[moved] Convergenge issue PSpice- LM5022

[Gerry95]

I designed a BOOST converter using LM5022 microcontroller. I got convergence issues and I have already tried to change the max Time step, deleting the snubber to get it easier, changing the simulation options, without any results.
The simulation shows there are 5 devices that fail to convergence.

Do you have any suggests to solve this problem?

 

[d123]

Hi,

Maybe posting an image of the convergence error pop-up as well will be more helpful.

I don't know what program you are using and you say you've already fiddled with the parameters with no success... In the one I use, changing the time to larger steps e.g. from 10G to 1m sometimes helps. Occasionally a part/the Spice netlist appears to cause the issue and sometimes it's the part itself that makes the simulation unviable - easy to solve if it's just swapping e.g. a "fancy"/newly available transistor for a common, well-modelled transistor, not so much if it's the IC you need to simulate. I think sometimes adding a resistor in the right place can solve these issues but I wouldn't know where to tell you to do so.

Maybe trying in another simulator to see if the same issue(s) arise(s)?

 

[BradtheRad]

* C4 can be removed. Or else put a low-ohm resistor inline with it. By itself it's charged immediately by the power supply. In real life it's okay to do this.
However the simulator works by mathematical calculations. With no resistance value the simulator is unable to calculate an RC time constant for C4 volt level from one frame to the next.

* Likewise CC4 might need a low-ohm resistor inline.

* Simplify locations where one ground icon serves two components. Then the simulator only needs to calculate two wires, not 3 or 4 or 5, and a node or 2 or 3.
Give the power supply its own ground icon.
Give C4 its own ground icon.
Give the IC its own ground icon.
Give C5 its own ground icon.
Give Rsense its own ground icon. Etc.

* L2-D2, L3-D3. Where you have a diode and inductor as neighbors, put a high-ohm resistor across one or both components. 10k or 100k is reasonable. Otherwise they might create ringing oscillations at shut-off.

* Sometimes a troublesome node (or terminal of a component) can be cured by installing a high-ohm resistor from the node to a supply rail.

 

[Gerry95]

Hi,

Maybe posting an image of the convergence error pop-up as well will be more helpful.

I don't know what program you are using and you say you've already fiddled with the parameters with no success... In the one I use, changing the time to larger steps e.g. from 10G to 1m sometimes helps. Occasionally a part/the Spice netlist appears to cause the issue and sometimes it's the part itself that makes the simulation unviable - easy to solve if it's just swapping e.g. a "fancy"/newly available transistor for a common, well-modelled transistor, not so much if it's the IC you need to simulate. I think sometimes adding a resistor in the right place can solve these issues but I wouldn't know where to tell you to do so.

Maybe trying in another simulator to see if the same issue(s) arise(s)?

Hello, I am using OrCad-Pspice for the simulation. I attached the output file with the convergence error.

 

[BradtheRad]

What is supposed to be the power supply for the control IC?
Your power supply icon appears to be AC. Instead it is normal to supply DC to a boost converter.

Start building your boost converter from the most simple basic topology. Remove the control IC. Apply a pulse train to the mosfet gate. Try various frequencies and duty cycles. The aim is to get it to work with no convergence errors. Or if you get an error then you'll have an easier time figuring out what to do about it.

 

[d123]

Hello, I am using OrCad-Pspice for the simulation. I attached the output file with the convergence error.View attachment 153154

Hi,

I am unfamiliar with OrCad so it would be pointless to speculate.

 

[Gerry95]

What is supposed to be the power supply for the control IC?
Your power supply icon appears to be AC. Instead it is normal to supply DC to a boost converter.

Start building your boost converter from the most simple basic topology. Remove the control IC. Apply a pulse train to the mosfet gate. Try various frequencies and duty cycles. The aim is to get it to work with no convergence errors. Or if you get an error then you'll have an easier time figuring out what to do about it.

The power supply range of the IC is 6-60 V. I have a specification of 200kHz abou the frequency. Before using IC, I got no error with a simplier circuit, using a pulse generator. So, the problem comes out when I use the IC and I don't know how to solve the convergence problem. I also tried to use the steady state conditions and a DC power supply without any results.

 

[FvM]

Did you try to run the PSPICE examples provided by TI along with the model?

 

[Gerry95]

Did you try to run the PSPICE examples provided by TI along with the model?

Yes, I used it first. It works properly so I also used the same setting options in the simulation window without solving my issue.

 

[BradtheRad]

The power supply range of the IC is 6-60 V.

Does it work (or does it break) if exposed to negative polarity?
What happens when the AC supply goes into negative region?

 

[andre_luis]

We don't know how the LM5022 component was internally modeled by TI, but depending on whether the SS input is "ideal" or not, e.g not trying to sink or to drain the smallest leak current, this can make voltage on the capacitor to stay floating, so as the first attempt I would try to add a high value resistor in parallel to the capacitor C_ss.

 

[FvM]

If the examples are working, it should be possible to move towards your circuit. I admit that SPICE convergence issues can be annoying and are sometimes hard to solve, particularly with very nonlinear devices like MOSFETs.

 

[Gerry95]

Does it work (or does it break) if exposed to negative polarity?
What happens when the AC supply goes into negative region?

I ve just checked and It does not work properly, I think It breaks because the pin voltage drops gets high. The minimum according to the datasheet is -0.3 V. Anyway, I tried to set a max time step of 10ns on 10ms of simulation and the convergence problem disappears but the simulation took more than 10 hours and the simulation time results higher than that I fixed in the setting. At 1% I stopped the simulation and the time was 18 ms.

 

[d123]

Anyway, I tried to set a max time step of 10ns on 10ms of simulation and the convergence problem disappears but the simulation took more than 10 hours (...) At 1% I stopped the simulation.

:laugh: I know that feeling.

 

[BradtheRad]

I tried to set a max time step of 10ns

Try increasing your tilmestep by 10x. Run the simulation again. If it makes you wait a long time then increase it further.

A reasonable timestep results in 100 frames per frequency period used in your circuit. So 10nS timestep is suitable when you have, say 1 MHz freq, running in your circuit. It's true when using a control IC that we don't know how to predict what frequency it will adjust to. Nevertheless since your inductor is 330uH, then it's likely to be slower than 1 MHz.