Hey there,
I'm finding it impossible to simulate this part in PSPICE when configured as a buck-boost (to give -5V with a +18V input)
The nodes that do not converge are all within the switcher model.
Any tips?
Thanks for the help,
Adam
This thread has been locked.
If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.
Hey there,
I'm finding it impossible to simulate this part in PSPICE when configured as a buck-boost (to give -5V with a +18V input)
The nodes that do not converge are all within the switcher model.
Any tips?
Thanks for the help,
Adam
Hi Adam,
Although we have verified the device does function in the buck-boost configuration, I am not sure this was taken into account when this model was created. I am looping in our modeling expert to confirm.
Thanks
Christian
Hi Adam,
This model is compatible with running simulations using an Inverting Buck Boost configuration. Can you share your simulation settings? What step size are you using?
Somehow I attached that previous image 5 times or so, Ooops! I tried the default settings and then played around like crazy with the auto convergence and reducing tolerances etc. The default time step in the files I downloaded was 20ns, I tried 2ns as well. To be sure that I didn't do something silly, I took the original files downloaded, modified the ground structure slightly so that it then an inverting buck boost and still had the convergence issues. I'm running PSPICE 17.2 so maybe that's responsible?
Hi Adam,
Thanks for sharing your schematic, simulation settings, and what steps you've taken to troubleshoot so far. All of this is very helpful.
I don't think the issue is stemming from the version of PSpice you're running. Let me try running simulations using the setup shown in your schematic to see if I get the same error. That will narrow down whether the issue is with the configuration or the simulation itself.
I'll get back to you shortly.
Thanks,
Sarah
Hi Adam,
Can you let me know if you are able to run a simulation using the following simulation settings along with a 20ns maximum step size?
Using these settings with your schematic I'm able to produce a -3.3V output.
Thanks,
Sarah
Unfortunately it still doesn't simulate for me. Perhaps I could try copying your advanced convergence settings? Are you using the auto converge feature?
No worries, I have the same issue with drag-drop attachments. Usually using Insert->Image/Video/File works without duplicating attachments.
Interesting. I notice that your setting for ITL4 is still at 100. Can you update this to 400 and let me know if there is any change to the result? And can you also confirm you've set the the maximum step size to 20ns and that VOUTIC is set to 0?
Thanks,
Sarah
So looks like it was already at ITL400 but the Advanced convergence feature was reducing it to 100 for some reason. When I turned that off it stayed at 400 but unfortunately still doesn't converge. So perhaps the advanced settings are where the differences are now. Or perhaps our simulation models are different? I've attached the PSPICE project just incase that helps figure out where the difference lies.
Hey Adam,
Thanks for the project files.
It looks like the feedforward capacitor and the top feedback resistor are why you were getting convergence errors and I was not. Using the smaller resistor values you showed in your previous schematic screenshot, the simulation is able to run successfully. However, after updating my component values to match those used in the project files you sent, I started running into the same issues.
If you revert to the smaller resistances used in the original schematic screenshot you shared, the simulation should run. Another option would be to decrease the value of the feedforward capacitor to something like 2.2p and using Rtop=10k & Rbottom=4.32k. I believe the time constant of Cff and Rtop are what is causing trouble for PSpice, but need to look into this more.
Can you let me know if you are able to run a successful simulation with these alterations?
Thanks,
Sarah
Sorry I missed your update until now and have now tried your recommendation. It works! I get the expected output voltage given the resistors loaded. I'll keep this in mind for any further simulations I do! :) Thanks for the help!! :)