Why is Xyce rewriting the second column of the csv during temperature stepping?

[pablo_sole...@brown.edu]

Circuit DRAFT 3

******Analysis Command********

.STEP TEMP 25 35 5

.tran 1n 350n ;Length of simulation

.print tran format=csv PRECISION=5 WIDTH=5  v(9)

I want to measure the period of V(9) with respect the temperature so I want to run a parameter step. However, the output csv only has two columns, the first being the index and the second being V(9).  How do I get it to not rewrite the column and print all the output  columns? Am I writing something incorrectly in the analysis command?

Another question..As long as I specify this step in the parameter sweep or the line ".options device TEMP={}" all the temperature dependent devices in the circuit use this temperature right?

[ngw]

To save you waiting:

• TEMP is a universal parameter;
• .STEP TEMP will over-ride .OPTION DEVICE TEMP;
• .TRAN TEMP LIST is limited to transient analysis;
• and you need to request TEMP; i.e., .PRINT TRAN FORMAT=CSV PRECISION=5 WIDTH=5  V(9) TEMP

Please consult the Reference Guide.

[xyce-users]

If you are using format=csv, then it doesn't put anything in the input file to indicate the transition from one .STEP iteration to the next.  (or in your case, from one temperature to the next).  It will appear as one giant column of data that includes all the temperatures.

If you try to plot your v(9), assuming Xyce didn't crash during any of the .STEPs, then you should see the line wrap around from the end of the transient to the beginning 2x, given that your .STEP command will result in 3 different temperatures.

If you want a file format that puts some kind of separator between each temperature, file formats that will do this include "format=tecplot", "format=probe" and "format=gnuplot".   The last one is the simplest and will put 2 blank lines in between each .STEP output.   tecplot and probe are a little more complicated and include metadata showing the temperature value.

If you want to double-check that all the temperatures you wanted were actually simulated, see the *.res file output, which is always produced with .STEP.

Hope this helps.

thanks,

the Xyce team

[xyce-users]

One more comment, in response to your second question:  "all the temperature dependent devices in the circuit use this temperature right?"

Yes, if you set temperature this way it will apply to all the devices in the circuit.  However, not all device models have a temperature dependence, and not all the ones that do have a temperature dependence have a great model of that dependence. 

Most semiconductor devices have  temperature dependence in them.  For example, all semiconductor models have diode equations in them, which all have a qV/kT term inside the exponential.  So, at a minimum there will be that dependency.  But that by itself is often not enough to adequately model temperature and there are additional temperature-based equations. 

Some models (such as most modern BJT models) include self-heating, which is another complication.

For  models which have a more complex temperature dependence there are usually additional model parameters you have to calibrate and set.

thanks,

The Xyce Team