LM5146-Q1: Issue in pSPice simulation of LM5146-Q1

Prayag Sahoo

Part Number: LM5146-Q1
Other Parts Discussed in Thread: LM5146

Hi Team,

I am simulating the pSpice model of LM5146-q1 available on ti.com.

I have set the current limit using design calculation sheet available on the product page to 15A i.e R(ilim)= 681 ohm. (Rds(on sensing))

My output voltage is set at 14.5V and R(Load) = 0.6 ohm.

When simulating the current is not being limited to 15A. It is going upto 29A.

Please suggest here.

Thanks

over 2 years ago

0 Rahil Ajani over 2 years ago

TI__Genius 9460 points

Hi Prayag,

Please complete and review the quickstart calculator and send me the file with the schematic. Use Rdson at Vgs=7.5V from the MOSFET datasheet.

Regards,

Rahil

0 Prayag Sahoo over 2 years ago in reply to Rahil Ajani

TI__Expert 5225 points

Hi Rahil,

Uploaded the files here.

I have downloaded the pSpice model from https://www.ti.com/lit/zip/snvmbl1 and changed the R(L) to 0.6 ohm, changed the feedback resistor value to get 14.5 V and Rlim to 681 ohm to limit the current to 15.5A.

Also attached the schematic and simulation result I had done.

Thank You

7585.LM5146-Q1 Quickstart Tool r2 - 48Vin 12Vout 8A 400kHz.xlsm

LM5146-Q1_TRANS.DSN LM5146-Q1_TRANS.libhttps://e2e.ti.com/cfs-file/__key/communityserver-discussions-components-files/196/LM5146_2D00_Q1_5F00_TRANS.OPJhttps://e2e.ti.com/cfs-file/__key/communityserver-discussions-components-files/196/LM5146_2D00_Q1RGY_5F00_TRANS.OLB

0 Orlando Murray over 2 years ago in reply to Prayag Sahoo

TI__Mastermind 22301 points

Hi Prayag,

We recently found an issue with the low-side diode partially conducting and messing up the ISEN function.

Please try deleting the existing diode and placing an ideal diode or pspice dbreak to replace D19.

Place-> PSPICE Component -> Diode

Or try with resistor sensing.

Hope this helps,

-Orlando

0 Prayag Sahoo over 2 years ago in reply to Orlando Murray

TI__Expert 5225 points

Hi Orlando,

I tried by changing D19 with a dbreak but there was no change in the result.

0878.LM5146-Q1_TRANS.DSN 7802.LM5146-Q1_TRANS.libhttps://e2e.ti.com/cfs-file/__key/communityserver-discussions-components-files/196/4331.LM5146_2D00_Q1_5F00_TRANS.OPJhttps://e2e.ti.com/cfs-file/__key/communityserver-discussions-components-files/196/3326.LM5146_2D00_Q1RGY_5F00_TRANS.OLB

0 Orlando Murray over 2 years ago in reply to Prayag Sahoo

TI__Mastermind 22301 points

Prayag,

The RDSON of your MOSFET on PSPICE is 4mΩ, however in your quickstart calculator you had 10mΩ.

Please correct this discrepancy.

When I update the RON in pspice to 10mΩ, I get a current limit of ~15.5A.

-Orlando

0 Prayag Sahoo over 2 years ago in reply to Orlando Murray

TI__Expert 5225 points

Thank you for pointing it out.

I have changed the Rd(on) of Q2 to 10m Ohm and when the current reached 15.5A the device shutdown i.e Vout =0V and Iout =0A.

My understanding was only the current will be clamped to 15.5A. Please help me understand here better.

Thank You

0 Orlando Murray over 2 years ago in reply to Prayag Sahoo

TI__Mastermind 22301 points

Hi Prayag,

After 128 continuous cycles of current limit, you will trigger hiccup mode restart.

It should re-soft-start after 8192 clock cycles of being shutdown.

-Orlando

Power management

Power management forum

LM5146-Q1: Issue in pSPice simulation of LM5146-Q1