SN74LVC2G74: PSpice Model Simulation Error - Values Must Be Monotonic Increasing

Hey Jacob,

Can you share your project file so we can test the same way you are?

Hi Emrys,

See attached!

OPJ File: /cfs-file/__key/communityserver-discussions-components-files/151/Test_5F00_Project.opj

SN .olb file: /cfs-file/__key/communityserver-discussions-components-files/151/SN74LVC2G74.OLB

Thanks Karan! The fact it was for TINA would be the problem!

Hi Karan,

Apologies. I got too ahead of myself. I tried importing the .lib and macro wizard generated .olb into the simulation and I'm still getting the same "Values must be monotonic increasing."

Hi Jacob,

To share PSpice project, please follow this thread:

https://e2e.ti.com/f/1/t/969692

Thanks,
JC

Thanks JC. See attached.

/cfs-file/__key/communityserver-discussions-components-files/151/test_5F00_project_2D00_2021_2D00_10_2D00_11T18_2D00_12.zip

Hi Jacob,

Would you please share the model file SN74LVC2G74_spice.lib?  It was not copied into the zip file.

Thanks,
JC

Hi JC,

It's the same model that Karan shared above. I just labelled it as ".._spice" because I already had the TINA model saved as just the PN.

Karan Kotadia said:

SN74LVC2G74.lib

Hi Jacob,

not sure why. I got a different error:

Any suggestions?

Thanks,
JC

Hi JC,

I got that error initially as well. Some of the traces in the simulation may not actually be connected. Make sure to drag around the connections to ensure all nodes are connected. 

Once you do that, I expect you'll see the same error that me and my customer are seeing.

Thanks,
Jacob

Hi Jacob,

I am not sure about that. It seems to be legit. Net "18" is inside the model and as you can see, it really connects to C1 only.

So are you able to run the simulation without it crashing or throwing the "monotonic" error?

JC,

I made another update to the model syntax to fix the errors you are seeing. Can you please try again?

5582.SN74LVC2G74.lib

Regards,

Karan

Hi Karan,

It's a no-go. I got a new error:

ERROR(ORPSIM-16551): Floating point computation failed during Device/Model Load. Possible solutions: 1)Ensure that all device parameters are in valid range. 2)Try using .options LIMIT
Divide by Zero in device X_U2.XU11.XU1.XU1.XUOUT.EROH, Divide

Thanks,
JC

Hi team,

Any further progress on the model?

Thanks,

Jacob

Hi Jacob,

No. Same error (divide by zero).

Regards,
JC

Hi JC,

Thanks for the update. Do we have the ability to get around the error and make a working model or is this a dead-end error?

Thanks,

Jacob

Hi Jacob,

Please check my email offline.

Thanks,
JC

Hi Karan,

Reviving this thread. There was an issue with my PSpice version which was causing the unique "monotonic" error. JC helped me get on the latest version of PSpice and now I'm getting the "Less than 2 connections at node..." error.

Is there a way to update the model to remove this error?

Thanks,

Jacob

Hi Jacob,

This is the same error that JC is receiving.

I am not sure of the cause of this error.

JC Zhu do you think you can help with this?

Regards,

Karan

Hi Karan,

See my reply on 10/14. you have unconnected devices in the model:

C1          18 GND 1P

Hi JC,

I fixed this issue in the reply on 10/15 where I updated that model.
What is the issue there?

Regards,

Karan

Based on JC's reply, it seems the 10/15 model is throwing a new error. I re-tried running the simulation with the 10/15 model and got the following: 

ERROR(ORPSIM-16551): Floating point computation failed during Device/Model Load. Possible solutions: 1)Ensure that all device parameters are in valid range. 2)Try using .options LIMIT

INTERNAL ERROR -- Divide by Zero in device X_U1.XU11.XU1.XU1.XUOUT.EROH, Divide

Hi Albert,

Thanks for the update! 

Hi Karan,

I tried the new model and am getting the connections error again. JC Zhu are you seeing the same error?

Hey Jacob,

I have another '74 function PSpice model that I've been working on that's been a bit "hit or miss" for simulation in PSpice for TI.

I have seen it work without problems, work after not converging once, and completely fail to converge.

If you switch to a dfiferent simulator (Tina-TI, Altium, etc.) then this version seems to work flawlessly.

If you'd like to try it, I attached the files below. The appropriate subcircuit to use is the "SN74LVCXG74" -- others are components of the device.

SN74LVCXG74.OLB

SN74LVCxG74.LIB

Thanks for sharing Emrys! I tried running the model in PSpice and I was getting the convergence issue. I tried making my rise/fall times on the scale of ms, but still ran into the same issue. 

I wonder why it is acting up in some simulators and working fine in others.

Great catch JC!

Karan KotadiaAny suggestions for what we should change one of the x values to? Or is the x value perhaps incorrect for one of the lines?

Hey Team,

I'm not as experienced with modeling as Karan and Emrys, can we wait until after the holiday for them to reply? I'll make a note so they get back to it first thing Monday.

Hey Jacob,

Usually we would have the first value at 2.99V and the second at 3.01V so that there is a 'step' between those.

I'd recommend instead to remove the second 3V line, and change the first to an average of the two values:

+(1.65,112.5)
+(2.3,50)
+(3,33.333)
+(4.5,21.875)

The output resistance value is based on the datasheet "worst case" -- so if you want to have more "typical" operation instead, I'd use these values:

+(1.65,55)
+(2.3,25)
+(3,16)
+(4.5,10)

Note that you'd have to change both the EROH (Resistance for Output HIGH) and EROL (Resistance for Output Low) tables

Hi team,

It was a long journey, but the model is working for me! I made the modifications suggested by Emrys and initial testing is showing the appropriate behavior. Thanks for all the help!

/cfs-file/__key/communityserver-discussions-components-files/151/2022.SN74LVC2G74.lib

/cfs-file/__key/communityserver-discussions-components-files/151/5582.SN74LVC2G74.OLB

Hey Jacob,

I really appreciate you being patient and working with us to get this figured out.

Please come back any time if you need help again.