# Setting manual thermal voltage for a diode in LTSPICE

I want to simulate some series and parallel connected solar cells with the same reference temperature but different operation temperature for each cell. To do so, I need to configure the thermal voltage of the diodes which I use in my circuit.

The problem is that it is not possible to change the operating temperature (.Temp) for each element of the circuit. Therefore, I want to calculate the diode properties manually. For the diode model, I do not know how can I specify the thermal voltage manually and I need your help.

Vt=kT/q is the thermal voltage that I want to configure it to a specific value.

You can set the temperature for each component individually using the following approach:

After placing your component and selecting the correct model for it, do a CTRL+Rightclick on the component. In the newly opened window, search for the "SpiceLine" field and enter temp=500 (or whatever value).

Now your diode will have that temperature where the rest of your circuit does not.

Example:

In the LT-Spice netlist the line for the diode is displayed like this:

D2 N002 0 1N914 temp=500


With following result:

• Thank you very much! It works perfectly correct! One more question: how can I add temp=500 to diode if I want to use it as netlist (I do not use schematic). I tried to export the schematic as a netlist but it just gave me no information! P.S. Since I have less than 15 reputations, I cannot vote for you but please accept my thanks in comment. – HAMED Nov 12 '15 at 12:31
• @HAMED I've included the netlist line for the diode with the changed temperature. I got this via: "View" -> "SPICE Netlist". I haven't tried if it works if you input the netlist by hand, but I guess it will. – Arsenal Nov 12 '15 at 13:00
• Thank you very much. I was using export netlist which gave me incorrect data. Now it works and I know what to do. Many thanks again – HAMED Nov 12 '15 at 13:02