How can I probe the temp value in tran simulation ?

See plotting-temperature-w-r-t-time-while-changing-temperature-using-dynamic-parameter-in-transient-analysis

Thanks, 

According to the thread, I got about way to draw the temperature value:

(1) I set via Outputs->Save All, and then on the "Save by Subckt" tab, enter "temp" in the Instance column 

(2) I set "temp" node on my circuit bc I couldn't find "temp" in VIVA-XL browser mode...

(3) I was able to draw the "temp" plot with reference to the time by probing the "temp" node.

Ichiro

My memorandum

Then I used "additionalParams" in Misc(tran-->option) tab instead of "Dynamic param" by GUI because "param_step" was required.
param=temp param_vec=[0n 20 50n 25] param_step=10n

Dear ichiro,

ichiro said:

(1) I set via Outputs->Save All, and then on the "Save by Subckt" tab, enter "temp" in the Instance column 

(2) I set "temp" node on my circuit bc I couldn't find "temp" in VIVA-XL browser mode...

I am not sure if you happen to read the Cadence On-line support article at URL:

Article (11539376) Title: Plotting temperature when it is changed as a dynamic transient parameter
URL: https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000000nb0ZEAQ

However, it recommends adding an unconnected wire to your top level schematic and name the wire "temp" (see Figure 1). It could also be called any other defined parameter if you wanted to plot its dynamic value. Add the wire "temp" as an output in the simulation as shown, for example, in Figure 2.This will have the effect of adding the following line to your input.scs file. In the test case I assembled using Explorer, which varies the temperature dynamically and probes the current through a load resistor that has a set of finite temperature coefficients, the input.scs save line appears as follows:

save vbias irload:in vload vssa temp 

and has the same impact of including an external simulation file with the "save temp" as its only line. Performing the simulation and opening the Results Browser reveals the transient outputs shown in Figure 3 where I also plotted the "temp" output as a function of time.

I hope this helps ichiro,

Shawn

Figure 1

Figure 2

Figure 3

Hi Shawn,

I got simply way to draw temp wave form that is:

(1) add "temp" node line on my schematic

(2) save the "temp" line(voltage), this automatically add "save temp" description without "output menu--> save all..-->save by subckt-->append "temp" "

(3) plot the temp node (just like a normal node voltage)

Thanks

And probably.. I am able to plot other parameter by above procedure..?

Thanks,

Ichiro 

Hi Shawn,

I got simply way to draw temp wave form that is:

(1) add "temp" node line on my schematic

(2) save the "temp" line(voltage), this automatically add "save temp" description without "output menu--> save all..-->save by subckt-->append "temp" "

(3) plot the temp node (just like a normal node voltage)

Thanks

And probably.. I am able to plot other parameter by above procedure..?

Thanks,

Ichiro 

The dummy temp node on the schematic is just a convenience so that you can either save it or plot it. It turns out that because of changes in the Save by Subckt option, you can't just put "temp" in the instance column any more (because tries to save temp.* if you do that). You could put a dummy instance name in the Instance box and then temp in the User Options field on the form, but that's horribly clunky (and you'd have to plot by using the results browser that way).

So adding the dummy node on the schematic (which would work for any parameter used in dynamic parameters too) is a better solution. Nothing gets netlisted for that node (because it's not connected to anything), and probing it results in a save statement (note that this will only work if you've got save=selected rather than save=allpub).

Or you could use the approach of an external file included with:

save temp

Andrew.