Search In: Doc:Documentation: Altium CircuitStudio
Altium DesignerAltium 365Altium MCAD CoDesignerAltium On-Prem Enterprise ServerAltium CircuitMakerCompany DashboardAltium Infrastructure Server
Close
搜索 Search on Documentation
Documentation CircuitStudio Documentation ... WorkspaceManager Dialogs

Project Options - Error Reporting

Created: 十二月 16, 2024 | Updated: 八月 11, 2018
Other Related Resources
Project Options - Connection Matrix

Parent page: WorkspaceManager Dialogs

The Error Reporting tab of the Options for PCB Project dialog

Summary

This tab of the Options for PCB Project dialog provides controls to define the reporting levels for each of the possible electrical and drafting violations that can exist on source schematic documents when compiling the project. When the project is compiled, these violation settings will be used - in conjunction with the defined Connection Matrix - to test the source documents for violations.

Any violations that are found and have a report level of Warning, Error or Fatal Error will be displayed as violation messages in the Messages panel. In addition, if compiler errors and warnings are enabled for display on the schematic (enabled on the Schematic - Compiler page of the Preferences dialog), an offending object will display a colored squiggle beneath it.

The process of compiling is integral to producing a valid netlist for a project. In fact, it is the process of compilation that yields the unified data model of a design – the single model of the data that is accessible across the design domains in CircuitStudio's unified design environment. Carefully check and resolve all reported errors prior to netlist generation.
For a comprehensive reference describing each of the possible electrical and drafting violations that can exist on source documents when compiling a project, refer to the Project Compiler Violations Reference.
When working with an Integrated Library project (*.LibPkg), the Error Reporting tab is part of the Options for Integrated Library dialog - a variation of the dialog described here. Only those violation types pertinent to compilation of this project type will be listed.

Access

This is one of multiple tabs available when configuring the options for a project – accessed from within the Options for PCB Project dialog. This dialog is accessed by:

  • Clicking Project | Content | from the main menus in the Schematic Editor or the PCB Editor.
  • Right-clicking on the entry for the project itself in the Projects panel then choosing Project Options from the context menu.
Only the second method of access can be used for an Integrated Library project.

Options/Controls

Violations List

This list presents all possible electrical and drafting violations that can exist on the source documents of the project. Violations themselves are gathered into the following categories:

Each specific violation type is presented with the following fields:

  • Violation Type Description - a short description of the type of violation (or conversely, what it is that is being checked).
  • Report Mode - use this field to specify the severity-level associated with violating the check. Use the drop-down to choose from the following reporting levels:

Right-Click Menu

The following commands are available from the right-click context menu for the tab:

  • All Off - set the Report Mode for all violation types to No Report.
  • All Warning - set the Report Mode for all violation types to Warning.
  • All Error - set the Report Mode for all violation types to Error.
  • All Fatal - set the Report Mode for all violation types to Fatal.
  • Selected Off - set the Report Mode for all selected violation types to No Report.
  • Selected To Warning - set the Report Mode for all selected violation types to Warning.
  • Selected To Error - set the Report Mode for all selected violation types to Error.
  • Selected To Fatal - set the Report Mode for all selected violation types to Fatal.
  • Default - set the Report Mode for all violation types back to their default settings.
Multiple violation types can be selected using standard multi-select techniques (Ctrl+click, Shift+click).

Additional Options

  • Report Suppressed Violations in Messages Panel - enable this option to display violations in the Messages panel even if they have been suppressed through use of No ERC directives.
  • Set To Installation Defaults - click this button to return the Report Mode entries for all violation types to their default settings.

Notes

  1. Use the Connection Matrix tab of the Options for PCB Project dialog to specify reporting levels associated with electrical violations concerning pins, ports and sheet entries, specifically.
  2. There may be points in the design that you know will be flagged as electrical violations that you do not want to be flagged. To suppress these, place a No ERC schematic design directive object at each point.
  3. Generally, it is better to first compile the design and examine the warnings with the default settings. For those warnings that are not an issue for the current design, the reporting level can be changed.

  4. One option of interest is Nets with only one pin. This can be used to detect single node nets where a pin has been connected to a Port, for example, but does not connect to another pin. This is set to No Report by default and can be changed to Warning to help detect broken nets.

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Content