TINA/Spice/UCC2801: switch modeling in TINA-TI?

user716692

Part Number: UCC2801
Other Parts Discussed in Thread: TINA-TI,

Tool/software: TINA-TI or Spice Models

About the UCCx813-1 model issue I have the following questions.

In the sub-circuit below (inside the unprotected model for UCCx813-1) VON and VOFF have been defined two times. What will be the final VON and VOFF?

Also VT and VH seems to be non-standard VSWITCH parameters. What are their functions? Do they work as Threshold and Hysteresis? What are the VT and VH formulae in TINA?

**********************************************************************************************

XUV VCC uvlout UVLOX2 PARAMS: VON=9.4 VOFF=7.4 ; UVLO Setting
.SUBCKT UVLOX2 1 2 PARAMS: VON=4.1 VOFF=3.6
* VIN OUT
S1 1 3 1 0 SUVLO
RUV 3 0 100K
EB1 4 0 Value= { IF ( V(3) > 3V , V(1) , 0 ) }
RD 4 2 100
CD 2 0 100P
.MODEL SUVLO VSWITCH RON=1 ROFF=1E6 VT={((VON-VOFF)/2) + VOFF} VH={(VON-VOFF)/2}
.ENDS

****************************************************************************************************************************************

over 7 years ago

0 Nikhil Gupta (Product Folder Models) over 7 years ago

TI__Mastermind 39210 points

Hi,

Yes this is a standard hysteretic switch (acts as a schmitt trigger with turn on at VT+VH and turn off at VT-VH). It takes 4 parameters - Ron, Roff, Vt and Vh. Refer to this document page 161. There are also many other resources available on google that show the working of this switch.

This is different from an exponential switch which does not have a sudden turn on. In this case the turn on/off is exponential in nature. This switch also takes 4 parameters but 2 of them are different from the schmitt trigger above) - Ron, Roff, Von, Voff. You can find the equations for this switch in this document on page 221.

In this particular case, VON and VOFF are just the parameters used to pass to the subcircuit. They are not the Von and Voff parameters that the exponential switch takes. The switch SUVLO depicted there is a hysteretic switch as described above. It is used for UVLO detection. Turn ON and Turn OFF points are defined by the value passed to the VON and VOFF parameters respectively (9.4V and 7.4V respectively in this case).

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

I have the same PSPICE document but didn't find the definition for VT and VH in VSWITCH section. I did see VT and VH in LTSPICE. I created a PSPICE simulation to illustrate my findings. VT ad VH were ignored.

By the ways, when I clicked on the pdf files above the web pages locked up my computer.

David

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

Hi David,

The PDF files are opening up fine for me in Firefox. Can you try a different browser. I will add them again below just in case (they are just links).

Regarding the schmitt trigger switch, we have been using this without any issue in PSpice for many years. It is a fairly standard device though not used as much as the smooth switch with the exponential behavior. In any case, make sure that you are using the right component in PSpice for the hysteretic switch (S_ST, available in the ANALOG library in PSpice, as opposed to the standard S component).

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

Hi Nikhil,

I tried the S_ST and it behaves the same as the one in LTSPICE.

I didn't see the definition or details in S_ST in the ReferenceGuideORCAD or the UserGuide documents.

Can you tell me where you can find the VT and VH definition? I want to compare it with that from LTSPICE.

Thanks.

David

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

Hi David,

I am not able to find the specific documentation from PSpice/Orcad. You might be able to get something by posting on their forum: http://www.pspice.com/forum.

The working should be identical to the one I had provided in the documents above. You can also simulate it to check the thresholds at which the switch turns on and off and check the resistance by connecting a 1V source across the switch and measuring the current through it.

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

Hi Nikhil,

I have created a PSPICE and a LTSPICE simulations on S_ST (PSPICE) and SW (LTSPICE). It seems that there are differences between the two.

Please note that the second trip point for PSPICE is 9V versus that for LTSPICE is 10V.

So what is the equation for VT and VH for PSPICE?

The one for LTSPICE is VT= {((VON-VOFF)/2) + VOFF} VH = {(VON-VOFF)/2}

PSPICE

LTSPICE

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

Hi David,

Your images did not come through.

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

Hi Nikhil,

I have created a PSPICE and a LTSPICE simulations on S_ST (PSPICE) and SW (LTSPICE). It seems that there are differences between the two.

Please note that the second trip point for PSPICE is 9V versus that for LTSPICE is 10V.

So what is the equation for VT and VH for PSPICE?

The one for LTSPICE is VT= {((VON-VOFF)/2) + VOFF} VH = {(VON-VOFF)/2}

PSPICE

LTSPICE

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

Hi David,

I made this simple circuit in PSpice. Hopefully this will explain the behavior in PSpice. The trip points are VT+VH and VT-VH as you can see below.

If you need any specific documentation about PSpice, please post the question on the PSpice forum.

As far as attaching on the E2E forum, please follow these FAQs if you have issues:

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

Hi Nikhil,

I tried your circuit in PSPICE and it worked but it didn't work with a sine wave source, e.g. VSINE with VOFF = 0, VAMPL = 12, FREQ = 1K, AC = 0. You will see the second trip point is at 9V instead of 10V.

David

0 user716692 over 7 years ago in reply to user716692

Intellectual 405 points

VSWITCH_vs_SW.docx

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

Hi David

I am not sure what thresholds you are using, but it works for me with the previous thresholds.

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

TI__Mastermind 39210 points

You might be having an issue with accuracy. Since your input is 12V, it may not be tripping the circuit at Vt+Vh = 12V due to rounding error in the simulator (the simulator in the back end will convert the voltage into a floating point number with many digits of precision, it is never advisable to evaluate Voltage == 12V in a simulator for that reason, we should use voltage > 12V or voltage < 12V instead).

Please change the input amplitude to 12.1V and see if that resolves your issue.

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

I changed the VIN to 13V. The second trip point is still at 9V. I attached a word file for that.

VSWITCH_vs_SW_A.docx

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

David,

It is still working for me. I do not see any issues. Are you sure there is nothing else interfering with your circuit like nets connected by name, etc. Have you reached out to the PSpice forum for assistance regarding the PSpice issue?

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

That is strange. Anyway, I think I should focus on the UCx813-1 unprotected model. Did anyone try it in PSPICE or TINA?

David

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

UCx813-1 model has been released a long time back and there have been many people who have used both the PSpice and TINA-TI model.

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

I replaced the protected model with the unprotected one in the PSPICE example file I downloaded from TI. It didn't converge successfully. That is why I ask whether the model has been tested or not.

Can you email me an example with the unprotected model? Thanks.

David

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

David,

Regarding UCC2801, I simply replaced the encrypted model with the unencrypted model (both available on the web) and it ran out of the box without any issues. I am using PSpice 17.2. The model is attached below along with the results.

I am suspecting there is something wrong with your setup as even the basic hysteretic switch is not working for you. It might be worthwhile to get that resolved with Cadence first before evaluating more complex circuits.

UCCx813-1_PSPICE_TRANS.zip

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

Hi Nikhil,

Thanks for your investigation. I fixed my PSPICE problems (configuration and .lib) already and got the same results as yours. Unfortunately, the same unprotected library (with VSWITCH replaced by SW) didn't work as good in LTSPICE. The V(Gate) has a break in the startup waveform as shown in the attached file. I still thin there are some differences between SWITCH definition in PSPICE and LTSPICE.

UCCx813-1 Boost converter testing.docx

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

David,

That looks to me like a classic time step issue. I don't think it is coming from the switch since it is working fine some of the times. Please see below. This issue exists in many simulators - there is a tradeoff between speed and accuracy. If you use a smaller time step, this issue can go away.

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

I tried your max time step at 10ns and 4ns, and the results are the same.

UCCx813-1 Boost converter testing_1.docx

0 Nikhil Gupta (Product Folder Models) over 7 years ago in reply to user716692

TI__Mastermind 39210 points

Hi David,
I do not have any more suggestions to make it work in your simulator. Since the model is open (unencrypted), you are free to post it in your target simulators forum to get further help.

The faster alternative in my opinion is what I had originally suggested i.e. to try this in TINA-TI or PSpice. The model has already been setup in these simulators for you.

0 user716692 over 7 years ago in reply to Nikhil Gupta (Product Folder Models)

Intellectual 405 points

Thank you very much for your help. I will let you know how I fix it.

David

Simulation, hardware & system design tools

Simulation, hardware & system design tools forum

TINA/Spice/UCC2801: switch modeling in TINA-TI?