You are here

Troubleshooting OrCAD Capture PSPice Simulation Flow Errors ( errhelp )





ORCAP-1028

ORCOMMN-2302

ORCAP–1030

ORCAP–1031

ORNET–1017

ORNET–1119

ORPSIM–15108

ORPSIM–15113

ORPSIM–15141

ORPSIM–15142

ORPSIM–15143

ORPROBE–3024

ORPROBE–3086

ORPROBE–3121

ORPROBE–3240

OORPROBE–3152


ORCAP-1028 and ORCOMMN-2302

ERROR (ORCAP-1028): The PSpice COM Wrapper error has occurred

ERROR (ORCOMMN-2302): Cannot initialize profile

Description

Upon opening a PSpice enabled design or running simulation, Capture calls PSpice internally; if the COM function is not acknowledgement within a finite time, it leads to the COM Wrapper error. Usually this error is followed by Server Busy error and Cannot initialize profile error messages.

image

image

image

Troubleshooting

This error can be machine specific (appearing for all the designs) or design specific (appearing only for a particular design).In order to determine if the problem is machine specific or design specific , open any sample project from the <CDS_INSTALL_DIR>\tools\pspice\capture_samples folder and run simulation. If COM Wrapper error is encountered, problem is machine specific.

Case 1: Machine specific

Try the following steps one by one and check after each step if problem is resolved:

  1. Choose File — Exit to close Capture and PSpice (if running).

  2. Open Windows Task manager (Pressing CTRL + ALT + DELETE and select Task manager). In the Windows Task Manager dialog box, select the Processes tab. Click the Image Name column to sort the processes alphabetically. Kill the following processes in Task Manager:

    • capture.exe

    • cdsMsgServer.exe

    • cdsNameServer.exe

    • MrkSrvr.exe

    • pspice.exe

    • pspiceexplorersrvr.exe

    • simmgr.exe

    • simsrvr.exe

  3. Invoke Capture. Choose View — Toolbar — Command Window and type the following in the command window:

    DboTclHelper_ReRegisterOrCADPlugins

For SPB/Orcad 16.2 and earlier releases, please unzip attached batch file pspice.zip and save at the location <CDS_INSTALL_DIR>\tools\pspice .Double clicking the batch file registers the required dlls and exes.

Case 2: Design specific

  1. Open the design for which error occurs in Capture.

  2. Highlight the dsn in project manager and choose File Save As. Save it to a location different than the existing project folder location.

  3. Now choose File — Open — Design and open the saved dsn file. The following Select Project Type dialog box will open:

    image

    Select Analog or Mixed A/D option and click OK.

  4. Choose PSpice — New Simulation Profile .Specify the name and in Inherit From click the Browse button highlighted below

    image

  5. Browse to the location where the sim profile exists for the original design. It is the <project folder>\(design name-PSpiceFiles)\(design name)\.sim file.

    For example: D:\my_design\example\example- PSpiceFiles\example\tran.sim

  6. Click Create. Now run simulation on this design.

TOC


ORCAP–1030 and ORCAP-1031

ORCAP–1030

The installation did not complete successfully. Cannot proceed. To rectify this error, close AMS..., run the following command by using the Start - Run menu option from the taskbar and restart the AMS...:<installed path>\\tools\\bin\\Pspiceexplorersrvr.exe /regserver

ORCAP -1031

The OrCAD installation did not complete successfully. Cannot proceed. To rectify this error, close Capture, run the following command by using the Start - Run menu option from the taskbar and restart Capture:<installed path>\\tools\\bin\\Pspiceexplorersrvr.exe /regserver

Description

This error message is encountered when a new PSpice project is created or an existing PSpice project is opened in Capture and appears because of incomplete installation.

Example

image

Troubleshooting

In order to resolve the issue follow below mentioned steps one by one:

  1. Choose File — Exit to close Capture CIS and PSpice (if running).

  2. Open Windows Task manager (Pressing CTRL + ALT + DELETE and select Task manager). In the Windows Task Manager dialog box, select the Processes tab. Click the Image Name column to sort the processes alphabetically. Kill the following processes in Task Manager:

    • capture.exe

    • cdsMsgServer.exe

    • cdsNameServer.exe

    • MrkSrvr.exe

    • pspice.exe

    • pspiceexplorersrvr.exe

    • simmgr.exe

    • simsrvr.exe

  3. Invoke Capture. Choose View — Toolbar — Command Window and type:

    DboTclHelper_ReRegisterOrCADPlugins

    Note: This step is applicable only for SPB 16.3 or later releases.For SPB/Orcad 16.2 and earlier releases, please unzip attached batch file pspice.zip and save at the location <CDS_INSTALL_DIR>\tools\pspice .Double clicking the batch file registers the required dlls and exes

    Now invoke Capture and try opening the PSpice project.

TOC


ORNET–1017

Unconnected pin, no FLOAT property or FLOAT

Description

This error message appears when you create a PSpice netlist for a design that contains unconnected pin and does not have the FLOAT property or FLOAT = e set in the User Properties dialog box. To resolve this error, make sure that you specify FLOAT = e or FLOAT = u (unmodeled) in the User Properties dialog box.

Example

ERROR (ORNET-1017): Unconnected pin, no FLOAT property or FLOAT = e R1 pin '1'

Troubleshooting

Check the pin1 of component R1.Either connect it to some node or specify FLOAT as pin property. FLOAT can have one of the following values:

  • Error

    The pin will not netlist. An error message will be returned when the PSpice simulation netlist is generated. Use Error when you want to be reminded that this pin is a "no connect" and should be treated in a special way. Error is the default value.

  • RtoGND

    The pin is connected to a virtual resistor, whose opposite pin is tied to GND. The resistor has a value of /GMIN. This value allows the simulation netlist to be

    created and allows PSpice to perform the analysis. The virtual resistor will not be processed as part of a layout netlist or appear in a BOM.

  • UniqueNet

    The pin, when left unconnected, is attached to a unique node when the PSpice simulation netlist is generated. Use UniqueNet when you want the pin to remain unconnected but correspond to the Probe data associated with its part.

  • Unmodeled

    This pin will not be considered in netlist .Unmodeled is used when the number of pins on a symbol are more than the number of pins on the model. Extra pins can be assigned unmodeled value. In case the same number of pins are present on the symbol and the model, the PSpiceTemplate property needs to be modified to remove corresponding pin.

    The FLOAT property can either be defined in the part editor when creating a new part, or you can edit a pin on an existing part using the property editor.

TOC


ORNET–1119

No PSpiceTemplate for %s, ignoring

Description

This warning message that appears when you create a PSpice netlist for a design that contains component(s) without PSpiceTemplate property.

Example

WARNING (ORNET-1119): No PSpiceTemplate for C7, ignoring INFO (ORNET-1156): PSpice netlist generation complete

Troubleshooting

Check the PSpiceTemplate property of the component listed in the error message by selecting the component in Capture and the choosing Edit Properties from the right-click menu. The PSpiceTemplate property should be present and there should not be any space in the property name.

Case 1: Component has been placed from the location

<CDS_INSTALL_DIR>\tools\capture\library

Instead of

<CDS_INSTALL_DIR>\tools\capture\library\pspice

For PSpice simulation place the components from the pspice folder as they are PSpice enabled.

Case 2: Component is an advanced analysis enabled part placed from location <CDS_INSTALL_DIR>\tools\capture\library\pspice\advanls

This problem may come due to incomplete installation. The Advanced Analysis parts do not have the PSpiceTemplate property. The PSpice netlister refers to different files in the <CDS_INSTALL_DIR>\tools\pspice\library folder for a successful net list generation. If any of the files is missing, the net list operation will lead to the Warning ORNET - 1119. Check for the following files in the <CDS_INSTALL_DIR>\tools\pspice\library folder

  • nom_aa.lib

  • templates.lib o templates.prp

If any of the above files are missing, copy the same from an existing working installation or ask customer support to provide you with the files.

Additionally, check the following:

  1. In Capture, choose PSpice — Edit Simulation Profile Select the Configuration Files tab and then select Library.

  2. Check if nom.lib is added in the Configured Files list. If it is not present,, click the Browse button and add nom.lib from the following location :

    < CDS_INSTALL_DIR >\tools\pspice\library\nom.lib

    Click Add as Global.

  3. Check that Library Path is pointing to < CDS_INSTALL_DIR

>\tools\pspice\library

In case not then manually add the library path and click OK. This should resolve the error.

Case 3: Component is created manually for vendor model

The PSpiceTemplate property should be present and there should not be any space in the property name.

TOC


ORPSIM–15108

Subcircuit %s used by %s is undefined

Description

This error message appears when PSpice is not able to find the subcircuit model definition in its search path.

Example

ERROR (ORPSIM-15108): Subcircuit POLYCAP used by X_U3 is undefined Circuit has errors ... run aborted

See output file for details

INFO (ORPROBE-3188): Simulation aborted

Troubleshooting

This error message appears when PSpice is not able to find the subcircuit model definition in its search path. Model definition for Cadence installation libraries is defined in nom.lib and for custom libraries user needs to define it manually.

  1. For Cadence installation libraries:

    In Capture, choose PSpice Edit Simulation Profile. Select the Configuration Files tab and then select Library. Check if nom.lib exists in the configured files section. In case not, click Browse for Filename and go to the location < CDS_INSTALL_DIR >\tools\pspice\library\nom.lib. Click Add as Global and then OK.

    Error should be resolved

  2. For user defined vendor models

In Capture, choose PSpice — Edit Simulation Profile Select the Configuration Files tab and then select Library. Browse to the location where the model is saved and click either Add to Design or Add to Profile Click OK

Error should be resolved

TOC


ORPSIM–15113

Model %s used by %s is undefined

Description

This error message appears when PSpice is not able to find the model definition in its search path.

Example

ERROR (ORPSIM-15113): Model Q40238 used by Q_Q1 is undefined Circuit has errors ... run aborted

See output file for details

INFO (ORPROBE-3188): Simulation aborted

Troubleshooting

This error message appears when PSpice is not able to find the model definition in its search path. Model definition for Cadence installation libraries is defined in nom.lib and for custom libraries user needs to define it manually.

  1. For Cadence installation libraries:

    In Capture, choose PSpice Edit Simulation Profile. Select the Configuration Files tab and then select Library. Check if nom.lib exists in the configured files section. In case not, click Browse for Filename and go to the location < CDS_INSTALL_DIR >\tools\pspice\library\nom.lib. Click Add as Global and then OK.

    .

  2. For user defined/vendor models

In Capture, choose PSpice — Edit Simulation Profile Select the Configuration Files tab and then select Library Browse to the location where the model is saved and click either Add to Design or Add to Profile Click OK

Error should be resolved

This error can also occur if model is defined as subckt whereas the corresponding capture part has PSpiceTemplate property beginning with Q (or any other device type) rather than X.

For example, PSpiceTemplate property has the value for a subckt model:

Q^@REFDES %c %b %e @MODEL

Replace Q with X to match the subckt model statement.

X^@REFDES %c %b %e @MODEL

This is the correct PSpiceTemplate value.

TOC


ORPSIM–15141 and ORPSIM–15142

ERROR (ORPSIM-15141): Less than 2 connections at node %s ERROR (ORPSIM-15142): Node %s is floating

Description

This error message appears when any node in the circuit does not have complete conducting path.

Example

ERROR (ORPSIM-15141): Less than 2 connections at node N00745 ERROR (ORPSIM-15142): Node N00081 is floating

Troubleshooting

Check in schematic the node listed in error message .For example, for the above message it is N00745.If it is left unconnected by mistake, complete the connections. In case it is intentionally left unconnected to determine open circuit voltage, add the Float property with the value RtoGnd to the component pin connected to the node. This will insert a E12 resistor connected to Ground.

Other cases in which this error can occur are:

  1. Component pin connected to node has value FLOAT = Uniquenet and node is left unconnected.

  2. Circuit does not has Ground . The only valid ground in a PSpice simulation is ground . Either edit the ground symbol and change the name from GND to 0 or choose Place Ground, ensure that the source.olb library is configured from

    <CDS_INSTALL_DIR>\tools\Capture\Library\PSpice\Source.olb', which contains the 0 source.

  3. Circuit has non PSpice parts. Check the parts connecting the node listed in error message. Select the part, double-click to open property editor, and check if PSpiceTemplate property exists. If you are using Cadence parts, make sure that you are accessing from the following folder:

<CDS_INSTALL_DIR>\tools\capture\library\pspice

TOC


ORPSIM–15143

Voltage source and/or inductor loop involving %s. You may break the loop by adding a series resistance

Description

This error message appears when two different sources are connected to the same net or there is an inductor in parallel with a voltage or current source. During the initial DC Bias Point calculation, inductors are shorted causing the shorting of the sources. Adding a small resistor in series with the inductor or the source will resolve the voltage loop error. This error message can also appear for digital or mixed designs when custom digital power supply node values are set equal to default power supply node values.

Example

ERROR (ORPSIM-15143): Voltage source and/or inductor loop involving V_V2. You may break the loop by adding a series resistance

Circuit has errors ... run aborted See output file for details

INFO (ORPROBE-3188): Simulation aborted

Troubleshooting

Case 1: When analog power supply is used

Check the nodes for voltage source mentioned in the error message. In the above mentioned message, for example, it is V2. Add a OHM or smaller resistor in series with V2 to resolve the error.

Case 2: When custom digital power supply is used

ERROR (ORPSIM-15143): Voltage source and/or inductor loop involving X$CD4000_PWR.VVSS. You may break the loop by adding a series resistance

Change the CD4000_PWR power supply pin properties as follows:

PSPICEDEFAULTNET = MY_VDD PSPICEDEFAULTNET = MY_VSS

Select the CD4000 part in the schematic to which the new power supply should apply, and then change the appropriate pin properties as follows:

PSPICEDEFAULTNET = MY_VDD PSPICEDEFAULTNET = MY_VSS

Note: For more information on using custom digital power supplies please refer the section Creating custom digital power supplies page 659 onwards of PSpice User Guide available at location <CDS_INSTALL_DIR

>\doc\pspug\pspug.pdf

TOC


ORPROBE–3024

Out of Memory error

Description

The error appears while displaying traces or loading large dat files having size of few GBs.Problem occurs due to the large number of data structures being created internally for handling all the sections in one go. The problem starts occurring when pspice.exe memory hits the .6GB size limit.

Example

Out of Memory error

Troubleshooting

Pspice data file with more than 1 million data points per trace (usually data files with size greater than 2GB) is considered as large data file .Typically, this problem occurs when waveforms are displayed during the simulation run. It is recommended for longer simulations, or simulations resulting in large DAT file sizes, to turn off the trace display until after the simulation completes. It is often necessary to verify that the simulation data looks correct during the simulation run. This can be done by periodically opening the simulation results in PSpice during the simulation run to verify that the plotted results are close to what is expected. First begin by disabling the trace display during the simulation run as follows:

. In Capture, choose PSpice — Edit Simulation Profile

  1. Select the Probe Window tab.

  2. Under Display Probe Window, select the option after simulation has completed as shown below

    image

    To view the waveforms during the simulation to verify results:

  3. In PSpice, during the simulation, choose View — Simulation Results to see the current simulation trace displays.

  4. After viewing, choose File — Close to close the display.

    NOTE: This does not close the simulation, only the displayed trace display.

You can also try below mentioned steps to reduce dat file size, preventing out of memory error:

  1. In Capture, choose PSpice — Edit Simulation Profile In the Data Collection tab, set the value as At Markers Only for various data collection options and click OK

    image

  2. Reduce Run to time and increase Maximum step size values

    image

  3. In the Start saving data after field, enter a delay time

    image

    image

    This limits file size by suppressing the first part of transient simulation output.

  4. While loading dat file, select the option Use fewer data points to display complete trace .This can also be set in Pspice probe window by choosing Tools - Options and then setting the option in the Large Data File tab.

    image

  5. If you need to select the Use all data points option to display trace in parts option, after opening the .dat file in probe window choose View — Large Data File Mode — Display in parts.

    Now add traces and keep clicking Load next part till the desired section is displayed.

    image

  6. TOC


    ORPROBE–3086

    No simulation data for marker '%s

    Description

    This error message appears when PSpice is not able to recognize voltage, current, or power markers placed on a component pin or net in Capture CIS.

    Example

    ERROR (ORPROBE-3086): No simulation data for marker 'V(out1)' ERROR (ORPROBE-3086): No simulation data for marker '{U1.AB[0:1]}' Troubleshooting

    Check the net listed in the error message

    For example, for the error No simulation data for marker 'V(out1)”, the net is OUT1. Similarly, for the error No simulation data for marker '{U1.AB[0:1]” it is bus AB[0..1] inside the hierarchical block U1.

    This error message appears in following scenarios:

    1. There is a mismatch in PSpice netlist w.r.t schematic. This can happen in case of complex hierarchical design where instance and occurrence level part references are different. Upon choosing PSpice — Run, the netlist is created with occurrence name whereas marker works on the schematic name. Hence, cross probing between Capture and PSpice fails with error ORPROBE-3086.

    2. Marker is placed on a hierarchical port having space in name. Delete the space in Port Name and recreate netlist.

    3. Marker is placed on a bus residing at lower level of a hierarchical design. Error does not occur when bus resides on the same page as the hierarchical block in the root schematic.

    In all the above mentioned scenarios workaround is to choose Trace — Add Trace to view the desired waveform in the PSpice Probe window.

    TOC


    ORPROBE–3121

    No Measurements are defined

    Description

    This error message appears while choosing Trace — Evaluate Measurement when defined measurements in the pspice.prb file are not found.

    Example

    image

    Troubleshooting

    In order to resolve the error try below mentioned steps one by one:

    1. Open the PSpice.ini file from the location

      <CDS_INSTALL_DIR>\tools\pspice\PSpice.ini in a text editor. Make sure that the PSpice.ini file has an entry for PRBFILE in PROBE section as mentioned below

      PRBFILE=<CDS_INSTALL_DIR>\tools\PSpice\Common\pspice.prb

      Then verify that the pspice.prb file exists at the location specified.

    2. In case condition in step 1 is met, check that PSpice.ini file does not have any variables pointed through CDSROOT.

    For example:

    LIBPATH=_CDSROOT_\tools\pspice\Library;D:\cdssites\amsdehdl

    _integration_165\local_model_lib BACKUP=_CDSROOT_\tools\pspice\Backup PRBFILE=_CDSROOT_\tools\pspice\Common\pspice.prb

    If yes, then change them to the actual location of CDSROOT

    For example: CDSROOT= D:\Cadence\SPB165 LIBPATH=D:\Cadence\SPB165\tools\pspice\Library;D:\cdssites\

    amsdehdl_integration_165\local_model_lib BACKUP=D:\Cadence\ SPB165\tools\pspice\Backup PRBFILE=D:\Cadence\ SPB165\tools\pspice\Common\pspice.prb

    Save the PSpice.ini file and then reinvoke Pspice. Environment variables are not supported in Pspice.ini file causing error.

    TOC


    ORPROBE–3240

    Invalid Expression(s)

    Description

    This error message appears during Evaluate Measurement step in PSpice probe window and is caused by violation of defined trace expression rules.

    Example

    image

    Troubleshooting

    Check the syntax of expression listed in error message. Correct syntax is

    Measurement (<trace>)

    Also, it should not have digital, logical, and arithmetic operators improperly mixed up or any illegal character for operator.

    Note: For more information on operators and expressions please refer Trace expressions page 771 onwards of PSpice User Guide available at location

    <CDS_INSTALL_DIR >\doc\pspug\pspug.pdf

    This error can also appear in the following scenarios:

    1. Nested functions are used, that is, the parameter for the function to be evaluated is another function that itself needs to be evaluated. For example:

      YatX(p(v(out)/v(out2)),ZeroCross(db(v(out)/v(out2))))

      PSpice currently does not support nested measurements. It is required to simplify the measurement as:

      ZeroCross(db(v(out)/v(out2))) YatX(p(v(out)/v(out2)),724k)

    2. Parameter is used as an argument in the measurement function Example: YatX(Voltage,{cc})

      Where cc is a global parameter on which parametric sweep has been performed.

      PSpice measurement function currently does not support model or global parameter.

    3. Measurement is done on FFT of waveform. FFT information is not available in

      .DAT file and, hence, measurement should not be performed on FFT.

    4. ** is used as exponentiation operator. Instead use PWR(x,y) operator

    Lres(1,2) = 1/(y2*((2*x1*3.141592654)**2)) INCORRECT

    Lres(1,2) = 1/(y2*(PWR((2*x1*3.141592654),2))) CORRECT

    TOC


    OORPROBE–3152

    Mismatched parenthesis in %s

    Description

    This error message appears during evaluate measurement step in Pspice probe window and is caused if opening parentheses are not equal to closing parentheses.

    Example

    image

    Troubleshooting

    Check the syntax of the expression listed in the error message; ensure that the number of opening and closing parentheses are equal.