Bode Plot of TPS51200

Thu,

As Nikhil said, you are trying to run the AC analysis on a transient model. Please download the TPS51200 Average PSPICE model from the product folder and hit run. The simulation profile is already configured.

When you open the file, you should have the following schematic:

1425.TPS51200 AC.pdf

Dear Nikhil and Ranjanir,

Thank you for your support. However, I am not clear the following points and would like to get your advice about them:

1. Why are 10H inductor and 10F capacitors included between VOSNS and VO pins?

2. The gain and phase there are of  VTT/VOSNS. Is that the gain and phase of the compensation loop?

3. How can we get the initial value of capacitors ?

Thank you very much for your help.

Best regards,

Thu

Hi all,

Is there anyone help me these problems? Please!!! I really need it.

Thu Duong said:

Dear Nikhil and Ranjanir,

Thank you for your support. However, I am not clear the following points and would like to get your advice about them:

1. Why are 10H inductor and 10F capacitors included between VOSNS and VO pins?

2. The gain and phase there are of  VTT/VOSNS. Is that the gain and phase of the compensation loop?

3. How can we get the initial value of capacitors ?

Thank you very much for your help.

Best regards,

Thu

Hi Thu

1. The model is used  to simulate the open loop AC response of the TPS51200 model along with the components from the EVM schematic. By adding the high capacitance and inductance between the feedback and the sensing nodes, you are making sure to not pass any DC information and only the small signal changes.

If you want to simulate the closed loop gain, simply remove the LC components and connect the sinusoidal signal between VOSNS and VTT.

2.  The gain is output/input signal, so the gain in decibels is gain of VTT/VOSNS pins.

3. The IC values of capacitors for VTT capacitors should be set to the value intended by the feedback resistors and the values in VREF should be set as VTT*2 as this is the input from which VTT is designed. Not all average models need us to set the IC values, but this particular model needs the initial condidtions set to remove convergence issues in simulation.

Thanks

Ranjani

hello,

1. to simulate the loop gain, how can I get the result?

2. Would you please explain the detail of using cap and inductor? As I know, Cap is used to block the DC signal, but why inductor is used.

Thanks for your help.

Thu

Hi Thu,

1. To simulate the Bode plot, open the PSPICE schematic and click on PSPICE --> Run or hit the F11 key to run the simulation directly. The simulation has been set up already for you and should run directly out of the box.

2. The LC filter that you see is used to inject the AC signal into the loop. When the simulator calculates the loop response (AC simulation), it needs to first calculate the closed loop DC bias point (which is does automatically before running the AC simulation). This is required to linearize the non linear elements in the circuit. For the DC bias point calculation, the inductor is a short and the capacitor is open, so the circuit effectively reduces to the original circuit. For AC analysis, the inductor is open and the capacitor is short so this effectively breaks the loop and the AC signal is injected through the "shorted" capacitor.

Let me know if you need further clarification.

Best regards,

Nikhil Gupta

Hi Nikhil,

Thank you very much for your information. It helps me a lot.

Concerning to ICs for power Management we will used, could you please show me how can I get the Average model of TPS51128, TPS51124, TPS74701.

Thanks and Best Regards,

Thu

Hi Thu,

Average models are only required for switching converters since the simulator can not find a steady state point (because of the switching activity). For a Linear Regulator which does not have any switching elements, you can use the same model for both transient and AC (Bode Plot) Analysis. Since TPS74701 is a LDO, you can use the model in the product folder for Bode Plots (http://focus.ti.com/docs/prod/folders/print/tps74701.html#toolssoftware).

For TPS51124, we do not have an Average Model as of now, but you can request the model through the following page: http://www-k.ext.ti.com/sc/technical-support/email-tech-support.asp?AAP. For more information about requesting new models that are not available on the web, please refer to the following post: http://e2e.ti.com/support/development_tools/analog_elab_and_tools/f/234/t/36943.aspx.

I do not see part number TPS51128 in the list of parts that TI has. Can you please verify the part that you are using?

Please let me know if you have any questions.

Best regards,

Nikhil Gupta

Dear Nikhil,

Happy New Year!

Thank you very much for your information. The part number I wanted is TPS51218. 

I did request the average models in the website you showed me but still have not received the reply yet.

Thanks and best regards,

Thu

Hi Thu,

Currently we only have the Transient model for TPS51218 and do not have an average model. Please use the transient model to verify the functionality for this part in time domain.

Best regards,

Nikhil

Thank  you very much for your support.

Best regards,

Thu