I just used TPS40170 in my power system. In TINA I simulated the original schematic, it is good. And I changed the BSC.. to SI7850DP, then because the Ron is different, so the resistor's value for OC and SC have also been changed.
But then, the simulation does not work. I read the datasheet again and the J/K selection method was considered to reducing the loss.
I also tried with SI4980DY, but neither worked. So I would like to know, why the external MOSFETs are not good, even in simulation!
Or any one has a solution to this problem?
Thanks in advanced
We have seen issues previously with vendor supplied FET models and the controller models for simulation in TINA-TI. What we have been using is a generic FET model which is the one that in included in the TPS40170 schematic. The device is named BSC... but it has only a few parameters that come from the datasheet for that device.
If you double click on the device, a window appears. Click on the SubCkt-Parameters line and then click on the ... box on the right side. This will show you the parameters that you can change to match the new FET that you have chosen (RDSON, CISS, CRSS, COSS and VSP). VSP is the Switching Point voltage (VGS value where the device starts switching).
Once you have made the changes to the parameters, you can rename the device to your chosen device and run the simulation.
thanks for your reply.
I used a pspice model for the FET and converted it into a macro in TINA and then simulated the circuit in TINA. But something went wrong and I got no results.
I tried the pspice model for TPS40170 in OrCAD, but it gave me always a "less than 2 connection" error. That's the reason, why I use TINA.
I take your suggestion and do the simulation again in TINA. The circuit was designed with SwitcherPro.
Now the simulation runs, but the result was not respected. I have to check it step by step. But at least I found the point to simulate and check.
Thanks and I will post my result, if it goes well.
Thanks to Britt's reply and it works now, I will post a summary about it:
1, Downloaded pspice model of SI7850DP works not good in TINA.
2, Change the parameters of BSC.. in the test circuit to fit the parameter of SI7850DP, and use this model as a model for SI7850DP.
3, Circuit was designed with SwitcherPro and simulated in TINA, in simulation we should change the SS Cap value to save time.
Now only one last question, why a pspice model does not work?
It is unkown, how much different between the changed model from BSC.. to SI7850DP'pspice model.
The PSpice model for the FET from the vendor user an older MOSFET model (MOS Level 3) that has some very good aspects and some very bad ones as well. In a simple circuit, the FET model may work fine in TINA-TI, however, when coupled with a much more complicated matrix due to the controller model, the simulator has trouble finding the correct solution, especially for a fast switching transient simulation.
A simulator is simply a linear equation solver (it doesn't know it is working on semiconductors) so the best solution may be for the circuit to simply do nothing. This is based on the many simulator settings that are available that determine the convergence of the simulator. In these cases, I cannot tell you exactly why the FET model does not work in the simulation. I can tell you that I have tried many different setting and models to avoid these cases without finding a better solution than the one I proposed.
There have been many situations where changing the FET to the vendor supplied model worked fine as well. Based on my experiences, it has been trial and error, and when no solution can be found with the vendor supplied FET, I use the simplified version.
Yes, using the simple model with parameter is the best and quickst solution. And we want to verify/simulate the design of TPS40170, not the dynamic behavior of a MOSFET, so at this point, your solution is a really good one.
If we talk about the simulation tools, then it might be something others.
TINA, is a TI supported sim-tool, means that one can simulate lots products of TI with it.
So at verifying the design with TI products, TINA is good and I think, TINA comes exactly for this reason.
I took TINA as a normal sim-tool, like OrCAD, but I might be wrong.
So now it is clear, LTspice for LT ,TINA for TI, and others with OrCAD.
All content and materials on this site are provided "as is". TI and its respective suppliers and providers of content make no representations about the suitability of these materials for any purpose and disclaim all warranties and conditions with regard to these materials, including but not limited to all implied warranties and conditions of merchantability, fitness for a particular purpose, title and non-infringement of any third party intellectual property right. TI and its respective suppliers and providers of content make no representations about the suitability of these materials for any purpose and disclaim all warranties and conditions with respect to these materials. No license, either express or implied, by estoppel or otherwise, is granted by TI. Use of the information on this site may require a license from a third party, or a license from TI.
TI is a global semiconductor design and manufacturing company. Innovate with 100,000+ analog ICs andembedded processors, along with software, tools and the industry’s largest sales/support staff.