Parent page: PCB Panels
The PCB Filter panel provides controls to construct filters through the creation of logical queries. A defined filter can then be applied to the active PCB, allowing you to select and edit multiple objects with great accuracy and efficiency.
The panel is accessed from the PCB editor in the following ways:
The PCB Filter panel is composed of three regions. The first two are selectable list areas that collectively define the scope of the filtering: Object and Layer.
The third region, Filter, displays the query created based on which objects and layers are currently selected.
The main region of the panel provides controls for quickly building simple filter expressions targeting any combination of objects. Object types are arranged in an 'object matrix', categorized in accordance with being net objects (Net), component objects (Comp), or free objects (Free). The following core object list is replicated across these three groups:
The Text object is available as part of the Comp and Free groupings, however, since this object type is not net-aware, it is not part of the Net grouping. In addition, the Free grouping also includes: Component, Component Body, Room, and Polygon.
If these are set to 'Component' and 'Top Layer', for example, the board view will highlight top layer components. The selections in both panel sections represent the cumulative effect of multiple stages of filtering action, which can be used to quickly highlight any type of design object.
To use an object in the construction of a filter expression, i.e. filtering by that object, enable the relevant check box associated with that object within the object matrix. Commands available on the right-click menu for the region enable you to quickly check or uncheck all entries in the matrix or toggle the state of all checkboxes in the matrix.
Use the Layer region of the panel to restrict the filter to a particular layer or layers or a specific class of layers. The entries listed reflect:
As you make your filtering selections, the resulting query expression is built dynamically and presented in the Filter region of the panel. Once the filter query expression has been defined as required, you then need to apply it as a separate action. To do this, click the Apply to All button at the bottom of the panel. Alternatively, if you require application to only those objects that are currently selected in the workspace, click the Apply to Selected button.
The selection in the panel's Object list will filter the board view to show primitive design objects. All objects will be highlighted unless modified by the settings in the Object and/or Layer filter lists.
The selection in the panel's Layer list filters the board view to show objects on the nominated physical design layer (Signal, Mask and Silkscreen layers). All valid layer objects will be highlighted unless modified by the settings in the Layer and/or Objects filter lists.
The collective filter action provided by the panel assists both viewing and selecting board design objects of interest.
Only highlighted (filtered) objects are selectable, making it easy to locate, edit and find information about the object.
Clear the currently applied filter by clicking the Clear button.
The visual result of the applied filtering on the document in the workspace is determined by a series of highlighting controls. The effect that is imposed in the editor view can be set to Normal, Mask or Dim, where in practice, Mask has the most obvious highlighting effect.
The Normal / Mask / Dim drop-down list provides options for visibly contrasting filtered and unfiltered objects within the workspace .
The visual highlighting effect for each masking mode:
The central region of the panel provides controls to construct filters through the entry of logical queries.
You can type a query directly into the field, and as you type, a list of possible keywords appears as an aid.
Two functions are available that help in the creation of queries - the Query Helper and the Query Builder. These functions can be very useful if you are unsure of the syntax of a query or the possible keywords that you may want to use.
To use the Query Helper, click the Helper button to open the Query Helper dialog. The underlying Query Engine analyzes the document and lists all available objects along with generic keywords for use in queries.
Use the top section of the dialog to compose a query expression using the available PCB Functions, PCB Object Lists and System Functions. The middle region of the dialog provides a range of operators for use when constructing an expression. Use the Check Syntax button to verify that an expression is syntactically correct.
When the expression for the query has been defined as required, click OK to load the central region of the panel with the query, ready to apply the filter.
To use the Query Builder, click the panel's Builder button to open the Building Query from Board dialog. This dialog enables you to create a query for targeting specific objects in the design document by construction of a string of ANDed and/or ORed conditions. The left side of the dialog is used to specify the condition(s) that are required to target the set of objects needed. Initially, the entry in the Condition Type/Operator column will be Add first condition. Clicking once on this entry will reveal a drop-down list of condition types.
The condition types that are listed will reflect only those relevant to a board design.
Select the desired condition then click in the Condition Value column to access a drop-down list of possible values for that condition type. As you define a condition in the left side of the dialog, a preview of the currently built query is shown in the right side.
Continue to add further conditions to narrow down the target set of design objects as required. Conditions can be ANDed or ORed together. The default logical operator is AND, which is automatically inserted when you add another condition.
To change the logical operator between conditions, click on the AND or OR entry in the Condition Type/Operator column then select the required operator. The preview of the query will update accordingly.
The and buttons at the top of the Building Query from Board dialog allow you to add and remove brackets around the presently selected condition (increasing and decreasing indent). This allows you to create precedence for certain logically ANDed or logically ORed conditions.
For example, consider the following built query:
InNet('5V') AND (OnLayer('TopLayer')
The first condition has been set to the condition type
Belongs to Net with value
16M_IN. Another condition has then been added using the condition type
Exists on Layer with the value
At this stage, with the second condition selected in the dialog, the right arrow button has been clicked. Brackets have been automatically added around the second condition and now the possibility to add a condition within that pair of brackets is available.
The third condition with condition type Object Kind is and value Track is then added within the brackets.
Use the Show Level drop-down at the top-left of the dialog to control the visual display of levels in your structured string of conditions. This essentially expands/collapses the display of brackets. Adding brackets effectively creates a new level. You can display levels 1-5, but for any further levels added, use the Show All Levels option.
Alternatively, click on the expand or contract symbols (associated with a bracketed condition) to show the next level(s) or hide the current level (and all levels below) respectively. The and buttons at the top of the dialog can also be used to expand or collapse the currently selected condition.
Use the and buttons at the top of the dialog to move a selected condition in the query string. For a condition that has sub-levels (i.e. a bracketed condition), any condition in the level structure can be moved. When levels are expanded, a condition can be moved down or up through the levels. When levels are collapsed, a condition will be moved over the level structure.
When the expression for the query has been defined as required, click OK to load the central region of the PCB Filter panel with the query, ready to apply the filter.
As you enter and apply a new query, it will be added to a query history list. Click the History button to access this list. The Expression Manager dialog opens with the History tab active.
To use an historical query from the list, either select its entry and click on the Apply Expression button or double-click on the entry directly. The dialog will close and the expression for the query will be loaded into the central region of the PCB Filter panel.
An historical query can be added to the list of favorite queries by selecting its entry and clicking the Add To Favorites button. Use the Clear History button if you want to 'flush' the history list. Up to nine of the most recently used query expressions from the list will be available for use from the panel's right-click menu.
Any defined query may be added to a list of favorite queries in two ways:
Click the Favorites button in the PCB Filter panel in order to access this list. The Expression Manager dialog opens with the Favorites tab active.
To use a favorite query from the list, either select its entry then click on the Apply Expression button or double-click on the entry. The dialog will close and the expression for the query will be loaded into the central region of the PCB Filter panel.
When a query expression is added to the Favorites list, it is assigned a unique name. By default, a generic name is assigned -
Favorite_n - where
n is the next available unused number. The name for an entry can be changed at any stage by using one of the following methods:
In each case, type the new name as required then click outside the Name field to effect the change.
To remove a query from the Favorites list, select its entry in the list then either click the Remove button or choose the Remove command from the right-click menu. A dialog will appear requesting confirmation of the removal. Up to ten of the most recently added query expressions to the list is available for use from the top of the panel's right-click menu. Note that the content of the Favorites list is common to (and accessible from) bot h the PCB Filter panel and PCBLIB Filter panel.
The PCB Filter panel also provides the facility for creating a design rule, where its scope will use the currently defined query expression in the central region of the panel.
To add a new design rule, click on the PCB Filter panel's Create Rule button. The Choose Design Rule Type dialog will open.
This dialog lists each of the rule categories and rule types that are available in the PCB document. Choose the type of rule you want to create then click OK (or double-click directly on the entry). The PCB Rules and Constraints Editor dialog will open.
The newly created rule name can be seen selected in the left side navigation tree. The rule query expression is in the dialog's top-right pane.
A rule of the chosen type is created and the main editing window for the rule is displayed, ready for you to define specific constraints for the rule. The query expression from the PCB Filter panel is entered into the Full Query region of the dialog. Refine the rule configuration settings as required, and apply the new rule.
Once you have defined a query and set up the options in the panel as required, the filter can be applied either by clicking one of the panel's Apply buttons or by clicking Enter.
To clear the currently-applied filter from within the panel, clear (select and delete) the query expression in the central region of the panel then either click one of the Apply buttons or press Enter. All objects in the design workspace will be restored to full visibility and be available for selection/editing.
Right-clicking within the PCB Filter panel provides access to additional options and commands via pop-up menus.
Right-clicking in the Object or Layer region of the panel opens the following context menu options:
^, *, /, Div, Mod, And
+, -, Or, Xor
=, <>, <, >, <=, >=
Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.
好的，您可以下载免费的Altium Designer Viewer查看文档，有效期6个月。
好的，您可以下载免费的Altium Designer Viewer查看文档，有效期6个月。