How to use the post-processor with tina?

Xiaoguang,

Are you trying to plot the average value of a single waveform waveform in the post processor? I do not believe that you can plot the average value of a waveform in the plotter. However, if you are simply looking for the average value of a waveform, click on the waveform in question and it will be highlighted Red:

Then click on the Process menu item and select Averages...

The window with the average values will be displayed:

Let me know if this is not what you were looking for.

Britt

Xiaoguang,

        Like Britt mentioned above, I don't think there is a way to plot the AVG and RMS value using the post processing tool. However if you need to see the AVG and RMS plots you can calculate those values on the fly using voltage controlled voltage sources, e.g.

say you need to calculate the AVG and RMS value of a voltage at a node called TEST,

AVG = 1/T * integral( TESTdt ) in tina this will translate to 1/(TIME + correction factor) * SDT(V(TEST))

* the correction factor avoids the 1/0 division when TIME = 0 i.e. simulation starts.

Similarly

RMS =  SQRT(1/(TIME + correction factor) * SDT(POW(V(TEST),2)))

I have attached an schematic containing both sources. The simulation results are given below,

Regards,
Marcos

Hello Marcos,

do you know how to extend your AVG & RMS calculations to plot "sliding" values?
(I want to output the actual AVG & RMS values for a given integration time).

I've something like that for LtSpice but don't know how to transfer it to TINA:
V=sqrt(idt(V(x)*V(x)-delay(V(x)*V(x),{ti}),V(x)*V(x)*{ti})/{ti})
"{ti}" is my integration time parameter and "x" is the input voltage

Do you know where can I get some documentation about the available build-in functions (SDT, DELAY, ...) for TINA?

Best regards,

Florian

Florian,

        I think the equation you wrote in your post will look something like this in TINA/PSPICE

.SUBCKT Sliding_surface x Vout

+ PARAMS: ti = 1n

E1     Vout  0  VALUE = {SQRT((SDT(V(x)*V(x) -  V(x)*V(x)*STP(TIME - ti)) +  V(x)*V(x)*ti)/ti)}

.ENDS

There is a "delay" in TINA called STP but I don't know if this might be what you are looking for.

To get more info on any of the built in functions you can go to the help menu in TINA or

alternatively just look up the pspice reference guide online and search for SDT, that will take you directly

to the function table.

Take a look at page 124 of:   http://www.coe.montana.edu/ee/andyo/EE503/pspug.pdf

I hope this helps. Feel free to repost if you have any further questions.

Regards,

-Marcos

Hello Marcos,

thank you for your answer.

As far as I can see the STP function of TINA is a switch- and not a delay-function.
If I put the expression "V(N1)*STP(TIME-1m)" to a controlled source, I will get 0 output if TIME < 1ms and V(N1) for the rest of the time.

P.S.:
In the help files of TINA I've nothing found about the build-in functions like SDT etc.

P.P.S.:
Normally I'm doing my simulations with Altium Designer or LTSpice.
Because some of the simulation models from TI are encrypted (like the UCC28950), I'm forced to use TI-TINA as a 3rd tool.
I don't have the money to buy PSpice as an additional imulation tool.
And in general I'm not very happy with TI-TINA (indepent of the discussed problem).

P.P.P.S.:
Is there a chance to get unencrypted spice models from TI (UCC29850 in the first step) so I can do the simulation with my prefered toolchain?

Regards, Florian

Florian,

We cannot provide an unencrypted version of the UCC28950 model without an NDA at this time.

Britt

Hi Florian,

        Yeah as you mentioned the STP is just a unit step. I think the only way you can implement the function you are after will be at the circuit level.

All the sqrt, sdt and arithmetic operations can be implemented using behavioral components ( the E source Value = {} combo) and the delay

can be implemented using a transmission line or T element in SPICE/TINA. Mixing behavioral and structural might open up more options that

can help you implement functions that are beyond the  native set of functions.

Regards,
-Marcos

Hi Marcos,

Thank you for your suggestion above, to generate RMS and average traces.  I am running into something a bit strange and have not spotted the difference yet: when I run your example circuit there are no errors or warnings.  When I run a copy of the averaging module inside my circuit a warning "Pin 0(V) of Controlled source wizard CS1 is not connected".  There does not seem to be an unconnected node but the warning is worrying me a bit.  Any thoughts why I would see it in my circuit but not yours?