Testpoint Report Setup

Old Content - visit altium.com/documentation

Modified by Admin on Jan 29, 2015

The two incarnations of the Testpoint Setup Dialog.

Summary

Assembly/Fabrication testpoint reports are configured using this dialog. While the controls of the dialog remain the same, its banner text will change depending on whether it was accessed to configure options for an Assembly, or a Fabrication Testpoint report.

In Altium Designer, a Testpoint is a pad or via that has one or more of the Testpoint Settings options enabled, as shown in the image below. Each testpoint report then type detects pads/vias with the appropriate testpoint type enabled.

Testpoints are assigned manually, or can be detected automatically by running the Tespoint Manager. Or refer to this article to learn more about Altium Designer's Testpoint System.

Access

Testpoint output can be generated in one of two ways:

Using an Assembly or Fabrication Test Point Report output generator in an OutputJob Configuration file (*.OutJob). Output is generated when the configured output generator is run.
Directly from within the active PCB document using the File » Fabrication Outputs » Test Point Report command or the File » Assembly Outputs » Test Point Report command. Output will be generated immediately upon clicking OK in the dialog.

Note : The settings defined in the Testpoint Setup dialog when generating output directly from the PCB are distinct and separate to those defined for the same output type in an Output Job Configuration file. In the case of the former, the settings are stored in the project file, whereas for the latter they are stored in the Output Job Configuration file.

Options/Controls

Report Formats

Text - standard text format
CSV - standard comma separated value format, which can be imported into a spreadsheet application such as Excel for further processing
IPC-D-356A - IPC netlist file which carries blind and buried via information as well as differentiating between through-hole vias and free pads. When imported into a CAM document along with image and drill data, it facilitates the recovery of original net names used in the PCB design, making the PCB easier to understand and manage within the CAM Editor.

Test Point Layers

Allows you to specify a scope for the report:

Top Layer - Check this option to include valid testpoints assigned on the top of the board
Bottom Layer - Check this option to include valid testpoints assigned on the bottom of the board

Units

Inches - Check this option to output coordinates in inches
Millimeters - Check this option to output coordinates in millimeters

Coordinate Position

Reference to absolute origin - Use the absolute origin as the reference point for tespoint coordinates
Reference to relative origin - Use the relative origin as the reference point for tespoint coordinates

IPC-D-356A Options

The IPC-D-356A Options region of the dialog becomes available only when the IPC format option is enabled.

Adjacency Information - Adjacency is a list of nets that could possibly be shorted. Typically the criteria for adjacency is based on a minimum feature separation distance. Net adjacency information is used to reduce isolation testing on flying probe test systems and other test coverage for efficiency purposes.
Board Outline - This record type will permit the description of outlines, and other segment type data that is not connected to a specific net. This record type follows the format of conductor data, with the following exceptions
Conductor Traces - Refer to IPD-D-356A spec for more detail

Generated Files

All generated testpoint files are named first by type (Fabrication or Assembly), then by filename, for example: Fabrication Testpoint Report for BoardFileName. The following file extensions are used, depending on which of the Report Formats is enabled: .txt, .CSV, .IPC (note that this is an ASCII file).

Location of Generated Files

The output path for generated files depends on how the output was generated:

From an OutputJob file - the generated files are stored in a folder within the project folder, the naming and folder structure is defined in the Output Container that the Testpoint output is targeting.
Directly from the PCB -the output path is specified in the Options tab of the Options for Project dialog. By default, the output path is set to a sub-folder under the folder that contains the Project file and has the name: Project Outputs for ProjectName. The output path can be changed as required. If the option to use a separate folder for each output type has been enabled in the Options tab, then the Testpoint files will be written to a further sub-folder, named: Testpoint Output.

Automatically Opening the Generated Output

When generating Testpoint output, you can specify that the output be opened automatically in a new CAM document. The way in which this is accomplished depends on how you are generating the output:

From an OutputJob file - enable the IPC-D-356A Output auto-load option in the Output Job Options dialog (Tools » Output Job Options from the OutputJob Editor).
Directly from the PCB - ensure that the Open outputs after compile option is enabled on the Options tab of the Options For Project dialog (Project » Project Options).