TINA/Spice/TPS54260: Dual supply TPS54260 Tina Ti

Tom Salm

Part Number: TPS54260
Other Parts Discussed in Thread: TINA-TI, , LM76003

Tool/software: TINA-TI or Spice Models

Hi,

I'm trying to simulate a dual power supply based on the TPS54260 in Tina-Ti but the simulation does not give the right results. When I try to do a DC analysis the error "operation point not found" pops up and the results of the transient analysis do not make any sense to me.

The schematic is based on the following design: http://www.ti.com/lit/an/slva369a/slva369a.pdf The circuit has been build before and is working but I can't get the simulation to match. Does anyone know what I do wrong?

over 6 years ago

0 Nikhil Gupta (Product Folder Models) over 6 years ago

TI__Mastermind 39210 points

Tom,

I would recommend starting with a Ramped up source for Vin. DC results will not give any interesting results for this model as all internal nodes will probably be at 0V at time t=0. Following the change to a Ramped input, please run a transient simulation to see the results. You can refer to the TINA-TI Transient Reference Design as a starting point for ease of use: www.ti.com/.../toolssoftware

0 Tom Salm over 6 years ago in reply to Nikhil Gupta (Product Folder Models)

Prodigy 80 points

Thank you for the quick response. I used the reference design as a base model and rebuild it to the current schematic. I now used the same generator as the reference design but the output is still 0 volts. The PH and PWRGD spike and than stay at 0 volts

0 Nikhil Gupta (Product Folder Models) over 6 years ago in reply to Tom Salm

TI__Mastermind 39210 points

Hi Tom,

Are you running a transient simulation? If so, can you send the TSC file. Otherwise, please try running the transient sims to a TSTOP depending on your Soft Start time.

0 Tom Salm over 6 years ago in reply to Nikhil Gupta (Product Folder Models)

Prodigy 80 points

Hi Nikhil,

I included the TSC file, hopefully are you able to analyse the problem in more detail

I already found out that the VIN wasn't set properly. I now have set it to unit step 48 volts

TPS54260.TSC

0 Nikhil Gupta (Product Folder Models) over 6 years ago in reply to Tom Salm

TI__Mastermind 39210 points

Hi Tom,
Sure, we will look into this and get back.

0 Imran Dharwad over 6 years ago in reply to Nikhil Gupta (Product Folder Models)

TI__Intellectual 1440 points

Hi Tom,

Currently the model doesnot support negative voltages(inverting topologies) as GND pin is internally grounded(0V).
Sorry for the inconvenience. We will revise the model and publish it to web in 2-3weeks.

0 Tom Salm over 6 years ago in reply to Imran Dharwad

Prodigy 80 points

Hi Imran,

That explains allot. I also did a simulation in PSpice and got the same problem there. The PH signal didn't go lower than -0.6 which I guess happens due to the diode voltage drop. I assume that the models of Tina-Ti and PSpice have the same internal ground.

Thank you anyway. I'm looking forward for the new model. Is it possible to get a notification when the model come online?

Tom

0 Nikhil Gupta (Product Folder Models) over 6 years ago in reply to Tom Salm

TI__Mastermind 39210 points

Hi Tom,

Some of the older device models have internal ground shorted to node 0, hence the model can not be used in inverting configuration (though this is not a device limitation). We are adding floating GND nodes to the newer models. I would request you to consider a newer device for your evaluation such as LM76003. This model supports the inverting configuration. Here is a comparison of LM76003 and TPS54260.

Alternately, you can find all models that support inverting configuration by clicking on the link in my signature file and typing "inverting" in the search box. If you do find a model that supports inverting configuration but is only available in PSpice, we will be happy to convert that to TINA-TI for you.

Simulation, hardware & system design tools

Simulation, hardware & system design tools forum

TINA/Spice/TPS54260: Dual supply TPS54260 Tina Ti