ericsson.sunshine?wrote:
? ?"Is it possible to plot the curve similiar to the datasheet ?"
Yes.
Sorry, after a few false starts ... I uploaded the file "20160801_log amp (TI) log112_DC.zip" to the Temp folder.
Run the simulation in that file.? Then after the simulation finishes, click in the plot window to select it, then go to Plot Settings -> Open Plot Settings File, and open the .PLT file again.? This should re-scale the axes so that the plot looks similar to the curve in the datasheet.? The difference is that the log amp runs out of positive range when the input current is too large.
? ?"And says the log amp is utilized to measure the physical quantities which has exponential characteristic (varies large.)
? ? I don't know how to show this characteristic in the waveplot of LTspice."
The plot shows it.? The log amp is able to handle input signals over a 5 to 8 decade range of values, or more, which is significant.
Stay away from negative values of input current.? Also avoid very small input values (less than about 100pA).? Either of those can cause the output of the log amp to deviate significantly from a log() response.
Also, the current Iref through the external resistor seems to no longer be 100uA when the input current is much out of range, and this can also mess up the plot. ?(This might be a problem in the SPICE model?? Or maybe not.)
? ?"The equation's simple to understand, but it's hard to plot the curve of "Vout vs. I1/I2". I don't why"
It works for a .DC sweep.? It doesn't work if the input current is not within the range where the log amp follows a log() curve.
I think the reasons it didn't work well in a .TRAN simulation, are (1) the input current went outside the range where the log amp fits the equation, (2) the log amp's response time gets to be ridiculously slow (even a 10 second ramp might be too fast), and (3) there might be some oscillation (instability) going on.
Andy
