Project Options - Options

Old Content - visit altium.com/documentation

Modified by Admin on Sep 13, 2017

The Options tab of the Project Options dialog.

Summary

The Options tab of the Project Options dialog enables you to specify the output path and related options for generated outputs for the project. You can also specify various netlisting and navigation options and specify the Net Identifier Scope.

Use this tab to define the path to which you want generated outputs for the project to be written. Several options are available with respect to generated output files, including whether or not you wish a separate folder to be used for each output type (e.g. netlists, Gerber files, etc) and whether you want to open outputs after compiling. The latter is associated to manufacturing output that can be automatically imported into the CAMtastic Editor.

The tab also offers netlist options - allowing you to control the use of ports and/or sheet entries to name nets and whether to append sheet numbers to local nets.

You can also determine the Net Identifier Scope to be used for the design, depending on your use of ports and sheet entries.

The lower region of the tab contains various navigation-related options. These options directly affect the display of objects when using either the Navigator or Browser panels (the display of the objects actually within the panels themselves). The display-related options take effect immediately after clicking OK to leave the Project Options dialog - there is no need to recompile/re-analyze the project/document. The highlight-related options determine how an object is visually displayed on a document in the main design window when, for example, clicking an object's entry in the Navigator or Browser panels, or when cross probing. You will need to re-select the object in the relevant panel for the change to take effect.

Access

Click Options tab in Printer Options dialog (Project » Project Options).

Options/Controls

Output Path - This path setting is the default output path for generation of the output files from the current design project or when compiling packaged libraries as an integrated library.
ECO Log Path - This path setting is the default output path for ECO log files.
Schematic Template Location - This path setting is the location for schematic template.

Output Options

Open Outputs after compile - Enable this option to open the outputs of files that were generated from compiling the design project.
Archive project document - Enable this option to archive the open design projects.
Timestamp Folder - Enable this option to include the current date and time information along with the name of each folder output.
Use separate folder for each output type - Enable this option to create separate folders for each output type generated for the design project. Otherwise if you wish to have all the output files stored in one Output folder, disable this option.

Netlist Options

Allow Ports to Name Nets - Enable this option for the port names to name the associated nets instead of system generated net names.
Allow Sheet Entries to Name Nets - Enable this option for the sheet entry names to name the associated nets instead of system generated net names.
Allow Single Pin Nets - Enable this option to allow a net existing in a single pin.
Append Sheet Numbers to Local Net - Enable this option to add the Sheet Number value (this SheetNumber parameter defined for this sheet is in the Document Options dialog) to local nets. A local net is a net that does not leave this sheet and if the net does leave the sheet then it does not get the SheetNumber appended.
If the Net Identifier Scope option is set to Global then every net label name that matches are connected on different sheets, thus the Append Sheet Number to Local Nets option is invalid.
Higher Level Names Take Priority - The net labels used on higher sheets in the hierarchy will be used to name the nets on the lower sheets.
Power Port Names Take Priority - The software has the ability to localize a global power net, by wiring a power port to a normal port. This would force all pins on that sheet, connected to that power port, to be in a separate net. Turning on this option would force it to use the net name on the Power Port.
The naming precedence is as follows: If power ports have priority, the order is: Power ports, Netlabels, ports, pins, but if power ports don't have priority, the order is: Netlabels, power ports, ports, pins.

Net Identifier Scope

Automatic (Based on project contents) – this mode automatically selects which of the net identifier modes to use based on the following criteria: if there are sheet entries on the top sheet, then Hierarchical is used; if there are no sheet entries, but there are ports present, then Flat is used; if there are no sheet entries and no ports, then Global is used.
Flat (Only ports global) – ports connect globally across all sheets throughout the design. With this option, net labels are local to each sheet; they will not connect across sheets. All ports with the same name will be connected, on all sheets. This option can be used for flat multi-sheet designs. It is not recommended for large designs as it can be difficult to trace a net through the sheets.
Hierarchical (Sheet entry <-> port connections, power ports global) – connect vertically between a port and the matching sheet entry. This option makes inter-sheet connections only through sheet symbol entries and matching sub-sheet ports. It uses ports on sheets to take nets or buses up to sheet entries in corresponding sheet symbols on the parent sheet. Ports without a matching sheet entry will not be connected, even if a port with the same name exits on another sheet. Net labels are local to each sheet; they will not connect across sheets. Power ports are global however – all power ports with the same name are connected throughout the entire design. This option can be used to create designs of any depth or hierarchy and allows a net to be traced throughout a design on the printed schematic.
Strict Hierarchical (Sheet entry <-> port connections, power ports local) – this mode of connectivity behaves in the same way as the Hierarchical mode, with the only difference being that power ports are kept local to each sheet; they will not connect across sheets to power ports of the same name.
Global (Net labels and ports global) – ports and net labels connect across all sheets throughout the design. With this option, all nets with the same net label will be connected together, on all sheets. Also, all ports with the same name will be connected, on all sheets. If a net connected to a port also has a net label, its net name will be the name of the net label. This option can also be used for flat multi-sheet designs, however it is difficult to trace from one sheet to another, since visually locating net names on the schematic is not always easy.

Allow Pin-Swapping Using These Methods

On the schematic, there are two ways a pin swap can be handled - by swapping the pins of the component or by swapping net labels on the wires attached to the pins.

Adding / Removing Net-labels - Enable this Net Labels option to allow net labels to be swapped. This option is suitable for FPGA components.
If this option is only selected (the Changing Schematic Pins option is disabled) then when you select a pin or part swap command you will only have access to pins that are connected via net labels.
Changing Schematic Pins - Enable this option to allow pins to be swapped. Be aware that once a component has its pins swapped, this component cannot be updated from the library where it is defined from. Swapping pins is suitable for simple components such as a resistor array.