LMZ31520 and LMZ31530 TINA-TI simulation model

K. Sasaki14

Other Parts Discussed in Thread: LMZ31520, LMZ31530, TINA-TI

Could you give me the LMZ31520 and LMZ31530 TINA-TI simulation model?

Our customer requires this model for operation simulation of their system. On WEBENCH, we can't change transient condition, and it does not appear load rise up waveform in transient simulation. Therefor I think steady state waveform isn't the waveform in steady state condition because it is not stable.

Best Regards,

Kohei Sasaki

over 9 years ago

0 Nikhil Gupta (Product Folder Models) over 9 years ago

TI__Mastermind 39210 points

Hi Kohei,

We will add this to the TINA-TI translation queue and get back to you once it is completed. This will be enabled as a TINA-TI export from WEBENCH Power Designer.

Thanks,

0 Nikhil Gupta (Product Folder Models) over 9 years ago in reply to Nikhil Gupta (Product Folder Models)

TI__Mastermind 39210 points

Also, we are looking into the issue of the Input and Load not being changeable in WEBENCH. We will get back shortly regarding this.

Thanks,

0 Mahavir Jain over 9 years ago in reply to Nikhil Gupta (Product Folder Models)

TI__Intellectual 2405 points

Hello Sasaki San,

Could you please share your e-mail ID? I can send you Startup testbenches with TINA-TI Simulation model for LMZ31520 and LMZ31530.

Thanks!!

Best Regards,
Mahavir Jain.

0 K. Sasaki14 over 9 years ago in reply to Mahavir Jain

Guru 10200 points

Mahavir-san,

Thank you for contacting me. My E-mail address is the following.

sasaki-k@clv.macnica.co.jp

Best Regards,

Kohei Sasaki

0 Mahavir Jain over 9 years ago in reply to K. Sasaki14

TI__Intellectual 2405 points

Hello Sasaki-san,

Please find attached the testbenches for LMZ31520 and LMZ31530 Startup test cases in TINA-TI. Kindly let me know if you face any difficulty.

Thanks!!

Best Regards,

Mahavir Jain.

LMZ31520_Startup.tsc

LMZ31530_Startup.tsc

0 K. Sasaki14 over 9 years ago in reply to Mahavir Jain

Guru 10200 points

Mahavir-san,

I confirmed LMZ31520 simulation with TINA-TI. However I couldn't change Vout value. I changed VADJ resistor value to 2.2k to set output voltage 1.0V, however the simulation failed.

I would like to simulate the output ripple and transient response(4A to 16A, 1.2A/us slew rate and 2A to 8A, 0.6A/us slew rate) with Vin is 12V, Vout is 1V and Fsw is 500kHz condition.

Can you simulate with the above condition?

Best Regards,

Kohei Sasaki

0 Nikhil Gupta (Product Folder Models) over 9 years ago in reply to K. Sasaki14

TI__Mastermind 39210 points

Hello Kohei-san,

I simulated the circuit with Radj of 2.2K and it worked fine (I used a primitive resistor from TINA-TI, not the sub circuit type present in the original schematic.. Attached is the TSC file and the Startup result.

LMZ31520_Startup_1V.TSC

Thanks,

0 K. Sasaki14 over 9 years ago in reply to Nikhil Gupta (Product Folder Models)

Guru 10200 points

Nikhil-san,

Thank you for your support. I could simulation with your attached file. Could you check my simulation file? I attach it.

Best Regards,

Kohei Sasaki

LMZ31520_Startup_sasaki.TSC

0 Nikhil Gupta (Product Folder Models) over 9 years ago in reply to K. Sasaki14

TI__Mastermind 39210 points

Hello Sasaki-san,

The issue is with the output capacitor that you have used. I think you have mistaken the Rpar with the ESR of the capacitor. Actually Rpar is the parasitic resistance which is in parallel with the cap (default value is "Infinite"). I would leave it as is. To add an ESR, simply add resistance in series with the output capacitor. I tried it and it worked OK. I did have to increase the simulation time to 1.5ms to see the complete Soft Start.

Just FYI, in your schematic you should notice that before the simulation fails, Vout is very low. That is essentially due to the fact that you have shorted Vout to GND through Rpar = 2mohms.

Thanks,

0 K. Sasaki14 over 9 years ago in reply to Nikhil Gupta (Product Folder Models)

Guru 10200 points

Nikhil-san,

Thank you for your support!

I could simulate by following your teaching.

Best Regards,

Kohei Sasaki

0 Sneha Kumari over 8 years ago in reply to Mahavir Jain

Intellectual 300 points

Hi,

I was trying to simulate LMZ31530 using the model from LMZ31530_Startup.tsc, posted here. In that simulation, INH pin is not working.In my simulation Vout is always coming, irrespective of the state of INH pin. Could you please check and confirm? I would like to connect this pin to PGOOD of another regulator. Hope this is fine to do in this way.

Thank you.

regards,

Sneha

0 Mahavir Jain over 8 years ago in reply to Sneha Kumari

TI__Intellectual 2405 points

Hello Sneha,

Please find attached LMZ31520 and LMZ31530 testbenches with updated model. The INH pin functionality should work properly now. Yes, you can connect it to PGOOD signal of previous regulator to synchronize the devices. Kindly let me know know if you need further help.

4745.LMZ31530_Startup.tsc 2287.LMZ31520_Startup.tsc

Thanks!!

Best Regards,

Mahavir Jain.

0 Sneha Kumari over 8 years ago in reply to Mahavir Jain

Intellectual 300 points

Hi Mahavir,

Thank you very much. I tried the simulation with new model. INH function is working properly.

regards,

Sneha

0 Sneha Kumari over 8 years ago in reply to Sneha Kumari

Intellectual 300 points

Hi,

I need one more support for the LMZ31530 part. Now, I am doing the load transient simulation. This is done using load resistor and switches, in parallel. I am stuck with convergence error[component :U1.D_U2_U8_D3], U1 is the LMZ31530. Simulation will not get completed. Simulation parameters are TinaTI default. I didn't try any changes. Please let me know if you need any further information. Simulation file is attached for the reference.

Thank you very much.

regards,

Sneha

2553.LMZ31530_LoadTransient.TSC

0 Sneha Kumari over 8 years ago in reply to Sneha Kumari

Intellectual 300 points

Dear All,

Any help on this issue would be very much appreciated...

regards,

Sneha

0 Mahavir Jain over 8 years ago in reply to Sneha Kumari

TI__Intellectual 2405 points

Hello Sneha,

Please find attached your schematic that shows load transient test on the device for transient current of 1A. I am not very sure if that meets your application requirement. So below are few recommendations if you want to try it out with switch based arrangement.

1. Please define switch VON, VOFF, RON and ROFF values properly. A 1nV value for ON voltage and 0V value OFF voltage, 0ohm ON resistance, 1Gohm OFF resistance are extreme/non-practical values and will lead to convergence errors.

2. If you are using 12V input signal for switch, you can define switch ON voltage to the same level i.e. 12V.

3. Please use the recommended startup parameter settings for load transient test also. You can get them from startup testbench analysis parameters.

4. Carefully choose the soft start time and output capacitor values as that decide time available for the device to reach steady state condition.

Kindly let me know if you face any issues.

Thanks!!

Best Regards,

Mahavir Jain.

LMZ31530_LoadTrans.TSC

0 Sneha Kumari over 8 years ago in reply to Mahavir Jain

Intellectual 300 points

Hi Mahavir,

Thank you very much for the reply. I am really sorry that I didn’t notice the Von voltage of switch. I never used to change it. Now I could run the simulation successfully with changed switch voltage and analysis parameters(same used in startup testbench). I couldn’t use the current source as load. I used the same switch controlled resistance as load. But, it is taking long time to run the simulation.

Regarding point #1 and 2, I tried changing the values of switch

Regarding point #3, I used the same parameters from the example file

Regarding point #4, the soft start capacitor and output capacitors are the actual values used in schematic. Hope this is ok.

Regards,

Sneha

Simulation, hardware & system design tools

Simulation, hardware & system design tools forum

LMZ31520 and LMZ31530 TINA-TI simulation model