複数の設計オブジェクトの編集

The process of editing multiple items in Altium 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.

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:
  • The Find Similar Objects dialog.
  • The PCB panel.
  • The PCB Filter panel.
  • The PCB List panel.
  • The Selection Filter option of the Properties panel.

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.

• 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.

Locking Design Objects

Design objects can be locked from being moved or being edited on the PCB document by enabling their Locked attributes. For instance, if the position or size of specific objects is critical, lock them. Locking can be done in the Properties panel by clicking on the padlock icon ( ) for the desired object(s) as shown in the following examples. 

   Examples of the Lock icon in the Properties panel in Component mode and Pad mode.

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.

Masking

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.

• 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.

The Find Similar Objects process uses the attributes of a target object as a reference for finding several other objects with similar characteristics. It can be accessed in the following ways:

• By using the Edit » Find Similar Objects menu command.
• By using the Shift+F shortcut.
• When right-clicking over an object.

The Find Similar Objects dialog is divided into two primary sections; the upper section consists of a grid that lists the attributes of the reference object, and the lower section consists of a group of check boxes that define what will happen once the Apply or OK button is clicked.

The left column lists the attributes of the reference object. The center column lists the value of those attributes and the right column defines grouping.

To search for objects with different values, enter the search pattern into the attribute value column directly; the '*' character can be used as a wildcard for finding any group of characters. Edits made to the attribute value in the Find Similar Objects process will not alter the attributes of the reference object.

The right column of the table contains a drop-down list of options used for specifying how the associated attribute should be used to find similar objects:

• Any - Find similar objects with an attribute value that has any value. This is the default that will ignore the associated attribute from the filter.
• Same - Find similar object with an attribute set to the same value as this one.
• Different - Find similar object with an attribute set to a different value to this one.

The options in the lower section of the Find Similar Objects dialog define the action to be taken for the identified items.  The check boxes and drop-down fields operate as follows once the Apply or OK button is clicked:

• Zoom Matching - Zoom the display to a window that encompasses all found objects in the workspace.
• Select Matched - Select all found objects matching the search criteria.
• Clear Existing - Clear any existing Selection or Editing Mask before performing the search. Uncheck this option if doing successive Find Similar Objects searches and it is desirable for the results to accumulate.
• Create Expression - Create an expression that matches the criteria specified by the Find Similar Objects dialog and enter it into the PCB Filter panel. The PCB Filter panel will be opened if it is not already. This option makes it possible to use the Find Similar Objects dialog as a quick way of constructing complicated filtering operations.
• Open Properties - enable to automatically open the Properties panel.

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.

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'