GENERATING A NETLIST FILE

Introduction

The Netlist Compiler command presents the Netlist Compiler dialogue form. If you have set Output to File(s), a file selector then follows, from which you choose a filename for the netlist. In most cases, the default settings will suffice; they cause a flat, physical netlist to be generated in SDF format for the current module and displayed in the pop-up text viewer. The functions of the various controls are as follows:

Output

Viewer, the default, sends the netlist to the pop-up text viewer. Nothing is written to disk, which makes this the quickest way to look at the connectivity that your schematic has produced. Once the viewer has been closed you can recall the netlist with the Text Viewer command on the View menu.

File(s) writes the netlist to disk instead. A file selector opens, pre-filled with the file extension that belongs to the selected format, and some formats write more than one file.

Format

A variety of netlist formats can be generated. SDF is the Labcenter native format; the others are used for interfacing to third party software. Notes on each one are provided in Netlist Formats. Third party software is subject to changes beyond our control, so where a package needs more detailed handling we publish an application note rather than describe it here; contact Labcenter technical support if you need one.

Logical/Physical

A logical netlist contains pin names whereas a physical netlist contains pin numbers. A more subtle effect is that in a physical netlist, the elements of multi-element parts such as the 7400 will be grouped (appearing, for example, as U1) whereas in a logical netlist they are kept separate (appearing, for example, as U1:A, U1:B, U1:C, U1:D). A logical netlist will generally be used for simulation whilst a physical netlist is best suited to PCB design. Physical is the default.

Scope

Three scopes are available. Current Module, the default, restricts the netlist generator to the module that is loaded. Current Board covers every sheet belonging to the current board, which is the setting to use in a multi-board project when you want one board's netlist rather than the whole project's. Whole Design covers every sheet in the design.

Current Module is generally used when you wish to extract the netlist from a child sheet, perhaps a daughter card which is to be represented as a layout in the PCB module, but which is part of a larger design that needs to be simulated whole. It is also possible to create a 'virtual test jig' by having a parent sheet which contains circuitry to simulate the components on the child sheet.

Depth

Flatten, the default, replaces objects that have sub-sheets with their implementation. Select This Level instead and that replacement will not occur, so objects with sub-sheets appear as-is in the partslist and netlist.

The most common reason for not flattening a design is if some components have attached child sheets representing their simulator models, but you wish to produce a purely physical netlist for PCB design. Note that if you wish to use this approach, you cannot have a hierarchical design as well: Proteus does not cater for selective flattening. However, with VSM, this is not an issue since you can easily link external model files to the design proper, using MODFILE properties. See the VSM manual for further details.

Errors

Various kinds of error can occur whilst a netlist is being generated. If any errors do occur, they will be displayed in the pop-up text viewer window.

Common errors include:

  • Having more than one component with the same name. Each component on the schematic must have a unique reference designator.
  • Conflicting property assignments on different elements of a multi-element part, for example U1:A specifies a DIL14 package but U1:B specifies an SO14.
  • Failure to connect power nets to a power supply. This usually arises because you have components on the schematic that have hidden power pins, and you have not specified which power supply rail they should connect to. You should use the Power Rail Configuration dialogue form to resolve this error.

See Also:

Netlist Formats

Power Rail Configuration