Editing Multiple Design Objects

Now reading version 22. For the latest, read: Editing Multiple Design Objects for version 24

Parent page: Getting Familiar with the Altium Design Environment

Altium Designer provides a range of editing tools and capabilities that have been designed to help with making large-scale edits to a design. The main tools for large-scale or global edits are the PCB Filter panel, PCB List panel and Find Similar Objects capabilities.

The process of editing multiple items in Altium Designer involves three steps:

  1. Select the objects to be targeted.
  2. Inspect the properties of those objects.
  3. Edit the properties that need to be amended.

With this editing paradigm in mind, the software offers a range of different ways to select, inspect, and edit multiple objects. Each method has its strengths and by having an understanding of how they work, you are equipped to choose the method that is most applicable to your specific editing challenge.

While this document covers the editing of multiple objects in the PCB editor, many of the same functions apply in PCBLIB documents and can be accomplished through use of the PCBLIB List and PCBLIB Filter panels. Refer to the documentation on those panels for more information.

Selecting Objects

Objects can be selected in a variety of ways and they all fall into two categories:

  • Graphical Selection – objects are selected in one of the following ways:
    • Individually by mouse clicks.
    • Accumulatively by Shift+mouse clicks.
    • Using one of the sub-menu selection commands from the main menu (Edit » Select).
  • Logical Selection – objects are selected using an interactive or query-based process that targets and filters objects using specific parameters and/or attributes as the search criteria. GUI elements that support this type of selection are:
See the Design Object Selection page to learn more.

Inspecting Objects

The attributes of objects can be inspected or viewed in a variety of ways:

  • Direct Inspection – the attributes of one or more objects are inspected directly through the Properties panel or graphically in the main editor.
  • Indirect Inspection – the attributes of one or more objects that have previously been selected are viewed using the PCB List panel.

Editing Objects

Similarly, objects can be edited in different ways:

  • Direct Editing – the attributes of one or more objects are edited directly through the Properties panel or graphically in the main editor.
To edit all selected objects, open the Properties panel by clicking the Panels button then choose Properties. To edit only the last object selected, right-click then choose Properties.
  • Indirect Editing – the attributes of one or more objects that have previously been selected can be edited using the PCB List panel.

Examples of viewing and editing Polygon properties directly through the Properties panel or indirectly through the PCB List panel.
Examples of viewing and editing Polygon properties directly through the Properties panel or indirectly through the PCB List panel.

Modifying Data Strings using the Properties Panel

Using Formulas

The Properties panel has the ability to modify data strings using formulas in the schematic and PCB editors. Formulas and expressions offer a convenient method of modifying attribute parameters of multiple selected objects to change their location or string-based values such as the Designator and Comment. This allows you to apply a specific expression to the selected string objects. The expression can include any built-in arithmetic operators and functions that apply to strings (found in Pascal). If you want to use the current value for the attribute as part of the expression, you will need to make reference to this original value either by using the full name of the attribute or by using the exclamation character (the supported substitute for the name of the attribute currently being modified). When using attribute names, if any names contain spaces, these must be replaced by the underscore character. For example, use of the Component Designator field within a formula should be entered as Component_Designator.

Using the Smart Edit Feature

Some parameter string fields also provide access to the Smart Edit dialog when multiple objects are selected, which is opened from the associated button.

The Properties panel offers further support for string modification through its Smart Edit feature. Select the cell entries pertaining to the attribute that you want to modify for all required objects, right-click then choose Smart Edit from the menu that appears. The Smart Edit dialog will open.

The dialog offers two methods for performing string modification accessed from the Batch Replace and Formula tabs.


Masking is a way of explicitly removing an object's eligibility for selection and/or editing. It can be faster to first mask out what is not required instead of selecting what is required.

Consider a design where all vias sitting under a specific BGA device need to have their diameter changed. One way to perform this operation would be to run a query that masks out all non-via objects on the design, then use the Edit » Select » Inside Area menu command to draw a rectangle around the BGA device to select the vias to be targeted. 

Masked objects appear faded, where the selected object passes the applied filter and is displayed normally, with all other design objects faded in gray. The level of fading can be adjusting using the Dimming options in the Highlight Methods region of the System - Navigation Preferences page.

Clearing Selections

The current selection can be cleared in the following ways:

  • Pressing the Shift+C shortcut.
  • Using one of the Edit » Deselect sub-menu commands.

Selection Commands

The following selection-based commands are available from the Edit » Select sub-menu.

  • Select overlapped - use this command to single select the next design object in a set of co-located (overlapping) objects, without utilizing a selection pop-up window. (Shortcut: Shift+Tab)
  • Select next - with an initial object selected in the design, use this command to extend the selection to include the next higher-level object (or objects), based on logical hierarchy. (Shortcut: Tab)
  • Lasso Select - use this command to select design objects within a user-defined, free-form 'lasso' area.
  • Inside Area – use this command to select design objects within a user-defined area. All objects that fall completely inside this defined area will become selected.
  • Outside Area – use this command to select design objects outside of a user-defined area. All objects that fall completely inside the defined area will remain non-selected. All objects outside of this area will become selected.
  • Touching Rectangle – use this command to select design objects touched by a user-defined bounding rectangle.
  • Touching Line – use this command to select design objects touched by a user-defined line.
  • All – use this command to select all design objects in the current document, including the board shape. (Shortcut: Ctrl+A).
  • Board – use this command to select the board shape and all design objects that lay within its bounding rectangle. (Shortcut: Ctrl+B).
  • Net – use this command to select all routed track and electrical objects associated with a particular net. Simply click on an object within the required net. Click on an area of the design, away from any objects, to access the Net Name dialog in which the name of the net can be entered directly. If unsure of the name, enter ? and click OK to access the Nets Loaded dialog, which lists all currently loaded nets for the design.
Selection is not cumulative for most of these commands including Net. When a new item is selected, the previous object will become deselected. Press the Spacebar to accumulate selected items.
  • Connected Copper – use this command to select all routed track and electrical objects that are all connected to the same piece of copper. Click on an electrical object (track, pad, fill, etc.) and all electrical objects that are connected by the same piece of copper will become selected. (Shortcut: Ctrl+H).
  • Physical Connection – use this command to select all routed track between two pad objects. Simply click on a track or pad and all contiguous tracks between the two pads will become selected, including any vias. The pads themselves will not be included in the selection.
  • Physical Connection Single Layer – use this command to select connected track segments on the current layer, i.e., to select contiguous copper until the layers change or a component pad is encountered.
  • Component Connections – use this command to select all routed connections emanating from the pads of a chosen component. The component's pads, along with connected tracks and vias will be selected, up to the next encountered pad in each case.
  • Component Nets – use this command to select all nets attached to a chosen component. All nets (and member net objects therein) attached to that component will be selected.
  • Room Connections – use this command to select all pad-to-pad routed connections that fall completely within the boundaries of the chosen room.
  • All on Layer – use this command to select all design objects on the current layer. The current layer is distinguished by the active tab at the bottom of the main design window.
  • Free Objects – use this command to select all free primitive objects within the design. Group objects (such as components, coordinates, dimensions, and polygons) will not be selected. These objects must be converted to their free primitives in order for this selection mode to apply.
  • All Locked – use this command to select all design objects that have their Locked property enabled.
  • Off Grid Pads – use this command to select all pads that are not placed on a defined snap grid.
  • Toggle Selection - use this command to change the selection status of one or more design objects in the current PCB document.
All currently selected objects will be deselected when using this command unless the Click Clears Selection option is disabled on the PCB Editor – General page of the Preferences dialog.
Various de-selection commands are available from the Edit » Deselect sub-menu, including deselection of all selected objects, all selected objects inside or outside of a user-defined area, all selected objects on the current layer, and all selected free objects.

PCB List Panel

PCB List Panel Inspect and Edit

The PCB List panel displays design objects from the active document in tabular format enabling you to quickly inspect and modify object attributes. When used in conjunction with the PCB Filter panel, it can be used as a powerful way to both inspect and edit multiple design objects. Objects do not need to be selected in order for them to be displayed (and edited) in the PCB List panel.

PCB List Panel Access

There are several ways to display the PCB List panel:

  • Press the Shift+F12 shortcut key to toggle the panel on and off.
  • Select PCB List from the Panels popup button in the bottom right of the main editor window (assuming the View » Status Bar option is enabled).
  • Click View » Panels » PCB List from the main menus.

Defining Panel Display Scope

Controls at the top of the panel show the current mode and controls how objects are filtered.

View/Edit Mode

Use the first field to choose the PCB List panel mode. Select View to view only object attributes. Direct editing from within the panel will not be possible in this mode, as indicated by the gray background of the spreadsheet-like region. Select Edit to view and edit the attributes of design objects directly in the tabular region of the panel.

Object Selection

Click on the next underlined control to select from the following options:

  • non-masked objects – this is the default option and causes the panel to display only design objects that are not masked-out in the workspace (i.e., only those objects that fall under the scope and specific query expression of the currently applied filter). This option is most effective when filtering is applied to the workspace and the associated dimming option is enabled.
  • selected objects - this option causes the panel to display only design objects that are currently selected in the workspace.
  • all objects - this option causes the panel to display all design objects.

Types of Objects

Clicking on all types of objects allows you to control the type of objects that can be displayed. Click on the control to open a selection pop-up.

The 'No' option refers to other object primitives that are featured in the PCB document but are not denoted in this list, such as Layer Stack Table and Drill Table object primitives.

Use the pop-up to choose which object types to include in the currently displayed list – either all objects or specific objects.

To choose one or more specific object types, enable the Display only option then enable the check box next to the required object(s) in the list beneath. The list will only contain those object types currently displayed in the main spreadsheet region of the panel.

The control will update to reflect the range of objects included (e.g., Component and Region).

Making Selections from the PCB List Panel

Design objects selected in the PCB List panel become selected in the design workspace. The list supports single or multiple selections, the latter using standard Ctrl+Click, Shift+Click, and click-and-drag features. Double-clicking on an entry will open the Properties panel in the appropriate mode and can then be edited as usual.

As objects are selected in the panel (or conversely, as objects are selected within the workspace), those objects will appear distinguished in the list by the use of a non-white background for all associated cells.

Inspecting and Editing Object Attributes

While in Edit mode, edit attributes of an object by editing the relevant cell in the panel. Click on a cell to focus it and then either right-click and choose Edit or click again to edit the attribute value directly. Depending on the attribute, either type a value, toggle a checkbox or select an option from a drop-down. The change will take effect after pressing Enter or clicking outside of the cell being edited.

An advantage of using the panel to edit object properties is that the panel will remain open, allowing attribute after attribute to be changed, as needed, without having to close and reopen the Properties panel each time.

Another advantage of using the panel for editing is that multiple objects can be edited from one place, without having to edit numerous times. Selected objects can be of the same or differing types. Those attributes that are common to all objects in the selection will be displayed in the panel.

Simply select the required cells – across all required objects – for the shared attribute to be modified. Then either right-click and choose the Edit command or press the F2 key (or the Spacebar). Edit the value for the chosen attribute with respect to the focused object in the selection (whose cell is distinguished by a dotted outline). Clicking outside the attribute's cell or pressing Enter will effect the change, which will subsequently be applied to all remaining objects in the selection.

By using filtering, a query can be applied (an expression for the filter) to target a specific group of objects in the design and then use the PCB List panel to edit the attributes for these multiple objects directly.

Smart Grid Tools

Smart Grid Commands

There are two Smart Grid commands available from the panel's right-click menu. These commands allow data from an external table (e.g., PDF) or spreadsheet (e.g., Microsoft Excel) to be used to either update the values of existing objects in the PCB List panel (Smart Grid Paste) or insert newly-created objects (Smart Grid Insert). 

Respective dialogs (Smart Gride Paste and Smart Grid Insert) for these commands are used to map the external tabular data coming in on the Windows clipboard to the attributes of objects in the PCB List panel, providing a preview of what changes will be made.

Smart Editing of String-based Attributes

The PCB List and PCBLIB List panel offer support for string modification through its Smart Edit feature. Select the cell entries pertaining to the attribute to be modified for all required objects, right-click, then choose Smart Edit from the context menu. This opens the Smart Edit dialog, which can be used to create Batch Replace or Formula based text substitutions.

The Batch Replace tab is used for string substitutions. For example, consider the designators of three header components that currently have the prefix P and you need to change them to have the prefix HDR instead. In this case, select the Name attribute for each of the components in the appropriate panel to open the dialog. On the Batch Replace tab, enter P in the From field and HDR in the To field (the replacement string at the bottom of the dialog is therefore {P=HDR}). After clicking OK, the designators will be modified accordingly. The Batch Replace tab also provides for the replacement of multiple, differing string portions in the same target string. Enter the various substitutions as distinct From-To entries.

The Formula tab provides for more advanced modification, allowing you to apply a specific expression to the selected string objects. For example, three selected memory components specified in a design with designators U1, U3 and U5. You might want to extend the designators of these components by including some indication of their role. After loading the required components (or designators) into the appropriate List panel, open the Smart Edit dialog using the techniques described in the Access section above. In the Formula tab, you could write an expression to add to the existing string value of the Name attribute. This would take the existing (original) string value and concatenate it with a specified new string, as illustrated below:

Name + '_MEM'

or, in shortened form:

! + '_MEM'

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

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.