PSpice - Recent Threads

How to define measurement statements to get simulation output results in a textual format ?

AyushD — Mon, 03 Feb 2025 12:02:34 GMT

Allegro PSpice Simulator allows us to define measurement statements that can analyze simulation data of different analysis types and generate a text file with measurement data on the output simulation waveform.

You can use the `.MEAS` or `.MEASURE` command the `.MEAS`. The measurements are assigned to unique variables defined by the user, which can be invoked in other measurement expressions.

To use these measurements, you can create a new text file with the `.inc` extension and add the measurement commands.
Configure the file in the design simulation settings.

The measurement results will be generated as a text file inside the project folder after a successful simulation.

There are several types of measurements you can perform using the `.MEAS` command:

1. `TRIG...TARG`: Find the difference in the x-axis value (time/frequency/variable) when conditions are met (between the trigger point and the target point)
2. `FIND...WHEN`: Find the value of the argument when the specified condition is met.
3. `AVG, MIN, MAX, PP, RMS, MIN_AT, MAX_AT`: Calculate average, minimum, maximum, peak-to-peak, RMS, minimum at, and maximum at values.
4. `PARAM`: Measure a parametric expression defined in curly braces.

The general syntax for the `.MEAS` command is:
.MEASURE {DC|AC|TRAN} <measurement variable name>

Example: Find the average voltage of the node ‘out’ within a time interval of 1 ms to 1.2 ms.

.MEAS TRAN avg_out_vAVG V(out) FROM 1m TO 1.2m

Result: AVG_OUT_V: AVG(V(OUT))= 3.9711E+00 FROM 1.0000E-03 TO 1.2000E-03

RE: How to define measurement statements to get simulation output results in a textual format ?

JX202609134513 — Mon, 14 Sep 2026 07:18:31 GMT

I have tried the method you suggested. I added an .inc include file under Configuration Files in Cadence Capture CIS 17.4. This .inc file contains only one single line: .MEAS TRAN VOUT_at_5ms FIND V(VOUT) AT 5ms

After running the simulation, I encountered an error message in the .out output file as shown below:

【**** INCLUDING my_measure.inc ****
.MEAS TRAN VOUT_at_5ms FIND V(VOUT) AT 5ms
$
ERROR(ORPSIM-16056): Unrecognizable command】

I replaced .MEAS with .MEASURE, but the error remained unchanged. Could you please advise why this error occurs and how I can resolve it?

RE: problems with smoke simulation

IshaS — Fri, 11 Sep 2026 09:44:05 GMT

Hi Digital1,

There seemed to be symbol name and pin-mismatch.

Great issue is resolved.

problems with smoke simulation

digital1 — Mon, 07 Sep 2026 10:30:11 GMT

I have a simple resistive circuit R1 and R2, R2 comes from the menu Place / PSpice Part/ Resistor and R1 comes from my CIS Cip database.

I have all the smoke parameters set up the same but for the R1 I have
the following non fatal errors

Voltage Data not found for smoke test RV

Please verify save data and data collections options in the simulation profile

R2 gives me the voltage data expressed as RV but R1 from my cip database does not

Has anybody else found this error and if so how do I correct it

RE: problems with smoke simulation

digital1 — Thu, 10 Sep 2026 16:25:16 GMT

Hi IshaS I found a workround my capture symbol was called resistor and the pspice symbol was called R when I renamed my capture symbol to R the problem went away sounds like one of those silly bugs

RE: problems with smoke simulation

digital1 — Thu, 10 Sep 2026 15:16:21 GMT

Hi IshaS

Thank you for your reply. I can say that Data collection for voltage current and power is set correctly otherwise surely i wouldnt have voltage data for R2
For statement 2 I have not used port names just 2 resistors and 1 dc voltage source and a pspice ground.here is the pspice netlist

V_V3 N00133 0 35Vdc
R_R1 N00133 N00145 R_R1 10k TC=0.00005,0
.model R_R1 RES R=1 DEV=1% TC1=0.00005 TC2=0
R_R2 N00145 0 1k TC=0,0

The main difference is R1 gives me a model statement and R2 doesn't but if i give R2 a tolereance then R2 has a model statement but it still gives me the voltage simulated or RV as it is called in smoke

R2 gives me the voltage data but R1 doesn't here is the smoke window from this simulation

AAs you can see I am using the latest version of Orcad

II really need this to work for 1 other thing all my smoke parameters come from CIS CIP and taken from manufacturers datasheets. As you can see all the other smoke parameters for R1 is working correctly

Improving Fourier (FFT) Accuracy in PSpice

IshaS — Wed, 09 Sep 2026 19:12:13 GMT

In PSpice, you can often improve the accuracy of your Fourier (spectral) analysis by modifying your transient analysis setup.

Accurate Fourier analysis in PSpice depends on selecting appropriate transient simulation settings. The quality of the FFT is directly influenced by the simulation duration, time-step resolution, and overall numerical accuracy.

Here are some guidelines for getting more accurate results:

_Final Time_

where Tss = Time to reach steady state.

The output must reach steady-state before you can even begin to look at the data. Otherwise, the signal is not periodic, and it will introduce noise in the Fourier transform. You can set the No-Print Delay (from the Analysis menu, choose Setup, then click Transient) to Tss to avoid having to restrict the data when using the FFT feature of Probe. Although the simulation still begins at Time=0, No-Print Delay effectively truncates the leading portion of the data file, making it smaller without affecting the accuracy of the FFT.

N = Integer number of cycles to be transformed (Frequency domain resolution = F0/N)

It is usually best to use 5 or more cycles; the magnitude of the frequency components between harmonics (which should be zero) gives you an idea of what the effective noise-floor of the transform is.

F0 = Fundamental frequency

In multi-tone analyses, F0 is the highest frequency of which all input frequencies are integer multiples, i.e., F0 = Fi / Ni for all input frequencies Fi, where Ni are arbitrary integers. If you are using the Fourier Analysis function of PSpice, then you should specify the fundamental frequency as F0/N to get the frequency resolution discussed above.

_Step Ceiling (and Print Step)_

Nfh = Highest harmonic component with a "significant" amplitude.

The Nfh component must be well resolved, at about 25-100 points per cycle (Ntres)."Significant" indicates relative amplitude compared to components to be measured.For example, consider a 1kHz sine wave into a highly nonlinear system. To study the first 5 harmonics, set the Step Ceiling (and Print Step) to 1/(5*1kHz*25)=8us. However, if the accuracy required is 1mV, and one of the neglected higher harmonics is greater than 1mV, then the higher harmonic component can "fold back" (a kind of aliasing) and disrupt the accuracy of the harmonics being measured.

25 This range was derived empirically, but it is interesting to note that if one period of a sine wave is represented by 25 evenly spaced points with linear interpolation, then the maximum possible error is approximately 0.8%,and with 100 points, the maximum error is approximately 0.05%.

_Simulation Accuracy_

Simulation accuracy is limited to about 3-3.5 digits (60-70dBc). The accuracy can be improved by tightening tolerances and taking the above considerations to extremes, but not by very much. This may not be considered sufficient for some applications, but keep in mind that even the best simulation models are probably not accurate enough to provide better results.

Do share your insights which one from the above helped !!.

Happy Learning.

RE: problems with smoke simulation

IshaS — Wed, 09 Sep 2026 12:17:16 GMT

Hi,

This error can come due to one of the following reasons:

1. Data collection for voltage, current and power not set correctly.

In order to resolve this go to PSpice > Edit Simulation Profile > Data Collection and ensure that for Voltages , Current and Power ALL is selected.

If not then change from the drop down to ALL.

2. This error can also come due to incorrect test node mapping.
Port names defined in test node mapping should be same as the pin name of component which is defined in PSpiceTemplate.

If there is a mismatch here, then this error will be reported.

To resolve this, edit the model and check Test Node Mapping. Make sure that port names are same as defined in PSpiceTemplate.

Can you please check, hopefully the above solution shall help.

Do share your input, how it goes.

RE: Wrong JFET parameters when using nested param .DC sweep

MK202608101044 — Wed, 12 Aug 2026 07:38:03 GMT

Hello, the minimal example I provided is the whole circuit. The problem came up during different simulation, but the problem is the same -> JFET parameters get calculated incorrectly causing the JFET to behave incorrectly as well.

I had trouble uploading the .out files, so I just copied the contents here. (it worked at first, but then after refresh I was not able to upload them)

Working:

**** 08/12/26 09:21:54 *** PSpice 25.1.0 (14 September 2025) ** ID# 0 ********

**** CIRCUIT DESCRIPTION

******************************************************************************

.param vd_p=0

vd d 0 {vd_p}

j1 d 0 0 myjfet

.model myjfet njf t_measured=25

.dc TEMP LIST -50 -25 0 25 50 75 100 125 150 175 200 ; param vd_p 0 1 1

**** 08/12/26 09:21:54 *** PSpice 25.1.0 (14 September 2025) ** ID# 0 ********

**** Junction FET MODEL PARAMETERS

******************************************************************************

myjfet
NJF
T_Measured 25
T_Current 27
VTO -2
BETA 100.000000E-06

Model-Specific Temperatures During Sweep Param value = -50

**** JFET MODEL PARAMETERS

myjfet (T_Current -50 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.071E-21
PB 1.064E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = -25

**** JFET MODEL PARAMETERS

myjfet (T_Current -25 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 9.554E-19
PB 1.044E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 0

**** JFET MODEL PARAMETERS

myjfet (T_Current 0 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.474E-16
PB 1.022E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 25

**** JFET MODEL PARAMETERS

myjfet (T_Current 25 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.000E-14
PB 1.000E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 50

**** JFET MODEL PARAMETERS

myjfet (T_Current 50 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 3.602E-13
PB 9.767E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 75

**** JFET MODEL PARAMETERS

myjfet (T_Current 75 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 7.884E-12
PB 9.526E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 100

**** JFET MODEL PARAMETERS

myjfet (T_Current 100 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.158E-10
PB 9.277E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 125

**** JFET MODEL PARAMETERS

myjfet (T_Current 125 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.229E-09
PB 9.019E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 150

**** JFET MODEL PARAMETERS

myjfet (T_Current 150 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 9.976E-09
PB 8.755E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 175

**** JFET MODEL PARAMETERS

myjfet (T_Current 175 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 6.475E-08
PB 8.484E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 200

**** JFET MODEL PARAMETERS

myjfet (T_Current 200 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 3.480E-07
PB 8.206E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures After Sweep Param value = 27

**** JFET MODEL PARAMETERS

myjfet (T_Current 27 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.361E-14
PB 9.982E-01
CGS 0.000E+00
CGD 0.000E+00

JOB CONCLUDED

**** 08/12/26 09:21:54 *** PSpice 25.1.0 (14 September 2025) ** ID# 0 ********

**** JOB STATISTICS SUMMARY

******************************************************************************

Total job time (using Solver 1) = .02

Failing:

**** 08/12/26 09:19:04 *** PSpice 25.1.0 (14 September 2025) ** ID# 0 ********

**** CIRCUIT DESCRIPTION

******************************************************************************

.param vd_p=0

vd d 0 {vd_p}

j1 d 0 0 myjfet

.model myjfet njf t_measured=25

.dc TEMP LIST -50 -25 0 25 50 75 100 125 150 175 200 param vd_p 0 1 1

**** 08/12/26 09:19:04 *** PSpice 25.1.0 (14 September 2025) ** ID# 0 ********

**** Junction FET MODEL PARAMETERS

******************************************************************************

myjfet
NJF
T_Measured 25
T_Current 27
VTO -2
BETA 100.000000E-06

Model-Specific Temperatures During Sweep Param value = 0

**** JFET MODEL PARAMETERS

myjfet (T_Current -50 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.071E-21
PB 1.064E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = -25

**** JFET MODEL PARAMETERS

myjfet (T_Current -25 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.979E-25
PB 1.097E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 0

**** JFET MODEL PARAMETERS

myjfet (T_Current 0 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.917E-27
PB 1.111E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 25

**** JFET MODEL PARAMETERS

myjfet (T_Current 25 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.917E-27
PB 1.111E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 50

**** JFET MODEL PARAMETERS

myjfet (T_Current 50 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.051E-25
PB 1.097E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 75

**** JFET MODEL PARAMETERS

myjfet (T_Current 75 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 8.282E-23
PB 1.066E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 100

**** JFET MODEL PARAMETERS

myjfet (T_Current 100 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 9.589E-19
PB 1.010E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 125

**** JFET MODEL PARAMETERS

myjfet (T_Current 125 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.178E-13
PB 9.157E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 150

**** JFET MODEL PARAMETERS

myjfet (T_Current 150 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.176E-07
PB 7.558E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 175

**** JFET MODEL PARAMETERS

myjfet (T_Current 175 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 7.612E-01
PB 4.814E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 200

**** JFET MODEL PARAMETERS

ERROR(ORPSIM-15007): Model myjfet has negative PB.
myjfet (T_Current 200 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.649E+07
PB -2.389E-03
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 1

**** JFET MODEL PARAMETERS

myjfet (T_Current -50 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.071E-21
PB 1.064E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = -25

**** JFET MODEL PARAMETERS

myjfet (T_Current -25 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.979E-25
PB 1.097E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 0

**** JFET MODEL PARAMETERS

myjfet (T_Current 0 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.917E-27
PB 1.111E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 25

**** JFET MODEL PARAMETERS

myjfet (T_Current 25 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.917E-27
PB 1.111E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 50

**** JFET MODEL PARAMETERS

myjfet (T_Current 50 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.051E-25
PB 1.097E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 75

**** JFET MODEL PARAMETERS

myjfet (T_Current 75 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 8.282E-23
PB 1.066E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 100

**** JFET MODEL PARAMETERS

myjfet (T_Current 100 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 9.589E-19
PB 1.010E+00
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 125

**** JFET MODEL PARAMETERS

myjfet (T_Current 125 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.178E-13
PB 9.157E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 150

**** JFET MODEL PARAMETERS

myjfet (T_Current 150 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.176E-07
PB 7.558E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 175

**** JFET MODEL PARAMETERS

myjfet (T_Current 175 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 7.612E-01
PB 4.814E-01
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures During Sweep Param value = 200

**** JFET MODEL PARAMETERS

ERROR(ORPSIM-15007): Model myjfet has negative PB.
myjfet (T_Current 200 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 2.649E+07
PB -2.389E-03
CGS 0.000E+00
CGD 0.000E+00

Model-Specific Temperatures After Sweep Param value = 0

**** JFET MODEL PARAMETERS

myjfet (T_Current 27 T_Measured 25)

VTO -2.000E+00
BETA 1.000E-04
IS 1.361E-14
PB 9.982E-01
CGS 0.000E+00
CGD 0.000E+00

JOB CONCLUDED

**** 08/12/26 09:19:04 *** PSpice 25.1.0 (14 September 2025) ** ID# 0 ********

**** JOB STATISTICS SUMMARY

******************************************************************************

Total job time (using Solver 1) = .52

Wrong JFET parameters when using nested param .DC sweep

MK202608101044 — Mon, 10 Aug 2026 08:04:28 GMT

Hello, I didn't find a bug reporting feature, so I will try here.

When simulating a TEMP sweep I stumbled across a bug with njf model. Its parameters get calculated differently based on the chosen sweep type. I created a minimal example here:

Input:

.param vd_p=0

vd d 0 {vd_p}

j1 d 0 0 myjfet

.model myjfet njf t_measured=25

.dc TEMP LIST -50 -25 0 25 50 75 100 125 150 175 200 ; param vd_p 0 1 1

Output:

...
myjfet (T_Current -50 T_Measured 25)
PB 1.064E+00
...
myjfet (T_Current -25 T_Measured 25)
PB 1.044E+00
...
myjfet (T_Current 0 T_Measured 25)
PB 1.022E+00
...
myjfet (T_Current 25 T_Measured 25)
PB 1.000E+00
...
myjfet (T_Current 50 T_Measured 25)
PB 9.767E-01
...
myjfet (T_Current 75 T_Measured 25)
PB 9.526E-01
...
myjfet (T_Current 100 T_Measured 25)
PB 9.277E-01
...
myjfet (T_Current 125 T_Measured 25)
PB 9.019E-01
...
myjfet (T_Current 150 T_Measured 25)
PB 8.755E-01
...
myjfet (T_Current 175 T_Measured 25)
PB 8.484E-01
...
myjfet (T_Current 200 T_Measured 25)
PB 8.206E-01
...
myjfet (T_Current 27 T_Measured 25)
PB 9.982E-01
...

This example produces normal results. However, if I add a nested parameter sweep, the calculated JFET parameters are wrong, resulting even in an error.

Input:

.param vd_p=0

vd d 0 {vd_p}

j1 d 0 0 myjfet

.model myjfet njf t_measured=25

.dc TEMP LIST -50 -25 0 25 50 75 100 125 150 175 200 param vd_p 0 1 1

Output:

...
myjfet (T_Current -50 T_Measured 25)
PB 1.064E+00
...
myjfet (T_Current -25 T_Measured 25)
PB 1.097E+00
...
myjfet (T_Current 0 T_Measured 25)
PB 1.111E+00
...
myjfet (T_Current 25 T_Measured 25)
PB 1.111E+00
...
myjfet (T_Current 50 T_Measured 25)
PB 1.097E+00
...
myjfet (T_Current 75 T_Measured 25)
PB 1.066E+00
...
myjfet (T_Current 100 T_Measured 25)
PB 1.010E+00
...
myjfet (T_Current 125 T_Measured 25)
PB 9.157E-01
...
myjfet (T_Current 150 T_Measured 25)
PB 7.558E-01
...
myjfet (T_Current 175 T_Measured 25)
PB 4.814E-01
...
ERROR(ORPSIM-15007): Model myjfet has negative PB.
...
myjfet (T_Current 200 T_Measured 25)
PB -2.389E-03
...
myjfet (T_Current 27 T_Measured 25)
PB 9.982E-01
...

When using .step instead of the nested sweep, it works normally. It also works normally using nested sweep, when sweeping a source and not a param.

Tested on version PSpice 25.1.0, PSpice 24.1.0 and PSpice 17.4.0

Best regards,

Matej

RE: Wrong JFET parameters when using nested param .DC sweep

IshaS — Wed, 12 Aug 2026 05:39:12 GMT

Hi,

Could you share the complete simulation output (.OUT file) for both.

- Working case (TEMP sweep only)
- Failing case (TEMP sweep + parameter sweep)

Also, just to confirm the same simulation circuit was used to perform above, right?

Your access to On-Demand Webinar : From Wall to Rail – Turning Rules of Thumb into Proof

Renu Vibha — Wed, 29 Jul 2026 05:50:12 GMT

Rules of thumb don't pass safety reviews; proof does.

This webinar demonstrates constraint-driven flyback design in Cadence’s Allegro X Design Platform and PSpice.

See how to verify hot-loop geometry, isolation spacing, and startup behavior before you build hardware.

For more details , check From Wall to Rail – Turning Rules of Thumb into Proof | Cadence

Modeling Schottky Diodes in PSpice – Understanding IS and N Parameters

IshaS — Tue, 28 Jul 2026 09:32:41 GMT

Schottky diodes are indispensable part of modern hardware design. Their low forward voltage drop (typically 0.2–0.45 V versus 0.6–0.7 V for a standard PN junction) and near-zero reverse recovery time make them go-to choice in high-frequency switching power supplies, RF signal detection, OR-ing circuits, and flyback clamp networks. Wherever efficiency, speed, or tight voltage headroom matters, a Schottky is usually in the signal path.

But selecting the right device is only half the job. Simulating it accurately is the other half and that's where most designs quietly go wrong.

In PSpice, a Schottky diode's behavior is governed primarily by two model parameters: IS (reverse saturation current) and N (ideality factor). These two values define the entire shape of the I-V curve. Get them right, and your simulation predicts forward voltage drop, power dissipation, and switching behavior with confidence. Get them wrong - which happens whenever you use an unverified default model - and every downstream calculation built on that simulation is off including thermal margins, efficiency estimates and gate drive timing.

This post walks through how to tune IS and N in PSpice using nested DC sweeps, so your simulation matches the datasheet and holds up on the bench.

The diode current is governed by the equation:
I = IS (e^(V / (N·Vt)) − 1)

This indicates that both IS and N play an important role in determining the forward voltage characteristics.

IS (Reverse Saturation Current): Determines where along the voltage axis the I-V curve sits. In Schottky models, IS is typically several orders of magnitude larger than in standard PN junctions — often in the μA to mA range — which is the physical reason Schottky diodes conduct at a lower forward voltage. A lower IS shifts the curve to the right, increasing Vf for a given forward current. A higher IS shifts it left, reducing Vf.

N (Ideality Factor): Controls the steepness of the exponential rise. An ideal diode has N = 1; real Schottky devices typically fall between 1.0 and 2.2 depending on the junction technology and operating region. A higher N flattens the curve — you need more voltage to drive the same current — and also makes the forward voltage more sensitive to temperature variation.

Together, IS sets the operating point and N shapes the curve around it. Both need to be calibrated to the actual device for the simulation to be trustworthy.

Simulation Steps:

Perform a DC sweep analysis on a forward-biased circuit.

Use Parametric sweeps to vary IS and N independently.
Example ranges:
- IS: 3e-04 to 3e-08
- N: 2.2 to 3
Observe resulting changes in forward voltage and current characteristics.

Effect of IS (Reverse Saturation Current):

- Forward voltage drop can be tuned by modifying IS.
- A lower IS results in a higher forward voltage for the same current.

Effect of N (Ideality Factor):
- Controls the slope of the I-V curve.
- Changing N modifies exponential behavior and deviation from ideal characteristics.

This approach helps in accurately matching the diode model to real device behavior and achieving reliable simulation results.

Have you run into a Schottky (or any diode) model that just wouldn’t match the datasheet or your bench data?
Drop your experience in the comments – what device, what mismatch, and how you resolved it.

Happy Learning!!

Associate psice model greyed out

Shashank — Tue, 21 Jul 2026 16:35:43 GMT

OrCAD X Capture 24.1.
Created Project A without selecting Enable PSpice Simulation.
Created Project B with Enable PSpice Simulation selected.
Placed the same SamacSys Library Loader component in both projects.
In Project A, Associate PSpice Model is grayed out.
In Project B, Associate PSpice Model is enabled.
Since Simulation Profile can still be created in both Projects , I am unsure why only Associate PSpice Model is disabled.
Is this expected behavior in OrCAD X Capture 24.1?
Is there a supported way to enable Associate PSpice Model in an existing project created without Enable PSpice Simulation, or is creating a new PSpice-enabled project required?
Is there any project setting that controls the availability of Associate PSpice Model?

RE: Associate psice model greyed out

Shashank — Thu, 23 Jul 2026 11:24:11 GMT

Hi Isha,

Thanks for the reply!

In custom libraries(manually created) and online downloaded libraries this option is greyed out.

Is there any way to change this to PSpice specific project?

RE: Associate psice model greyed out

IshaS — Thu, 23 Jul 2026 11:07:32 GMT

Hi Shashank,

This appears to be expected behavior.
When a project is created without selecting "Enable PSpice Simulation", the project is treated as a standard schematic project and certain PSpice-specific commands are disabled.
One of those commands seems to be Associate PSpice Model. Even though Capture may still allow creation of a Simulation Profile later, the project itself was not initialized with the full PSpice simulation configuration, so some simulation-related UI options remain unavailable.

which components do you see as disabled?

PSpice Special Components: Print1, Print2 and PRINTDGTLCHG

AyushD — Tue, 07 Jul 2026 16:41:44 GMT

Print1:

Use this component to insert .PRINT command in your simulation. This component enables you to print voltage at node in simulation output (.out) file.

You need to configure one or more parameters on this symbol instances from following list to use in simulation flow.

Analysis Type: Assign any value to one of the variables AC/DC/TRAN, depending upon the analysis you are performing. For example if your simulation profile is configured for Transient Analysis you should set TRAN property value as 1.
Functions: You can use following special function on output nodes
- DB
- PHASE
- REAL
- MAG
- IMAG
You can use one or more of the parameters at a time. To select these you need to assign any value to these parameter, say, 1. For example, if you have set DB and PHASE values to 1 on symbol instance and this component is connected to node VOUT, it will print following in output file:
DB of Voltage at VOUT node
PHASE of Voltage at VOUT node

Print2:

PRINT2 performs the same function as PRINT1, only difference being this component should be used for differential voltage between two nodes.

PRINTDGTLCHG:

Use this component for digital nodes. It lists every change of state for a given node in the output file. You need not specify any parameter on this symbol instance.

使用 PSpice-for-TI时，显示这个芯片没有在已配置的库中找到，我尝试在Simulation Settings中配置，

WZ202606154651 — Mon, 15 Jun 2026 14:22:10 GMT

使用 PSpice-for-TI时，我在我自己创建的例程中使用LMR33630ADDA_TRANS等芯片时，会出现一个警告，显示这个芯片没有在已配置的库中找到，我尝试在Simulation Settings中配置，并没有什么用，并且仿真结果异常

RE: 使用 PSpice-for-TI时，显示这个芯片没有在已配置的库中找到，我尝试在Simulation Settings中配置，

IshaS — Wed, 17 Jun 2026 10:35:54 GMT

Can you try this:

配置仿真设置

在 PSpice 设计界面中，点击顶部菜单栏的 PSpice > Edit Simulation Profile。
点击顶部的 Configuration Files 标签页。
在左侧面板中选择 Category > Library。

RE: Exporting PSPICE netlist with Subckt parameters

oldmouldy — Thu, 04 Jun 2026 16:01:38 GMT

I have the same settings and using 25.1.s030. It doesn't look like I can attach an archived project to try.

Exporting PSPICE netlist with Subckt parameters

SC202412036016 — Wed, 03 Jun 2026 20:44:16 GMT

I am trying to export a PSPICE netlist of a simple subcircuit where I have to pass in parameters, however parameter definition is happening after ENDS, instead of the top line where the subcircuit is being defined. There is a .PARAMS in the subckt line however the actual parameter (lval) is showing up right at the end. Any ideas on where the issues may be?

I cannot seem to attach a screenshot of the template settings, but if this works for anyone would be great if you can send a screenshot of the template settings where the ParamList is displayed at the top.

1. To extract the netlist I go to Tools > Create Netlist

2. Here is the output:

* source BLOCK_AOL
.SUBCKT Aol_Block InN InP OutN OutP PARAMS :
G_G1 OUTP OUTN INP INN -1u
L_L1 N00976 OUTN {LVAL} TC=0,0
R_R2 N00976 OUTP 1M TC=0,0
.ENDS Aol_Block
.PARAM lval=1n

RE: Exporting PSPICE netlist with Subckt parameters

SC202412036016 — Thu, 04 Jun 2026 14:39:57 GMT

Hi - I do have that checked and so it does export the netlist, however the issue is that the PARAMS list on the subcircuit line is blank and instead the parameters are placed on the last line after the .END statement. Unfortunately I cannot seem to upload screenshots of my Create Netlist settings so will describe it here.

On the PSPICE tab, the following are checked:

Create Hierarchical Format Netlist

Create SubCircuit Format Netlist >> Descend

Compatibility Mode (16.2 and Prior Releases)

I then click on Settings. In the Hierarchical PSPICE Netlist Settings this is what I have :

Sub-circuit Call: X_<RefDes> <PinList> <SubcktName> PARAMS : <ParamList>

ParamList Element Definition: <Param> = <Value>

Sub-Circuit Header: .SUBCKT <SubcktName> <PinList> PARAMS : <ParamList>

ParamList Element Definition: <Param> = <Value>

Param Usage Reference: {Param>}

Sub-circuit Ends: .ENDS <SubcktName>

If one of you is able to actually get the parameter values exported on the sub-circuit line, please let me know if your settings are different from what I have above.

Thanks.

RE: Exporting PSPICE netlist with Subckt parameters

oldmouldy — Thu, 04 Jun 2026 13:29:36 GMT

Try the following: Select the DSN file entry in the Project Manager pane. Then Tools>Create Netlist, PSpice tab, enable Create SubCircuit Format Netlist and left-click>OK

RE: Exporting PSPICE netlist with Subckt parameters

IshaS — Thu, 04 Jun 2026 06:29:36 GMT

Hi SC202412036016

Can you please try:

* source BLOCK_AOL
.SUBCKT Aol_Block InN InP OutN OutP PARAMS: LVAL=1u
G_G1 OUTP OUTN INP INN -1u
L_L1 N00976 OUTN {LVAL} TC=0,0
R_R2 N00976 OUTP 1M TC=0,0
.ENDS Aol_Block
.PARAM lval=1n

Share your insights how it goes at your end.

Persistent netlisting error

AG202606016357 — Mon, 01 Jun 2026 12:07:33 GMT

Hello,

I'm using "PSpice for TI" to simulate a DCDC converter implementing a specific TI PWM controller (hence the selection of the simulation tool).

My schematic is drawn and seems correct. Still, when I launch the netlist generation, I get the following error message:

"ERROR(ORCAP-15065): There are netlisting errors.

Check the session log."

In the session log, I find:

"INFO(ORNET-1041): Writing PSpice Flat Netlist \\xxx\yyy\SCHEMATIC1\SCHEMATIC1.net
INFO(ORNET-1169): Unable to open the property mapping file: devparam.txt. To resolve this problem, ensure that PSpice.ini exists at the correct location. After that check Library Path in simulation settings contains <installation-path>/tools/pspice/library path and then create the netlist again.
INFO(ORNET-1162): Unable to create design property file"

I completed the proposed checks and everything is OK.

I gave a try with a very simple schematic (1 DC source, 1 ideal R and 1 ideal C). I got the exact same error.

How can I solve this error?

What should I do?

Thanks for helping me.