PCB Inspector

Parent page: Panels

Manually select PCB objects or use the PCB Filter Panel to populate the PCB Inspector panel with objects to be viewed or edited. Here, the PCB Inspector is showing the objects from a (OnLayer ('Top Layer') AND IsComponent) scope applied in the PCB Filter panel (with its 'Select' option checked).

Summary

The PCB Inspector panel enables you to interrogate and edit the properties of one or more design objects in the active PCB document. Used in conjunction with appropriate filtering, the panel can be used to make changes to multiple objects of the same kind, from one convenient location. It's a natural partner to the PCB Filter panel.

Panel Access

To display the PCB Inspector panel, click the PCB button  at the bottom-right of Altium Designer when the PCB Editor is active, and select the PCB Inspector entry from the pop-up menu. Alternatively, you can access the panel through the View » Workspace Panels » PCB » PCB sub-menu.

Panels can be configured to be floating in the editor space or docked to sides of the screen. If the PCB Inspector panel is currently in the group of docked Workspace panels on the left, use the PCB Inspector tab located at the bottom of the panels to bring it to the front.

Defining Panel Display Scope

The PCB Inspector panel allows you to define which objects are displayed in the panel (the display scope) via filtering controls. This can be accessed using the underlined control at the top of the panel.

You may have a large quantity of objects selected in the workspace that are of differing type. Out of all such objects, you may wish to edit the properties of certain object types only, without losing or having to alter your selection.

Use the pop-up to choose which object types you wish to include in the panel for display and editing - either all objects or specific objects. To choose one or more specific object types, enable the Display only option and then enable the check box next to the required object(s) in the list beneath. The list will only contain those object types currently selected in the main workspace.

When enabling specific object types for display, the control will reflect the choice by listing the enabled types, separated by commas.

Inspecting Object Attributes

The main regions of the PCB Inspector panel show sections of attributes for objects falling under the defined display scope.

Clicking on a single object in the PCB design editor window will select that object and display attributes associated to it in the PCB Inspector panel. Information is displayed under the following common collapsible sections:

Kind

This section of the panel contains one entry only, relating to the kind of design object that is being 'inspected'. For example, clicking on a component in the workspace will display the entry Component, clicking on a component designator will display the entry Text, and so on.

Object Specific

This section of the panel contains attributes specific to the object being inspected and which are not graphical attributes. For example, selecting a component will display the following attributes that are specific to a component:

• Layer
• Name (the component designator)
• Component Comment
• Lock Strings
• Footprint
• Channel Offset

Other selected objects will have different attributes displayed. For example, selecting a pad object will display attributes including Pad Shape/Size, Solder Mask Tenting and Electrical Type.

Graphical

This section of the panel contains graphical attributes of the selected object. Attributes here may include the location of the object, its rotation and dimensions, and whether it is locked.

Editing Object Attributes

You can edit attributes of a selected object, by editing the relevant entry in the panel. The change will take effect once you click outside of the field you are editing. This is one of the advantages of using the panel to edit object properties - the panel will remain open, allowing you to change attribute after attribute, as needed, without having to close and reopen a properties dialog each time.

If the object you are inspecting has child objects associated with it, they will appear in blue in the Object Specific section (rather like a hyperlink). Click on these entries to display the attributes pertaining specifically to these child objects, as illustrated in the image below. For each child object, a link will be available back to the parent object.

A child object will appear as a link, which allows the child object attributes to be inspected and edited.

Another advantage of using the panel for editing is that you can edit multiple objects from the one place, without having to edit, through dialogs, one object at a time. Selected objects can be of the same or differing type. Those attributes that are common to all objects in the selection will be displayed in the panel. Common attributes that have differing values between objects will be displayed as <...>. As the attributes are edited as required, the changes made will be conveyed instantly to each object in the selection.

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

Editing Attributes with Numeric Values

For a numerical-based attribute of a selected object, the simplest modification to that attribute's value is made by typing a new value to replace the existing one. The plus and minus operators can be used to specify the value's sign. A value entered without a specified sign is assumed to be positive. Therefore entering 20 is the same as entering +20.

You can enter specific units of measurement for a value entered. The software will convert the value into the current units defined for the document. If no units are specified, the default units set for the document will be used.

Modification Using an Expression

More advanced modification can be achieved by using an arithmetic expression. Select the entry for the attribute you wish to modify and type the expression that will be used to modify its value. You can enter any arithmetic expression, using any built-in arithmetic operators and functions (found in Pascal).

If you wish 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). If you wish, you may use any other attribute field name in an expression. When using attribute names, if any names contain spaces, these must be replaced by the underscore character.

To illustrate an example of using a simple expression, consider a component, the Height attribute of which is currently 200mil. If you wanted to extend this height to 500mil, you could enter the expression:
Height + 300
...or, in shortened form:
! + 300
Note that the spaces are optional. When you press ENTER the value will be updated to 500mil.

If instead you want to reduce the height to 100mil, you could use the subtraction operator, as illustrated by the following expressions:
Height - 100
! - 100
To illustrate use of a function, the previous expression could be re-written as:
! - sqr(10)
...the result would be the same - a height of 100mil (ten squared).

By using the attribute's name, or substitution character (!), the previous expressions add to or subtract from the current value for the attribute. Without such entries in the expression, you would be setting the attribute's value to the evaluated result of the expression. For example, if the attribute name or substitution character had been left out of the previous expressions, the resulting value for the component height would have been 300mil and -100mil respectively.

Again, you can enter specific units of measurement for a value entered into an expression. The software will convert the value into the current units defined for the document. If no units are specified, the default units set for the document will be used. By selecting multiple objects in the workspace, you can change numerical attributes simultaneously using an expression. For example, you may want to adjust the height of a series of components associated with a particular region of the board, or shift components vertically or horizontally by a specific distance.

 Batch Replacement of String-based Attributes

There are times when you may want to modify a string-based attribute that is common to multiple selected objects. For example you may wish to rename the designators of selected header components from P1, P2, P3, etc, to HDR1, HDR2, HDR3, etc. To perform this type of batch replacement, the use of string substitution syntax is supported in the panel.

A string substitution entry is enclosed in braces and has the form: {oldstring=newstring}

An entry of this form causes all occurrences of 'oldstring' found in the attribute's value to be replaced with 'newstring'. In the case of the designators, you would enter {P=HDR) in the value field for the Name attribute.

Should you wish to replace multiple, differing string portions in the same target string, type multiple substitution entries, with each enclosed in its own set of curly braces. For example, consider the following free text strings placed on the PCB of a four port communications switching device, where each port provides for communication with an 8-bit peripheral device:
CommPortA_8
CommPortB_8
CommPortC_8
CommPortD_8

Now consider having modified the design to allow for communications with 32-bit external peripheral devices. Also, the customer has requested that the Comm prefix be replaced by IO. The free strings now need to be updated, which is where batch string substitution comes into play.

If the intended format of the new strings is to be IOPortx_32, where x represents the port (A, B, C or D), then you could select the four free string objects, access the PCB Inspector panel and enter the following into the value field for the String attribute: {Comm=IO}{8=32}

The software takes this entry and effectively performs a batch substitution - substituting for the first expression, then the second.

Smart Editing of String-based Attributes

The PCB Inspector panel offers further support for string modification through its Smart Edit feature. Simply click on a shared attribute of the selected objects, whose value is a string. A  button will become available at the far right of the cell. Click on this button to access the Smart Edit dialog.

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

Batch Replace Tab

This tab provides simple straightforward substitution, along the lines of the string substitution discussed previously (but without having to enter the curly braces). Click in the From field and enter the portion of the current string that you wish to replace. Click in the To field and enter the string to be used as the replacement. The familiar string substitution syntax is displayed at the bottom of the tab.

For example, consider the designators of three header components that currently have the prefix P, but you need to change them to have prefix HDR instead. In this case, select the components, click on the Name attribute in the panel and access the Smart Edit dialog.

Then on the Batch Replace tab, enter P in the From field and HDR in the To field (the replacement string is therefore {P=HDR}). After clicking OK, the designators will be modified accordingly.

As with basic string substitution, the Batch Replace tab provides for replacement of multiple, differing string portions in the same target string. Enter the various substitutions as distinct From-To entries. Consider the previous Comms Port example (see Batch Replacement of String-based Attributes), where strings of the form CommPortx_8 need to be changed to IOPortx_32. In this case, you would enter two distinct substitution entries on the Batch Replace tab.

Formula Tab

This tab provides for more advanced modification, allowing 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). Once again, if you wish 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. So, for example, use of the Component Comment field within a formula should be entered as Component_Comment.

Consider 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. Using the addition operator, 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'
Note that the spaces are optional. When you press ENTER the designators of the components will be updated to U1_MEM, U3_MEM and U5_MEM respectively.

To illustrate the use of string-based functions consider the Copy function, which can be used to take a portion of an original string and place it within an expression to create a new string. Take again the Comms Port example (see Batch Replacement of String-based Attributes), where strings of the form CommPortx_8 need to be changed to IOPortx_32. In this case you could select the four free string objects, access the Smart Edit dialog for the String attribute and write the following expression on the Formula tab:
'IO' + Copy(String,5,6) + '32'
...or, in shortened form:
'IO' + Copy(!,5,6) + '32'

Notes

• Pressing the F11 key will toggle the visibility of the panel in the workspace.
• Information will only appear in the panel when either:
    1) One or more objects have been selected in the design editor window, or;
    2) Object entries are selected in the PCB List panel.
• With multiple components selected in the workspace, you can drill-down to make changes to Designator or Comment and the changes will be made to all components in the selection. Using the hyperlink entries you can pass back and forth between parent and child objects, without losing the selection.
• You can use the TAB and SHIFT + TAB keyboard shortcuts to pass down and up the list of attributes in the panel respectively. Alternatively, the arrow keys can also be used.
• When applying a filter using the PCB Filter panel, the attributes for the resulting filtered objects will only be displayed in the PCB Inspector panel if the Select option - located in the Objects passing the filter area of the panel - is enabled prior to application of the filter.