Designator

Parent page: Schematic Objects

A Designator uniquely identifies a component in the design.

Summary

The designator field is a child parameter object of a schematic component (part). It is used to uniquely identify each placed part, distinguishing it from all other parts placed in all the schematic sheets in the project.

Availability

The designator is automatically placed when the parent component part object is placed. As such, it is not a design object that can be directly placed by the user.

Graphical Editing

The designator string can be edited graphically, using what is known as in-place editing. To edit a designator string in-place, click once to select, pause for a second, then click a second time to enter edit mode.

Click once to select the string.

Pause, then click a second time to enter in-place edit mode.

Here the string has been selected, ready to type in a replacement string.

The value of the designator string can be edited in-place.

Once editing is complete, press Enter or click away from the string to exit in-place editing mode.

An object that has its Locked property enabled cannot be selected or graphically edited. Double click on the locked object directly and disable the Locked property, to graphically edit the object.

Non-Graphical Editing

There are 2 aspects to consider in relation to editing the designator: editing the value of the designator; and editing the display properties of the designator.

Rather than manually editing each component designator, it is more practical to leave the assignment of the designators until the schematic is complete. Then all designators can be logically assigned for the entire project using one of the Schematic Editor Annotate commands, which offers full control for sheet-by-sheet positional annotation.

Editing the Designator Value in the Schematic Library Editor

By default, the designator is not visible in the Schematic Library Editor. It is edited in the Schematic Symbol Properties dialog, double-click on the Component name in the SCH Library panel or click the Edit button to open the dialog, as shown in the image below. Typically the designator is only given a suitable prefix followed by a question mark. The question mark is detected by the Schematic Editor's Annotation tool and replaced with a suitable numeric suffix during project annotation.

Double click on the component name, or click the Edit button, to open the dialog and defined the value of the Designator string.

Alternatively, the designator string (and the comment string too) can be displayed in the Schematic Library Editor, and then doubled-clicked on to edit its properties. To display it, click Tools | Options | , to open the Library Editor Workspace dialog, then enable the Always Show Comment/Designator option, as shown in the image below. This setting is a property of the Schematic Library.

Enable the Always Show Comment/Designator option to display these strings in the Schematic Library Editor.

Editing the Designator Value in the Schematic Editor

The designator can be defined in the Schematic Editor as the component is being placed, or after the component has been placed on a schematic sheet.

  • To edit the designator during component placement, press the Tab key while the component is floating on the cursor. The Properties for Schematic Component dialog will open, enter the required designator string and click OK to close the dialog and complete the component placement. Continue to place components, or right-click or press Esc to terminate placement.
  • To edit the designator after placement, double-click on the placed component to open the Properties for Schematic Component dialog where the designator can be edited. Click OK to close the dialog and commit the change.

Editing the Designator Display Properties

The appearance of the designator string, which includes the font type, size and color, can be defined as:

  1. A property of the symbol, by setting the properties of the designator in the Parameter Properties dialog in the Schematic Library Editor. This requires the designator string to be made visible, as described previously.
  2. By editing the component designator string of the placed schematic component - double-click on the designator string to edit the properties (or use the in-place editing technique described previously).

Both approaches open the Parameter Properties dialog, as shown below. Note that all properties of the designator string can be edited in this dialog.

The value and the appearance of the Designator string can be edited in the Parameter Properties dialog.

Via an Inspector Panel

Panel pages: SCH Inspector, SCHLIB Inspector

An Inspector panel enables the designer to interrogate and edit the properties of one or more design objects in the active document. Used in conjunction with the Find Similar Objects dialog, the panel can be used to make changes to multiple objects of the same kind, from one convenient location.

Fixing the Location of the Designator String

The default behavior of the designator string is to autoposition it as a component is rotated during placement. If this behavior is not required, turn off the Autoposition option in the Parameter Properties dialog (refer to the previous image), either during symbol creation or after the component has been placed on a schematic sheet. Note that doing this sets this parameter to be classified as a manual parameter (meaning manually positioned parameter). Manual Parameters are identified by a dot on the lower left corner of their selection box.

Notes

  1. The Schematic Editor includes a simple auto-increment feature for the designator, which can be used during the placement of multiple instances of the same part. To use this, press Tab while the first component is floating on the cursor and enter a suitable designator, for example R1. Subsequent components will then be designated R2, R3, etc. Note that when you switch to placing a different component type you must again press Tab and enter a suitable designator prefix.
  2. When placing multi-part components and the initial designator is assigned as just described, a part suffix will automatically be assigned, for example U3A, U3B,... If the initial designator is not assigned all parts will have the same suffix, this is resolved by the Schematic Editor's Annotation command. The part suffix can be alpha or numeric, use the Alpha Numeric Suffix option in the Schematic - General page of the Preferences dialog to configure this.

 

You are reporting an issue with the following selected text and/or image within the active document: