice.sourceforge.io/ngspice-electrothermal-tutorial.html .

[busaboy]

User has simplified the circuit using B sources like Holger's presentation above.

[tggzzz]

This is my tutorial on electro-thermal simulation with ngspice: https://ngspice.sourceforge.io/ngspice-electrothermal-tutorial.html .

Thanks

Bookmarked for later study.