I downloaded Pspice models of ttc004 and tta004 from Toshiba documentation.
In these Pspice models, there is TNOM=25.
How should I deal with it since TNOM=27 is the default value in LTspice.
I removed the TNOM=25 from the models when i added those in the LTspice set of BJTs. Is this the right fix ?
In these Pspice models, there is TNOM=25.
How should I deal with it since TNOM=27 is the default value in LTspice.
I removed the TNOM=25 from the models when i added those in the LTspice set of BJTs. Is this the right fix ?
Presumably TNOM specifies the junction temperature at which the model parameters apply. For any other temperature the simulator has to correct the parameters for the temperature difference.
Do you get error messages when you don't remove it? 27 degrees Celsius is also the usual default in PSpice (and in many other simulators).
In any case, a temperature difference of two degrees Celsius is too small to worry about for most applications, so removing the statement seems like a good workaround.
Do you get error messages when you don't remove it? 27 degrees Celsius is also the usual default in PSpice (and in many other simulators).
In any case, a temperature difference of two degrees Celsius is too small to worry about for most applications, so removing the statement seems like a good workaround.
Last edited:
I know this is an old thread but... Are the TTC004/TTA004 models that you have unencrypted?
I ask since I downloaded the TTC004B/TTA004B models (which are encrypted) and LTSPICE does not seem to recognize them.
Can you post the TTC004/TTA004 models that you used that work in LTSPICE?
Late, but if you use MicroCap V12, it works like this. Get rid of TNOM, delete the devices, and re-add them with the edited spice libs, using the component editor. You can change DC analysis temperature to 25 if you want, but 25 or 27 will make less difference than the spice parameter tolerance. Drop the devices into your schematic and double click them to see the model parameters. Notice it has added several parameters starting T_ and they are all set to "undefined". When you run the simulation, it fills in those T_fields with the simulation temperature at that moment. As that temp is changed in the simulation, it will change that parameter on the fly. If you want to fix the temperature of one of these components, then in your simulation, double click it and change T_ABS to whatever temperature (in deg C) you want to fix it at. I think that is what you are wanting to do. For instance, if you are are doing a DC analysis of bias current in an audio amp, you can, as a first approximation, fix all the signal level components at around 30degC, and leave the bias transistor, drivers and output devices with T_ABS "undefined". What I then did was a "Dynamic DC" analysis at 27 or 30degC, and set the bias current to your desired value. Then do a "DC" analysis ramping the temperature 100,0,5 in MC12 parlance, ie 0 to 100degC in 5 deg steps, and plot the bias current. You could also plot the total bias volts (around 1.3V, between the two driver bases for CFM). That can give you a good idea of where your bias circuit was going wrong if it soars of to amps or dies to zero. It's not long since I discovered this. I had been greatly doubting the results I was getting and had this niggling feeling that it was just wrong to let every active device go through the whole temperature range when they usually sit at nominal case temperature which changes maybe 10 degrees. I eventually found T_ABS. If you set T_ABS to, say 30C, it will stay there through the whole analysis, and the MicroCap help on it and other T_xxx parameters was very useful. For instance, you can step the temp of one device through a range, and have another device follow it 20 degrees behind it, or 30 degrees in front or whatever. NOTE - when you change any model parameter in a microcap schematic, it copies the model into your local schematic text info and modifies that, so it is volatile outside that schematic. It also applies to all devices of that type in your schematic.
You may want to try simulating a cheap long thin amplifier commonly discussed and simulate it's bias setup, with and without fixing the lower transistor temperatures. A real eye opener. I have used many simulators over the decades, including some of the research that turned into SPICE as we know it and I can recommend MicroCap V12 over anything else I have used. The fact that the author developed it for 40 years and then made his life's work free to the community I applaud. We now have a first class simulator at schematic level, with excellent documentation, completely free. Get it while you can, I can't imaging the web site will stay open for ever. If you are still about mchambin, how did you get on with the TT004's ?. They look good, but like most things, there no stock almost anywhere. Only Arrow have them, and they wan't business tax numbers etc.
If you think you have an adequate bias circuit, please try the above procedure. It scared me, but I've now got a (simulated) bias arrangement which is a nice gentle bath tube, with a range of 34mA +/- 5mA over a 0 to 100degC range. I can't test those values in real life, and it's a tedious difficult job measuring bias current over temperature anyway, but it looks like it follows the simulation fairly well.
You may want to try simulating a cheap long thin amplifier commonly discussed and simulate it's bias setup, with and without fixing the lower transistor temperatures. A real eye opener. I have used many simulators over the decades, including some of the research that turned into SPICE as we know it and I can recommend MicroCap V12 over anything else I have used. The fact that the author developed it for 40 years and then made his life's work free to the community I applaud. We now have a first class simulator at schematic level, with excellent documentation, completely free. Get it while you can, I can't imaging the web site will stay open for ever. If you are still about mchambin, how did you get on with the TT004's ?. They look good, but like most things, there no stock almost anywhere. Only Arrow have them, and they wan't business tax numbers etc.
If you think you have an adequate bias circuit, please try the above procedure. It scared me, but I've now got a (simulated) bias arrangement which is a nice gentle bath tube, with a range of 34mA +/- 5mA over a 0 to 100degC range. I can't test those values in real life, and it's a tedious difficult job measuring bias current over temperature anyway, but it looks like it follows the simulation fairly well.