PSpice Errors and Solutions

.PROBE and .ALIAS must agree on /CSDF

Either a .PROBE/CSDF and .ALIAS or a .PROBE and .ALIAS/CSDF were entered.

Solution

1. Correct the conflict by specifying /CSDF on both or neither statement.

Invalid device type

The first character of all devices defines what kind of device it is. The first character is not known to be a valid device.

Solution

1. Correct the spelling of the name.

Maximum number of alias nodes exceeded

Too many nodes have alias names associated with them.

Solution

1. Eliminate the aliases for some nodes.

Unable to open index file

The index file could not be created. Either it is open by another program or the system-wide limit on the number of files which can be concurrently open has been exceeded.

Solution

1. If another program has the file open, close that program.

Model type unknown

In a .MODEL statement the model type was probably mistyped.

Solution

1. Make sure that the model type is valid. The valid model types for each device are listed in the Reference Manual section dealing with the device.

Duplicate library entry for <modelname>

The identified model appears in more than one library. Only the first one will be used.

Solution

1. Remove the definition from all the other libraries, or change their names to make them unique.

Out of Memory

Insufficient memory for circuit.

Solution

1. Allocate PSpice more memory:
   • If you are running other programs concurrently with PSpice, close them and try again.
   • Install more memory for your computer.

Unrecognizable command

The first character on a line was a period (.), indicating a command, but the subsequent characters did not define a valid command.

Solution

1. Correct the spelling of the command.

Unable to open stimulus file

The identified file was listed in a STIMULUS device, but could not be found.

Solution

1. Correct the spelling of the file name.

Model references form circular list. For example:

A model with an AKO: references another model with an AKO: which in turn references the first.

Solution

1. Break the loop of AKO: references.

Unable to open probe file

The Probe Data file could not be created. Either it is open by another program or the system-wide limit on the number of files which can be concurrently open has been exceeded.

Solution

1. If another program has the file open, close that program.

Unable to make index for library file

An index file had to be created for a library file. However, the system did not permit it.

Solution

1. An index file will reside in the same directory as the library file. Make sure that you have permission to write to that directory.
2. If the index file already exists, make sure that you have permission to modify it.

Model <modelname> referenced by model <modelname>, is undefined

There was an AKO: reference (.MODEL first_name ... AKO: second_name ...) The second model is not defined in either the circuit file or any of the referenced libraries.

Solution

1. Check for correct spelling of the second model name.
2. If necessary, add the name of the library in which it can be found.

Subcircuit <filename> used by <filename> is undefined

The identified subcircuit is not defined in either the circuit file or any of the referenced libraries.

Solution

1. Check for correct spelling of the model name.
2. If necessary, add the name of the library in which it can be found.

Unable to open library

The specified library could not be found.

Solution

1. Check the spelling of the file name.

Making new index file for library file

The index file associated with the indicated library file is being rebuilt.

This is for your information only, and is not an error. The index file is being rebuilt because it either did not exist or the library file was changed.

Missing model name in library

During the process of building the index file for a library file, a .MODEL statement was encountered which did not have a model name.

Solution

1. Correct the .MODEL statement, using the following basic syntax:
   .MODEL <name> <type> <optional parameters>

Missing model type in library

During the process of building the index file for a library file, a .MODEL statement was encountered which did not have a model type.

Solution

1. Correct the .MODEL statement, using the following basic syntax:
   .MODEL <name> <type> <optional parameters>

Missing subcircuit name

During the process of building the index file for a library file, a .SUBCKT statement was encountered which did not have a name.

Solution

1. Correct the .SUBCKT statement, using the following basic syntax:
   .SUBCKT <name> [<nodes> ...]

|VON - VOFF| too small for VSWITCH model

The ON and OFF voltages specified are too close in value to each other.

Solution

1. Change value to be more reasonable.

RON or ROFF less than or equal to zero for VSWITCH model

Either the ON resistance or OFF resistance is not positive.

Solution

1. All resistances must be positive. Fix the incorrect value.

RON or ROFF greater than 1/GMIN for VSWITCH model

Either the ON resistance or OFF resistance is too large.

Solution

1. All resistances must be less that 1/GMIN. Fix the incorrect value.

RON = ROFF for VSWITCH model

The ON resistance is the same as the OFF resistance.

Solution

1. They must be different to be a meaningful device. Change one of them.

ION - IOFF| too small for ISWITCH model

The ON and OFF currents specified are too close in value to each other.

Solution

1. Change either to be more reasonable.

RON or ROFF less than or equal to zero for ISWITCH model

Either the ON resistance or OFF resistance is not positive.

Solution

1. All resistances must be positive. Fix the incorrect value.

RON or ROFF greater than 1/GMIN for ISWITCH model

Either the ON resistance or OFF resistance is too large.

Solution

1. All resistances must be less that 1/GMIN. Fix the incorrect value.

RON = ROFF for ISWITCH model

The ON resistance is the same as the OFF resistance.

Solution

1. Change one of them. They must be different to be a meaningful device.

<param> not a subcircuit param

One of the optional parameters listed in the PARAMS: section of a subcircuit call is not defined.

Solution

1. Correct the spelling to match those defined by the subcircuit.

Less than 2 connections at node

This node connects to only one device terminal in the circuit or in a subcircuit model. A port may be mislabeled.

Solution

1. Starting with the node indicated in the message, verify the circuit connections.

Node is floating

The voltage of this node cannot be determined. The node or the circuitry containing it may be isolated from power supplies or ground by capacitors, or the node’s connections to power supplies or ground is missing.

Solution

1. Starting with the node indicated in the message, verify the circuit connections.

Invalid radix, expecting BIN (1), OCT (3), or HEX (4)

In a .VECTOR command, the optional RADIX parameter was entered, but its value was not 1, 3, 4, B, O, or H.

Solution

1. Correct the RADIX value.

Unrecognized parameter

In a .VECTOR command, a parameter was entered which was not valid.

Solution

1. Correct the statement.

Tolerances on model <modelname> ignored due to <tolerance>

A model which is the target of a .STEP PARAM or .DC PARAM had tolerances. This is a warning only.

The tolerances are ignored.

MC or .WCASE ignored (No <analysis type> command in circuit)

A .MC command was encountered specifying an analysis which was missing.

Solution

1. Add a .DC, .TRAN, or .AC command as appropriate.

No models had tolerances. .MC or .WCASE ignored

A .MC command was encountered, but none of the models had tolerances specified.

Solution

1. Either add tolerances to one or more models, or remove the .MC command.

The circuit matrix is singular and cannot be solved.

The matrix is singular (has a 0.0 value along the diagonal.)

Solution

1. Check for the following frequent causes:
   • floating nodes
   • a closed path through the circuit which has zero resistance

The circuit matrix is too close to being singular to solve.

The matrix is nearly singular (has value almost 0.0 along the diagonal.)

Solution

1. Check for the following frequent causes:
   • a path to ground which is very high impedance
   • a path with a very large gain

Convergence problem

PSpice could not derive values for the node voltages or device currents that satisfy the convergence criteria used.

Solution

1. Check circuit connections, device model parameters used, expected operating regions of the devices, etc.
2. Set initial conditions, relax the tolerance parameters, use GMIN stepping (for DC convergence problems), etc.

Convergence problem

PSpice could not derive values for the node voltages or device currents that satisfy the convergence criteria used.

Solution

1. Check circuit connections, device model parameters used, expected operating regions of the devices, etc.
2. Set initial conditions, relax the tolerance parameters, use GMIN stepping (for DC convergence problems), etc.

Time step is too small in Transient Analysis at xxx

The simulation must terminate due to the time step needed for convergence becoming too small.

Solution

1. Check for the following possible causes:
   • waveforms with very fast rise/fall times
   • model parameters completely wrong

Missing or invalid expression

An expression was expected, but was either missing or invalid.

Solution

1. Make sure that expressions are enclosed in '{' and '}' characters and that any '(' characters have a matching ')' character.
2. Make sure that continuation lines have a '+' character in the first column.
3. If the netlist was generated by Capture, contact the Customer Support.

Missing expression

An expression was expected, but was either missing or invalid.

Solution

1. Make sure that expressions are enclosed in '{' and '}' characters and that any '(' characters have a matching ')' character.
2. Make sure that continuation lines have a '+' character in the first column.
3. If the netlist was generated by Capture, contact the Customer Support.

Bad radix spec

In a digital stimulus device, the radix specified was not one of the permitted values: 1, 3 or 4.

Solution

1. Correct the radix.

LABEL invalid in REPEAT loop

In a digital stimulus device, a LABEL: appeared in a REPEAT ... ENDREPEAT construct.

Solution

1. Remove the label.

Missing goto label

In a digital stimulus device, a GOTO was encountered but the target label was missing.

Solution

1. Correct the statement.

GOTO invalid in REPEAT loop

In a digital stimulus device, a GOTO appeared in a REPEAT ... ENDREPEAT construct.

Solution

1. Remove the GOTO.

HREPEAT missing FOR or FOREVER

In a digital stimulus device, a REPEAT appeared but one of the two required keywords FOR or FOREVER was missing.

Solution

1. Correct the specification.

Attempt to redefine builtin name

In a .FUNC statement, a reserved macro name such as 'SQRT()' was being redefined.

Solution

1. Refer to the Reference manual for the list of reserved macro names and avoid redefining them.

Must be D

In a .PRINT/DCTLCHG statement, a request for a voltage or current was indicated.

Solution

1. Make sure only digital nodes are printed with a .PRINT/DGTLCHG statement.

Must be I or V or D

In a .PRINT TRAN statement, only currents, voltages, and digital states can be printed.

Solution

1. Correct the statement.

Must be I or V

In a .PRINT AC or .PRINT DC, only currents and voltages can be printed.

Solution

1. Correct the statement.

Must be V

In a .PRINT NOISE statement, only voltages can be printed.

Solution

1. Correct the statement.

Must be I or V, D not allowed

In a .PRINT AC or .PRINT DC, only currents and voltages can be printed.

Solution

1. Correct the statement.

Expression not allowed here

In a PLSYN device, a TESTVECTOR parameter was specified as a {parameter}.

Solution

1. Change the {parameter} to a literal constant.

Unknown parameter

In a RAM, ROM or PLD device, an unknown parameter was entered.

Solution

1. Check the spelling of all parameters and correct as necessary.

Probability must not be less than 0.

In a .DISTRIBUTION statement a probability was less than 0.

Solution

1. Make sure all probabilities are between 0 and 1 inclusive.

At least two pairs of numbers necessary

In a .DISTRIBUTION statement, at least two (probability, value) pairs must be entered.

Solution

1. Make sure you have at least two pairs.

Please simplify .. distribution too complicated

In a .DISTRIBUTION statement, more than 100 (probability, value) pairs were entered.

Solution

1. Reduce the complexity of the expression.

Use RLGC & LEN for lossy line

A lossy transmission line was specified and a either Z0 or TD parameter was entered.

Solution

1. Remove the Z0 or TD parameter; lossy transmission lines are characterized with the R, L, G, G and LEN parameters.

Use Z0 & TD or F/NL for ideal line

An ideal transmission line was specified and a Lossy parameter was entered.

Solution

1. Remove the Lossy parameter; ideal transmission lines are characterized with the Z0, TD, F and NL parameters.

Z0 or RLGC parameters must be specified

Transmission lines require either Z0 or R, L, G, and C to be set.

Solution

1. Enter a value for Z0 if ideal, or for R, L, G, and C if lossy.

TD or F must be specified

An ideal transmission line was specified, but neither TD nor F was entered.

Solution

1. Enter a value for either TD or F.

BadTransferFunction

An E or G device was entered and LAPLACE was specified for it. The laplace expression was invalid.

Solution

1. Correct the expression.

Missing REPEAT iteration count

In a PWL type Voltage or Current source, the REPEAT iteration count was missing.

Solution

1. Correct the device specification.

Symbols Table overflow

You have too many devices to simulate with the memory available.

Solution

1. Give PSpice more memory:
   • If you are running other programs concurrently with PSpice, close them and try again.
   • Add more memory for your computer.

Voltage Source and/or Inductor Loop Involving xxx

This may be caused by a loop constructed with a combination of voltage sources and/or inductors.

Solution

1. Break the loop by adding a series resistance.

Convergence problem

PSpice could not derive values for the node voltages or device currents that satisfy the convergence criteria used.

Solution

1. Check circuit connections, device model parameters used, expected operating regions of the devices, etc.
2. Set initial conditions, relax the tolerance parameters, use GMIN stepping (for DC convergence problems), etc.

Convergence problem

PSpice could not derive values for the node voltages or device currents that satisfy the convergence criteria used.

Solution

1. Check circuit connections, device model parameters used, expected operating regions of the devices, etc.
2. Set initial conditions, relax the tolerance parameters, use GMIN stepping (for DC convergence problems), etc.

Invalid Outside of .SUBCKT

A .ENDS statement was encountered, but a subcircuit was not being defined.

Solution

1. Remove the .ENDS statement or, if it was intended to mark the end of the circuit, change it to .END.

Library Index File Does Not Have the Correct Format

The index file shown is corrupt.

Solution

1. Delete the index file shown. This will cause it to be rebuilt in the correct format.

Unable to Find Library File

The specified library could not be found.

Solution

1. Check the spelling of the file name.

Library File Has Changed Since Index File Was Created

The specified library file was modified since its index file was last created.

Solution

PSpice will automatically recreate the associated index file.

The Timestamp Changed from xxx to yyy

The specified library file was modified since its index file was last created.

Solution

PSpice will automatically recreate the associated index file.

Model <modelname> Used by <filename> Is Undefined

The identified model is not defined in either the circuit file or any of the referenced libraries.

Solution

1. Make sure the model name is spelled correctly.
2. If necessary, add the name of the library in which it can be found.

Missing param name in library

During the process of building the index file for a library file, a .PARAM statement was encountered which did not have a parameter name.

Solution

1. Correct the .PARAM statement. The basic syntax is:
   .PARAM name = value

There Are No Devices in This Circuit (This Message Will Be Printed)

Multiple circuits may be simulated from a single file. After each .END statement is encountered and the simulation has been completed, PSpice will continue to read the input file for any subsequent circuits. If any data is read but no valid devices exist when the end of file is reached, this message is issued.

Solution

1. Remove blank lines after the last .END statement in the circuit file.

Only one .TEMP value allowed with .STEP

If you have a .STEP command, there may be a .TEMP command specifying only a single temperature.

Solution

1. Remove all but the first temperature listed in the .TEMP statement.

Only one .TEMP, .DC TEMP, or .STEP TEMP permitted

The temperature(s) at which a circuit may be simulated can be set in exactly one of three ways.  Two or more different ways have been specified.

Solution

1. Remove all but one of the .TEMP, .DC TEMP and .STEP TEMP statements.

Unable to open file

In a .INCLUDE ... FILE = ... statement, the specified file name could not be found.

Solution

1. Correct the spelling of the file name.

Missing .ENDS in .SUBCKT

The file ended during the processing of a subcircuit definition before the .ENDS statement was encountered.

Solution

1. Insert a .ENDS statement at the appropriate place in the file.

Name on .ENDS does not match .SUBCKT

A subcircuit was being processed.  The last line of a subcircuit is the .ENDS statement, which may optionally have a name.  This name must be identical to the subcircuit name if it is present.

Solution

1. Remove the offending name from the .ENDS statement.

Invalid device in subcircuit

While processing a subcircuit, an unknown device was encountered.

Solution

1. Correct the spelling of the device name.

Subcircuit <filename> is Undefined

The indicated subcircuit could not be found in the circuit file or any of the libraries.

Solution

1. Check the spelling and correct as required.
2. Add the name of the library in which it is defined to the library list.

Incorrect Number of Interface Nodes for <filename>

The subcircuit was defined with a different number of interface nodes than were listed when an instance was placed.

Solution

1. Make sure that the definition and the reference to the subcircuit have the same number of nodes.

Digital Simulator Option not present

The Digital Simulator Option must be purchased to use this feature.

Solution

1. Contact Cadence to purchase the Digital Simulator Option.

Cannot Open Temporary Digital File

One or more temporary files required by the digital simulator could not be opened.

Solution

1. Increase the FILES= value in the C:\CONFIG.SYS file.
2. If this does not solve the problem, contact Customer Support.

Missing model

A model name was expected on a device statement, but was missing.

Solution

1. Correct the statement.

Missing number of nodes

In a Pin Delay Device (U... PINDLY), the number of nodes parameter was missing.

Solution

1. Correct the statement.

Too few output nodes specified

In a Pin Delay Device (U... PINDLY), the number of output nodes parameter was missing.

Solution

1. Correct the statement.

Bad or missing parameter

In a Digital Stimulus Device (U... STIM ...), one of the required parameters was either invalid or missing entirely.

Solution

1. Correct the statement.

Invalid value

In a Digital Stimulus Device (U... STIM ...), one of the states specified was not 0, 1, R, F, X, or Z.

Solution

1. Correct the state value.

Undefined parameter used in expression

In an expression, a reference was made to a parameter which was neither one of the predefined ones, nor one defined in a .PARAM statement.

Solution

1. Make sure the spelling of all parameters within the expression is correct.

Undefined Parameter: <parameter>

In an expression, a reference was made to this parameter which was neither one of the predefined ones, nor one defined in a .PARAM statement.

Solution

1. Make sure the spelling of all parameters within the expression is correct.

I(node) is not valid

In a .PRINT ... statement, an attempt was made to print a current at a node.

Solution

1. Correct the statement. You can only print currents through a device and voltages at nodes or device pins.

Must be independent source (I or V)

In a .PRINT ... statement, only a voltage source or current source is allowed.

Solution

1. Correct the statement.

Digital node table overflow

There are too many digital nodes to simulate with the memory available.

Solution

1. Allocate more memory to PSpice by doing one of the following:
   • If you are running other programs concurrently with PSpice, close them and try to simulate again.
   • Purchase more memory for your computer.

Missing parameter

A parameter was expected in a .AC or .DC statement, but was missing.

Solution

1. Correct the statement.

Not a valid parameter for model type

A parameter in a .MODEL statement was misspelled.

Solution

1. Correct the spelling.

Must be 'I' or 'V'

In a .DC or .STEP DC, an attempt was made to sweep some device other than a voltage or current source.

Solution

1. Change the device you want swept to a voltage or current source.

Missing node number

In an .IC or .NODESET statement, the node number to be set was not specified.

Solution

1. Correct the statement.

Missing device name

In an .IC or .NODESET statement, the device whose node was to be set was not specified.

Solution

1. Correct the statement.

Analog simulator option not present

The statement requires analog simulator option, but that option is not installed.

Solution

1. Contact Cadence to purchase the analog simulator option.

Invalid parameter

For a device other than a MOSFET or IGBT, a parameter was entered that is specific to these two devices.

Solution

1. Correct the device.

Inductor part of this K device

In a K (Coupling) device, the same Inductor was entered twice.

Solution

1. Delete the second inductor reference.

Inductor part of another core device

The same inductor appears in more than one K (Core) device.

Solution

1. Remove the reference in the second K device.

Transmission line part of this K device

In a K (Coupling) device, the same Transmission Line was entered twice.

Solution

1. Delete the second reference.

Invalid specification

In a voltage source or current source, the transient specification was not EXP, PULSE, PWL, SFFM, or SIN.

Solution

1. Correct the transient specification.

Bad value

A floating point value was expected, but an invalid number was encountered.

Solution

1. See the online PSpice Reference Manual for the format of valid numbers, and correct the statement.

Invalid number

An invalid floating point number was generated in the process of a calculation. The most common cause of this is a .MODEL parameter which is too far out of line.

Solution

1. Check all .MODEL parameters for correct scaling. If the problem persists, contact Customer Support.

No analog devices--DC sweep ignored

The circuit has only digital devices. Digital devices are only simulated in the Transient (time-domain) analysis.

Solution

1. Remove the .DC statement.

No analog devices--small-signal analysis Ignored

The circuit has only digital devices. Digital devices are only simulated in the Transient (time-domain) analysis.

Solution

1. Remove the .AC, .OP, .SENS, .TF or .NOISE statement.

Missing value

An expected value is missing.

Solution

1. Make sure that continuation lines have a + character in the first column.
2. If the netlist was generated by Capture, contact Customer Support.

EOF in subcircuit

During the definition of a subcircuit, an end-of-file condition was encountered. The file is probably corrupt.

Solution

1. Regenerate the file.

Return to top