SOAtherm-NMOS symbol missing in LTspice XVII

Question

I am trying to follow the tutorial for Modeling Safe Operating Area Behavior of N-Channel MOSFETs ( https://www.analog.com/en/technical-articles/ltspice-modeling-safe-operating-area-behavior-of-n-channel-mosfets.html ), but LTspice XVII does not have the SOAtherm-NMOS symbol that is used in the tutorial.

AnneM · Accepted Answer

jgavin - I've been informed that the SOAtherm-NMOS symbol has been obsoleted, and this functionality now works without needing that symbol. 
 
 See SOAtherm-Tutorial.asc in the examples/educational directory)

helmuts · Answer

Hello, 
 The symbol SOAtherm-nmos.asy has been removed. 
 Excerpt from the file changelog.txt : 01/18/19 Removed the obsoleted SOA accounting files from new installations. 
 If you had installed LTspiceXVII before this date, the symbol is still t here, because LTspice hasn't removed it in the newer version. 
 Even if you still have this out-dated symbol, you can't use it anymore, because the model-file belonging to this symbol has been removed by the later versions of LTspiceXVII. 
 In the old way of SOAterm, a subcircuit has been used for this model in the simulation. I guees it had increased the simulation time too much. 
 
 The new method of SOAtherm: 
 First I recommend to run the example from the folder Examples . 
 C:\Users\yourname\Documents\LTspiceXVII\examples\Educational\SOAtherm-Tutorial.asc 
 When the simulation of this example has finished, it plots tj#q1 and tc#q1. The default ambient temperature is 85&deg;C. You can change the assumed ambient temperature with the procedure below. 
 CTRL-right-mouse-click on the Mosfet -> a dialog box will appear Enter in SpiceLine Tambient=50 Click on "Vis"in this line, if you want make this parameter visible in the schematic OK 
 VDMOS-models which have thermal parameters can be identified by looking for the parameter "Rtheta" in its VDMOS model. Only a small percentage of the models have thermal data. The thermal calculations are only done if the following SPICE-directive is in the schematic. 
 .options SOAaccounting=1 
 Helmut

helmuts · Answer

Hello gian6, 
 The few mosfets with thermal models in LTspice seems to assume that the Mosfet is mounted on a PCB. One cannot add a heatsink. 
 If you have a thermal model with R and C of the Mosfet of interest, you could add your own thermal model. This RC-ladder network will be fed by a current proportional to the power dissipation of the Mosfet. A current source Bi can be used to calculate the power dissipation. It's current will be fed to the thermal RC-ladder network. The Cauer-Network topologie is preferred over the Foster model in this case. 
 Bi 0 Tj I=Id(M1)*V(D,S) +Ig(M1)*V(G,S) 
 The RC-ladder starts with node Tj and ends with node Tc. The heatsink will be connected to node Tc. 
 If you have a thermal RC-model, I will help you to make an example. 
 Helmut

helmuts · Answer

Hello attila2.toth 
 It's true that there is no pin for Tc and Tj. 
 One have to use "Add Traces" in the plot window. Then the dialog window with all items which can be potted will be shown. The interesting item is tc#m1 and tc#m1. See my screenshot below. There is one not documented feature about the parameter "Tambient". The default Tambient is 85&deg;C. You can change it with the procedure below. I recommend to make the SpiceLine visible in this case. 
 CTRL-right-mouse-click on the Mosfet A dialog window with all attributes will appear. SpiceLine: Tambient=50 OK 
 Helmut

2084.SOA-therm.zip

helmuts · Answer

Hello Attila, 
 I made a simple example witha RC-ladder. 
 Watch how good the externally calculated Tj match the internally calculated Tj. 
 Helmut

3487.SOA-therm-rc.zip

helmuts · Answer

Hello Attila, 
 > where did you find the C1 R2 C2 R3 parameters for the FET? 
 I simply tried to get a similar temperature rise as the LTspice-Model of M1. Basically one could say the left resistor is Rthjc and the sum of both resistors is RthjA. You can find a thermal model on the manufactures' web pages for some of their Mosfets. These models have four or more resistors and capacitors. 
 If you want model cooling with PCB-copper-area, you would replace R3 or at least part of it with a few R and C or with the PCB-model from LTspice. At the end of the RC-ladder you place the V-source with the ambient temperature. 
 Below is an example using the PCB-model from LTspice - symbol SOAtherm-PCB. 
 I recommend to check a selfmade thermal model with measured data or with published data. 
 Helmut 
 
 5672.SOA-therm-rc-pcb.zip

helmuts · Answer

Hello, 
 You cannot adjust the Mosfet model on the fly (during simulation), but you could add an external arbitrary resistor with a B-source in series to the drain. I have never done this in the past, but you could give it a try. 
 Example with a Bv-source: 
 V=Id(M1)*20m*((V(Tj1)-25)/50) 
 This function linearily increase Rdson by 20mOhm per 50&deg; Tj above 25&deg;. 
 See my uploaded example. 
 Helmut 
 
 6087.SOA-therm-rc-pcb-Rdson.zip