Editing Multiple Objects

Parent page: Editing Strategies

Electronic design is the process of capturing a logical design in the schematic then representing that design as a set of objects in the PCB workspace. Even for a small circuit, the schematic can include many components, each with numerous models and parameters, and the PCB workspace can also contain a large number of design objects that make up the board. During the course of the design process, the properties of these objects need to change as you work to balance out the various design requirements.

To support the task of editing many objects, each version of Altium design tools includes a feature often referred to as Global Editing. The name describes an editing ability rather than a specific feature or button. In early versions, the approach was to edit one object, and then push those changes onto other objects. With the introduction of the DXP integration platform, the technique for applying an edit globally changed.

The basic approach to editing multiple objects now is:

• select the objects to be edited,
• inspect their properties then
• edit them.

Keeping this select – inspect – edit sequence in mind, let's look at some examples of how you actually do that in the software.

This article describes various techniques for applying edits to multiple objects in your design. It covers how to select multiple objects and use the Inspector panel to modify their common properties.

Selecting Multiple Objects

Standard Windows methods of selecting multiple objects apply, i.e. dragging a selection box around a set of objects will select any objects fully contained within the bounding rectangle. The Shift key is used for cummulative selection within CircuitStudio and will toggle the selection of the item under your cursor without affecting existing selections.

Inspecting the Objects

The SCH Inspector panel shows the properties of the selected objects.

Both the schematic and PCB editors include a panel called the Inspector. The basic behavior of the Inspector panel is that it lists the properties of all objects that are currently selected. The set of selected objects can be the same kind of object.

Note in the image above that the SCH Inspector panel includes two options at the top. It is important that you set the second of these, which sets from where the found objects are located – from the current document, open documents, or open documents of the same project. To have all of the selected power ports loaded into the SCH Inspector panel, you must set this to open documents or open documents of the same project.

Editing the Objects

Editing the net name Text

So far you have selected the Power Objects you want to edit, inspected their properties in the Inspector panel, and you are now ready to edit them.

When you click to edit the net name text, the text is selected and ready to edit. Type in the new value. The browse button appears at the end of the Text field. Click this when you want to perform a partial string substitution. For this edit, we will be replacing all the text, so we replace the entire contents of the cell with the new text, 3V3.

The change you make to the text value is applied to all the selected objects as soon as you press Enter on the keyboard or click another cell in the SCH Inspector panel.

If you change your mind during the edit, press the Esc key on the keyboard to abort the edit. To Undo an edit that has been applied, select Edit » Undo from the menus. If the edit has been applied to multiple schematic sheets, you will need to perform an Undo action in each sheet.

The image below shows the SCH Inspector panel after changing the text then pressing Enter next to one of the edited power ports.

Two of the updated power ports

You can use this approach to apply an edit globally to any type of object in the Schematic or PCB Editors.

After performing the edit, you will find that all the other objects on the schematic are faded out, or masked, if the mask level  has been previously set. While something is masked, it cannot be edited. To remove the mask, click the Clear Masks button on the View tab of the Ribbon shortcut: Shift+C).

Applying an Edit to Different Types of Objects Globally

The PCB Inspector panel can be used to edit multiple instances of the same object and can also be used to edit common properties of different objects.

Changing the Net Name for Existing Routing

For the first example, let's assume that you have made design changes on the schematic by removing a pin from one net and adding it to another. If the nets were already routed on the PCB, when you update the PCB, you could end up with routing that has the wrong net name. This routing could include tracks and vias, as well as other kinds of objects.

There are a few ways this could be resolved. The easiest way is to use the PCB Inspector panel. Use the following the process.

1. In the PCB, click Home | Clipboard | Select » Connected Copper command then select all the primitives in the routed net that need their name changed.
2. If it is not already visible, open the PCB Inspector panel (F11).
3. The PCB Inspector panel will only show properties that are common to all the selected objects. If your selection was correct, one of these will be the Net name. To change this, select the new net name from the drop-down list then press Enter to apply the change. The net property of all the different objects in the routed net will be changed.

Changing the Layer Property of Different Objects

Another example might be that you need to move all the objects that are on one mechanical layer to another mechanical layer. To do this:

1. Click the Layer tab for the current mechanical layer at the bottom of the workspace to make it the active layer.
2. Select all the objects on that layer using the Home| Clipboard | Select » All on Layer command.
3. If it is not already visible, display the PCB Inspector panel (F11).
4. Select the new layer name from the Layer list then press Enter to apply the change.

Changing the layer for selected objects

Locking Design Objects

Design objects can be locked from being moved or being edited on the schematic or PCB document by enabling their Locked attribute. For instance, if the position or size of specific objects are critical, lock them. This Locked attribute is available in the design objects' properties dialogs, or the Locked attributes can be toggled collectively in the SCH Inspector or PCB Inspector panels.

Locking Design Objects on Schematic Sheets and PCB Documents

To lock a group of schematic objects, you can use the SCH Inspector panel to toggle the Locked options of all selected objects. You can do the same for a group of PCB objects in the PCB Inspector panel, as well.

To lock an individual object, double-click the object then when its properties dialog opens, enable the Locked option, as shown in the image below.

If you attempt to move or rotate a design object that has its Locked property enabled, a dialog appears asking for confirmation to proceed with the edit.

If the Protect Locked Objects option is enabled on the PCB Editor – General page of the Preferences dialog and the design object is locked , this object cannot be selected or graphically edited. Double-click on the locked object to disable the Locked property or disable the Protect Locked Objects option to graphically edit this object.

If you attempt to select locked objects along with other objects, only those objects that are unlocked can be selected and moved as a group when the Protect Locked Objects option is enabled.