Working with a Designator Object on a Schematic Sheet in Altium Designer

Parent page: Schematic Objects

The Designator uniquely identifies each 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 to distinguish it from all other parts placed in all the schematic sheets in the project.

Availability and Placement

The designator is automatically placed when the parent component part object is placed. It is not a design object that the user can directly place.

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.

 In this image, 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.

Non-Graphical Editing

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

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 Library Component Properties dialog. To open the dialog, double-click on the component name or click Edit in the SCH Library panel, 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.

Alternatively, the designator (and comment) strings can be displayed in the Schematic Library Editor, and then doubled-clicked on to edit their properties. To display them, select Tools » Document Options to open the Schematic Library Options dialog, then enable the Always Show Comment/Designator option, as shown in the image below. This setting is a property of the current 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 in the Properties for Schematic Component dialog.

• To edit the designator during component placement, press the Tab key while the component is floating on the cursor. The Library Component Properties 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 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 software default by setting the Designator defaults in the Schematic - Default Primitives page of the Preferences dialog. This setting will apply unless overridden by settings defined in the component symbol in the Schematic Library Editor.
2. 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 in the previous section.
3. By editing the component designator string of the placed schematic component - double-click on the comment string to edit the properties, or use the in-place editing technique described below.

All the above 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, SCH Filter, SCHLIB Filter

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 appropriate filtering - by using the applicable Filter panel, or the Find Similar Objects dialog - the panel can be used to make changes to multiple objects of the same kind, from one convenient location.

Via a List Panel

Panel pages: SCH List, SCHLIB List, SCH Filter, SCHLIB Filter

A List panel allows the designer to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering - by using the applicable Filter panel, or the Find Similar Objects dialog - it enables the display of just those objects falling under the scope of the active filter – allowing the designer to target and edit multiple design objects with greater accuracy and efficiency.

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 that 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, etc. 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.