how to plot output with Temperature in hspice?

[triquent]

1)I simulate the bandgap reference circuit by several different temperature using .alter command. I want to know how to plot the Vout versus temperature?(DC simulate)
2)how to measure the total current for the bandgap circuit in hspice(my spec for the bandgap circuit is totoal current<10uA)?also if i changed the power supply Vdd and measure the total current. How can i plot Idd versus Vdd?

can anyone recommend a good book about hspice code writing?

thanks!

 

[simonkuo]

1) For plot the temperature VS. bandgap voltage, sweep the temperature to simulate in DC simulation then use the awave to plot. Use the temperature variable as the axis, then plot the bandgap output voltage.
2) For total current comsume, try to plot the bandgap power supply current say I(VDD).

 

[leo_o2]

You can do DC sweep for temperature.
.DC temp -40 100 10

 

[shiowjyh]

Hello,

For dc analysis,
Both simonkuo and leo_o2 are right.

How can i plot Idd versus Vdd? :shii:

Well, since you have I(vdd) and vdd,
just put one of those on your x-axis and you can get it... (using awaves)

The hspice manual presents many good writing methods, please read it over..
For further advanced, there are lots on opening internet, please use searching engine to help you out.

You have to investigate the transient analysis either....

Regards,

 

[triquent]

Then how to plot vout versus vdd(power supply)?
I tried
.dc vdd 2 3 0.1
.probe v(out)
but doesn't work.

 

[muldersun]

Then how to plot vout versus vdd(power supply)?
I tried
.dc vdd 2 3 0.1
.probe v(out)
but doesn't work.

If you define

v1 vdd gnd 2
.dc v1 2 3 0.1
.probe v(out)

 

[leo_o2]

I think you should sweep the variable instead of the voltage source.
(1) Define a variable
(2) Do sweep

 

[Hughes]

Then how to plot vout versus vdd(power supply)?
I tried
.dc vdd 2 3 0.1
.probe v(out)
but doesn't work.

If you define

v1 vdd gnd 2
.dc v1 2 3 0.1
.probe v(out)

muldersun is correct. Furthermore, if you define:
V1 vdd gnd vdd
.param vdd=3

The dc-sweep statement also should be:
.dc v1 2 3 0.1

But if you define:
V1 vdd gnd pvdd
.param pvdd=3
The dc-sweep statement can be
.dc v1 2 3 0.1
or
.dc pvdd 2 3 0.1

If the sweep variable begins with letter 'v' or 'i', hspice treats it as voltage source name or current source name.