NETLIST, LINKING AND PARTITIONING ERRORS
Overview
Before any simulation can start, the design has to be turned into something the simulator can run. That happens in three stages: the netlist is compiled from the schematic, models are linked to the parts in it, and the result is divided into partitions. Each stage reports its problems under its own window title, so the title on the log tells you which of the three sections below to read.
Netlisting Errors
Netlisting errors occur when the schematic module cannot create a netlist from the schematic, and they are reported under the title NETLIST COMPILER ERRORS. You will encounter the same errors if you try to export the schematic to ARES for PCB layout. Common causes are:
- Having two components with the same name, or unnamed components, for example two resistors both labelled R?
- Badly formed script blocks such as MAP ON tables. Refer to the script syntax definitions in the schematic manual if you cannot spot the problem immediately.
The messages the compiler produces are listed below.
Linking Errors
Model linking is the process by which model files are called up for the components that are modelled by equivalent circuits, and its problems are reported under the title NETLIST LINKER ERRORS. By far the most common of them is a model file that cannot be found:
Cannot find model file '<file>'.
The model file is looked for in the design's own folder first, and then in each of the folders listed under System > System Settings in the field User Simulation Model and Module Folders. That field takes a list of folders, so a model kept in a location of your own is found by adding that location to the list rather than by moving the file.
Watch also for the warning Used cached model '<file>'.. Models are cached once read, and this warning tells you that the copy in use came from the cache rather than from disk. It is the usual explanation for an edit to a model file that appears to have had no effect.
Parameter Mapping Tables
A single model is often written to cover a family of devices, with a parameter mapping table supplying the values that differ from one device to the next. Where the part you have used is not listed in that table, the linker reports:
Value '<value>' of <property> not found in parameter mapping table of sheet '<sheet>'.
The message names the value that was not matched, the property whose value was used to select the row, and the sheet whose table was searched, which between them is usually enough to identify the missing row.
There are two ways to fix it. Add a row for the device you are using, or add a row whose selector value is DEFAULT. A DEFAULT row is used whenever the selector value matches nothing else, and it suppresses the error entirely. That is the right choice for a model that should tolerate device types it has never heard of.
Many of the parts supplied with Proteus are modelled by library models rather than by model files on disk, and an operational amplifier is the usual example: OA_MOS, OA_FET, OA_MFET and OA_IDEAL are all entries inside the compiled model libraries in the Models folder. A library model is not a text file and cannot be opened in an editor, so the way to find out what a given model covers is the model's own help, reached by selecting the part and pressing CTRL+H.
Pins That Are Not Modelled
Two warnings cover the case where the body of the part has a pin that the model behind it does not:
- Pin '<pin>' is not modelled. means the model simply does not implement that pin.
- Pin '<pin>' does not exist in child module. means the part is modelled by a child sheet, and that sheet has no terminal of that name.
Both are warnings rather than errors, and both are often perfectly harmless. Most operational amplifier models do not model the offset null pins, for instance. They can equally be a mistake, though, and if a new model does not work these are a common cause, especially when there are also No DC path to ground warnings.
A related warning, Missing interface model '<name>' in <part>., means the model named by the part's interface model property could not be found. See Mixed Mode Interface Models.
Partitioning Errors
Partitioning is the mechanism by which the design is divided into the parts of the circuit that need to be simulated, and its problems are reported under the title PARTITION ANALYSER ERRORS. The two you are most likely to meet are these.
Cyclic Dependencies
Cyclic dependencies detected - check tape placement!
An arrangement of tapes is such that the partitions behind and in front of a tape are mutually dependent, so neither can be simulated first. Assuming that you have correctly set any Isolate Before and Isolate After flags on probes and generators, the simplest action is to delete the tape objects and simulate the whole circuit in one go.
The same class of tape problem also produces Read/Write conflict on partition <file> - check tapes., where one partition file is being written and read in the same run.
No Model Specified
No model specified for <part>.
The component indicated has neither a PRIMITIVE nor a MODFILE property, and it has appeared in the part of the circuit that needs to be simulated. If the device is genuinely irrelevant to the simulation, a connector for example, tick Exclude from Simulation on its Edit Component dialogue form. Otherwise you need a model.
Older designs achieve the same thing with a PRIMITIVE=NULL property. That form is still accepted when a design is loaded, and it is converted to the same internal setting that the checkbox controls, so there is no need to change existing designs.
Other Partitioner Messages
| Message | What it means |
| Nothing to simulate! | The partitioner found no circuit to run. Usually the design holds no probes or graphs to define what is wanted, or everything in it has been excluded from simulation. |
| Partition <n> contains no physical components. | A partition was formed but holds nothing that can be simulated. |
| <n> partitions exceeds limit of <n>. | The arrangement of tapes has divided the circuit into more partitions than the partitioner supports. Remove some of the tapes. |
| Probe '<probe>' is on both analogue and digital traces - please use two probes. | A single probe has been added to both an analogue and a digital graph. Place a second probe and use one on each. |
| Play file '<file>' not found for tape '<tape>'. | A tape set to play back a partition file names a file that does not exist. See Tapes and Partitioning. |
| Link to '<name>' not found in '<part>'. | A part refers to another part that is not present in the design. |
| Mutual inductor '<name>' not found in '<part>'. | A coupled inductor names a partner inductor that does not exist. |
See Types of Simulator Model for more information about simulator model types.
Power Rail Configuration Errors
All power nets in the design must be bound to a power supply, either on the schematic or through the Power Rail Configuration dialogue form. If one or more power nets are unbound, an appropriate error is reported in the simulation log:
No power supply specified for net <net> in Power Rail Configuration.
The net name in the message is a link, so clicking it takes you to the offending net on the schematic.
Note that a net is defined as a power net in the following circumstances:
- Any net that is wired to a power terminal is deemed to be a power net.
- Any device with hidden power pins will create power nets with the same names as the pins. For example, a 74LS00 will create power nets VCC and GND.
Note also that connecting a battery or SPICE voltage source to a power net is not sufficient to prevent this error. You must define a power supply and bind the net to it in the Power Rail Configuration dialogue form.
A second and more confusing failure arises when two separate power rails turn out to be wired together, which makes both bindings meaningless:
Power rails '<rail>' and '<rail>' are interconnected in net <net>.
This usually means a wire or a label has joined two supplies that were meant to stay apart, so follow the net link in the message and look at what the net actually connects.
See Also: