TINA/Spice/INA286: ERROR(ORPSIM-16352): Time value must not be an expression

John Conwell

Part Number: INA286
Other Parts Discussed in Thread: TINA-TI,

Tool/software: TINA-TI or Spice Models

Hello,

I am currently simulating a design that includes the PSpice model for the INA286, downloaded from the TI website. When I attempt to run the simulation, I get the following error (U2 references the INA286):

**** EXPANSION OF SUBCIRCUIT X_U2.XU1.XControl.XClkF1 ****
.PARAM TR_TM { IF (TR_MODE > 0.5, 1, 1000000 ) }
X_U2.XU1.XControl.XClkF1.VCLKF1 X_U2.XU1.XControl.46
+ X_U2.XU1.XControl.XClkF1.3 DC 0 AC 0 0 PWL 0 0 100N 0 REPEAT
+ FOREVER 0 0 1N -1 {2.015U*TR_TM}
--------------------$
ERROR(ORPSIM-16352): Time value must not be an expression

**** EXPANSION OF SUBCIRCUIT X_U2.XU1.XControl.XClkF32 ****
.PARAM TR_TM { IF (TR_MODE > 0.5, 1, 1000000 ) }
X_U2.XU1.XControl.XClkF32.VCLKF32 X_U2.XU1.XControl.ClkF3
+ X_U2.XU1.Startup DC 0 AC 0 0 PWL 0 0 125N 0 REPEAT FOREVER 0 0 1N 1 {50N*TR_TM}
----------------------------------------------------------------------$
ERROR(ORPSIM-16352): Time value must not be an expression

**** EXPANSION OF SUBCIRCUIT X_U2.XU1.XControl.XClkF2 ****
.PARAM TR_TM { IF (TR_MODE > 0.5, 1, 1000000 ) }
X_U2.XU1.XControl.XClkF2.VCLKF2 X_U2.XU1.XControl.48 0 DC 0 AC 0 0
+ PWL 0 0 125N 0 REPEAT FOREVER 0 0 1N 1 {1.965U*TR_TM}
-----------------------------------------$
ERROR(ORPSIM-16352): Time value must not be an expression

I have attached the relevant simulation file (.lib). What can I do to solve this?

ThanksINA286.lib

over 6 years ago

0 John Miller - Sensing over 6 years ago

TI__Mastermind 34005 points

John,

Thank you for the inquiry.
What simulator are you using?

Regards,
John

0 John Conwell over 6 years ago in reply to John Miller - Sensing

Prodigy 60 points

Hi John,
I am using Cadence OrCad PSpice.

0 John Miller - Sensing over 6 years ago in reply to John Conwell

TI__Mastermind 34005 points

John,
What version of Cadence are you using?
Can you share the project/schematic where you are seeing the error?
Regards,
John

0 John Conwell over 6 years ago in reply to John Miller - Sensing

Prodigy 60 points

John,

I am using Cadence version 17.2-2016 S035 (I have attached the about screen if this is not enough). I have also attached the project.

INA286_EXAMPLE.zip

0 John Miller - Sensing over 6 years ago in reply to John Conwell

TI__Mastermind 34005 points

Thank you John.

I will look at it and get back to you tomorrow or early next week.

Regards,
John

0 John Miller - Sensing over 6 years ago in reply to John Miller - Sensing

TI__Mastermind 34005 points

John,

Just a quick update.
I have been able to reproduce the error you have seen with the INA286 model in Cadence v17.2
Apparently Pspice doesn't like the format of some calculations done in some of the internal clocks.
I will keep looking at this and hopefully have a fix early next week.

Interestingly, TINA doesn't seem to have a problem with the same formats & calculations.

Regards,
John

0 John Conwell over 6 years ago in reply to John Miller - Sensing

Prodigy 60 points

John,

Thank you for your help! I look forward to hearing from you.

John

0 John Conwell over 6 years ago in reply to John Miller - Sensing

Prodigy 60 points

Hi John,

Any updates?

Thanks,

John

0 John Miller - Sensing over 6 years ago in reply to John Conwell

TI__Mastermind 34005 points

John,

I could not yet figure out a clever workaround for the main error, but I hope to have a brute-force solution later today.

The .lib files didn't seem to be included in your Cadence hierarchy. It's not a big deal for the INA286, but what model do you use for S1?

Regards,
John

0 John Conwell over 6 years ago in reply to John Miller - Sensing

Prodigy 60 points

S1G.libIt seems I forgot to add it. Here it is.

Thanks,

John

0 John Miller - Sensing over 6 years ago in reply to John Conwell

TI__Mastermind 34005 points

Thanks for the diode model John.

The error you found comes from some internal clocks that are intended to mimic the switching in the real device.
Unfortunately the clocks use some equations that aren't compatible with the latest version of Cadence.
The intent was to be able to enable or disable the clocks by setting a local PARAM called TR_MODE to zero or one.
The advantage of enabling the clocks (TR_MODE = 1) would be to mimic the switched loading at some of the pins, but the disadvantage would be longer sim times. The advantage of disabling the clocks (TR_MODE = 0), would be faster sim times.

The original model has been split into two distinct models. One has the internal clocks enabled (_CLOCKED), the other has the clocks disabled (_UNCLOCKED).
The models are in separate Pspice v17.2 projects attached to this thread.

Please give them a try and let me know if you have any more questions or concerns.

Regards,
John

INA286_CLOCKED.zip

INA286_UNCLOCKED.zip

Simulation, hardware & system design tools

Simulation, hardware & system design tools forum

TINA/Spice/INA286: ERROR(ORPSIM-16352): Time value must not be an expression