WEBENCH® Tools/LM5022: How to use LM5022 transient PSPICE model in circuit with VIN referenced to system ground (SPICE node 0)?

Hi David,

Thank  you for posting.  You may not able to do it because GND in Pspice is a global node, namely its internal circuits all reference to 0V.  So in your simulation, you need level shift the circuit relative to the IC GND, namely add  the absolute VIN voltage as a dc bias to all circuit node (external circuit).  Now, your Vout is actual VOUT + |Vin|.  So your results should be the simulated voltage minus |Vin|.

Thanks,

Youhao Xi, Applications Engineering

Hi Youhao Xi,

Thank you for the quick response.

I don't really understand this solution and the reason may be because I did not fully describe my problem. The circuit attached to my query is a small part of a larger sub-system that I wish to simulate as a combined entity. The combined circuit is actually quite simple in concept but given the limitation of the SPICE models I cannot see how to organize the simulation. The combined circuit includes a positive and a negative voltage, VIN+ and VIN-, with respect to a common node, which I have been calling ground. A pair of buck regulators generate a reduced positive and a reduced negative output voltage VOUT+ and VOUT-, again with respect the same common node that I have called ground. The illustrated circuit is the negative buck regulator. The positive buck regulator will be conventional.

I would like to reference the positive buck regulator GND node to ground in the usual way, while referencing the negative buck regulator's input to ground, as this is the actual circuit topology. However, the SPICE model of the LM5022 does not support this as it turns out. Of course I could simply rename the nodes, as perhaps you are suggesting, so that VIN- becomes ground, my mid-point ground becomes VIN+ and VIN+ becomes VIN++. This will of course solve the problem with respect to the LM5022 used as a negative buck regulator. However, the problem will then be shifted to whichever positive buck regulator I select as the SPICE model will presumably again fail to support connecting its GND node to any node other than the ground node to which I have connected the LM5022 ground. Therefore, I still don't see how to configure the two buck regulators such that I am simulating the real-life conditions while accepting the SPICE model limitation.

Regards,

David Drori, Novarex Technological Enterprises

Hi David,

If you have a larger system which you want to simulate, I am afraid I don't have the solution.  To make it work, the entire LM5022 model should be changed, referencing to a floating ground which you can set to any circuit node.

Alternatively, can you just simulate the LM5022 section by itself, and in your larger system, just replace the LM5022's output rail with a dc voltage source?  This can simplify your effort?  

Thanks,

Youhao

Hi Youhao Xi,

I would like to retain the actual LM5022 design in the larger simulation as the positive and negative buck regulator outputs are subsequently converted into an AC voltage which may be loaded inductively. Amongst other things, I wish to simulate the circuit behavior when loaded inductively, and in particular to observe how the buck regulators and their large output capacitances behave when energy is regenerated by the load inductance pumping current back into the regulator outputs during portions of the synthesized AC cycle.

Unfortunately, you endorse my suspicions that I will have to modify the TI LM5022 SPICE model to refer to the LM5022 GND node instead of the SPICE global ground. I assume that this entails the following:

1. Changing all references to node 0 with references to the LM5022 GND pin in the main LM5022 subcircuit.
2. Adding a GND input node to all lower-level subcircuits that refer to node 0, and replacing all those references to node 0 with references to the added GND input node.

Can you confirm that this is what is required and perhaps point out any potential obstacles that I may encounter as I admit that I am not really familiar with the SPICE syntax.

Is there any particular reason why the TI model refers internally to the global node 0 rather than to the device's own GND node? Using global node 0 seems to ensure that the device cannot be simulated in topologies with multiple devices connected with their GND pins connected to different nodes, as in my application. Is there any advantage in device models internally referring to global node 0 that outweighs the limitations that this practice places on users' simulated designs? I wonder if you could perhaps bring this issue  to the attention of the TI SPICE model developers as a general issue that surely impacts a wide variety of TI SPICE models, rather than being a problem limited to the LM5022 model.

Regards,

David Drori, Novarex Technological Enterprises

Hi David,

First, you are right about the necessary changes. 

Regarding the model,  you can imagine many op-amps and logic circuits, and reference voltages are used in the behavioral model.  Modeling is not a simple task, and using the global node 0 in the modeling can prevent mistakes and facilitate the work.  After all, most applications and designs are not using the circuit on floating "ground".   Sorry, your use case seems not being considered when our engineers created the model.  We have noticed this from your post, and we are considering to take this into account in our future work. 

Thanks you, 

Youhao