TINA/Spice/LM5117: Unencrypted PSpice Transient Model

Aniket Kulkarni

Part Number: LM5117
Other Parts Discussed in Thread: TINA-TI,

Tool/software: TINA-TI or Spice Models

The un-encrypted PSpice model simulation returns error for the LM5117 when simulated with the SIMetrix simulation tool. The internal diode discontinuity error is the top issue.

over 6 years ago

0 Saket over 6 years ago

TI__Intellectual 2680 points

Hi Aniket,

Which version of Simterix are you using? You should not get these error in latest Simterix's version.
If you are facing this issue in latest version then kindly share the schematic file with me.

Regards,
Saket

0 Aniket Kulkarni over 6 years ago in reply to Saket

Prodigy 180 points

I am using the Simetrix 8.10. I have created the schematic with same circuit as in the Fig. 29 in the datasheet of the LM5117.

0 Saket over 6 years ago in reply to Aniket Kulkarni

TI__Intellectual 2680 points

Hi Aniket,

Could you please share your Simetrix schematic file?

Regards,
Saket

0 Aniket Kulkarni over 6 years ago in reply to Saket

Prodigy 180 points

DC-DC.sch

0 Saket over 6 years ago in reply to Aniket Kulkarni

TI__Intellectual 2680 points

Hi Aniket,

I was referring to .sxsch file that you were trying to run in Simetrix. Could you please send me that?
I will try to run it and see if I can suggest any solution.
Apologies for the confusion!

Regards,
Saket

0 Aniket Kulkarni over 6 years ago in reply to Saket

Prodigy 180 points

I understood it. The site doesn't support .sxsch files. I got error while uploading it. That's why, I changed the file name to .sch from .sxsch.

Please download the .sch file and rename it to .sxsch and open it in Simetrix.

0 Saket over 6 years ago in reply to Aniket Kulkarni

TI__Intellectual 2680 points

Got it Aniket!
But the schematic does not contain model definitions in F11 window and I am getting errors while running.Could you please share sxsch file along with model definitions?

One more thing, you are trying to run DC simulation on a transient model and we usually do not validate a transient model for DC simulations.

Regards,
Saket

0 Aniket Kulkarni over 6 years ago in reply to Saket

Prodigy 180 points

Hi Saket,

You need to load the spice definition for the LM5117 and PMSN5R5. That will solve the issue.

I tried the transient simulation but did not work. So I thought trying the DC simulation.

Please try the DC simulation.

You get the iterating limit and DC operating point error.

If it doesn't work, please suggest a way to share the .sxsch file as it cannot be uploaded here due to extension constraints.

Thanks.

Aniket

0 Saket over 6 years ago in reply to Aniket Kulkarni

TI__Intellectual 2680 points

Hi Aniket,

Try to zip it and share.
I will need a schematic file with diode,mosfet definitions in order to help you with this issue.

Regards,
Saket

0 Aniket Kulkarni over 6 years ago in reply to Saket

Prodigy 180 points

DC DC Converter.zipHi Saket,

The models for them are available online also. Here's the zip file. :)

0 Saket over 6 years ago in reply to Aniket Kulkarni

TI__Intellectual 2680 points

Thanks Aniket!
I am looking into the issue will try to get back by 16APR.

Regards,
Saket

0 Aniket Kulkarni over 6 years ago in reply to Saket

Prodigy 180 points

Hi Saket,

Waiting for your reply.

Regards,

Aniket

0 Saket over 6 years ago in reply to Aniket Kulkarni

TI__Intellectual 2680 points

Hi Aniket,

I simulated the setup and it's giving error in DC Bias point calculation. It seems to be an issue with Simetrix, not the model.(As same model works finein Pspice and TINA)
You can try to contact Simterix support team and see if they can help you with this issue.

I am trying few things here and will get back to you if I am able to fix this issue.
Thank you for your patience.

Regards,
Saket

0 Aniket Kulkarni over 6 years ago in reply to Saket

Prodigy 180 points

Thanks Saket.

I have sent the query to SIMetrix team. Just in case you missed to see the Convergence failure report, please have a look at it. It might help resolve the issue.

Regards,

Aniket

0 Aniket Kulkarni over 6 years ago in reply to Aniket Kulkarni

Prodigy 180 points

Hi Saket,

SIMetrix team solved my query.

Thanks for all the help.

Regards,

Aniket

0 Saket over 6 years ago in reply to Aniket Kulkarni

TI__Intellectual 2680 points

Great Aniket!

Could you please share how Simetrix team has fixed this issue?

Regards,

Saket

0 Aniket Kulkarni over 6 years ago in reply to Saket

Prodigy 180 points

Following are the steps SIMetrix team suggested.

The TI application circuit uses a mode which skips the DC operating point. The circuit will not run in any simulator without this setting. In SIMetrix you set this mode using this procedure:

1. Select menu Simulator | Choose analysis
2. lick on the Advanced Options button in the Transient tab
3. Check the Skip DC bias point box.

In addition we needed to set this option:

1. Select menu Simulator | Convergence Options
2. Under Slew rate for discontinuous sources enter a value of 1e16 for slew rate.

Also added VH=1m to every Switch model that defines the VT parameter and has not defined VH earlier. It is due to consideration of VH=1 by SIMetrix software.

I suggest TI can update the model relatively.

Regards,

Aniket

0 Saket over 6 years ago in reply to Aniket Kulkarni

TI__Intellectual 2680 points

Hi Aniket,

Thanks for sharing!

Regards,
Saket

Simulation, hardware & system design tools

Simulation, hardware & system design tools forum

TINA/Spice/LM5117: Unencrypted PSpice Transient Model