Contents
The Summer 09 release of Altium Designer heralds the arrival of graphical editing with respect to assembly variants and board-level annotations. Performed from within the compiled document views of the source schematic documents, this feature enables you to make changes in-situ quickly, efficiently, but more importantly, visually – providing a faster and more intuitive alternative to the Assembly Variants and Board-Level Annotation dialogs.
Compilation is the Key
Related article: The Editor View and the Compiled Documents View
Graphical editing of assembly variant and board-level annotation information can only be carried out from the 'compiled document' view of schematic documents. This view appears as one or more tabs alongside the Editor tab of your schematic, after your project is compiled. If the sheet is used only once in your project, there will be just one compiled document tab. If the sheet is instantiated multiple times in your project (for example, if you use Multi-Channel Design or Device Sheets), then there can be more than one compiled document tab.
It is critical to remember that the Editor tab is where you edit your logical document. Any changes you make here (for example, changing the properties of a logical component or a logical designator) will be saved to the schematic document (*.SchDoc). The compiled document tabs, however, are where you edit the physical state of the compiled project. Any changes you make here (for example, setting a particular instance of a component as not fitted in a variant, or locking a physical designator) will be saved to the project file (*.PrjPcb) and/or annotation file (*.Annotation) file respectively.
So to edit your assembly variants and board-level annotations graphically, you must first compile your project. After compilation, click on the required compiled document tab of the schematic sheet upon which changes are to be made. Only those objects that can be edited graphically on the compiled sheet will be available, with all other objects being filtered and rendered unavailable for selection and editing. The dim level for the uneditable objects is controlled through use of a slider bar, which can be found on the Schematic – Compiler page of the Preferences dialog (DXP»Preferences).
Example compiled view of a schematic document - masking ensures only those objects that can be edited graphically, are available to do so. Use the available slider bar to control dimming of the uneditable objects.
Editing of Variant Information
Related article: Managing Design Variation with Variants
The ability to graphically edit the components for an assembly variant of a design directly, and visually, in the workspace, provides a more efficient and intuitive way in which to make changes to individual components. This complements well, the traditional Assembly Variant Management dialog (Project»Assembly Variants) – used to add new variants for a project and from where batch changes to multiple components can be performed.
The concepts of assembly variants remain the same – the graphical editing does not introduce anything different from that respect. Think of the graphical editing more as a powerful, visual addition to your variant-editing arsenal!
All changes made to an assembly variant using the graphical editing features will be reflected in the Assembly Variant Management dialog when it is next accessed. Changes are stored in the project file.
Quick access to the Assembly Variant Management dialog is provided using the 
button, on the Assembly Variants toolbar.
Choosing which Assembly Variant to Use
Before you can start editing the components for an assembly variant, you need to first choose which variant you want to make changes to! Selection of an existing assembly variant of your design is performed from the Assembly Variants toolbar. Simply choose the required assembly variant from the list.
Use the Assembly Variants toolbar to
select the assembly variant for which
you wish to view and make changes.
Essentially, you are choosing which variant to 'view' and potentially modify. Changes made, on the compiled document views of schematic source sheets, affect just the chosen assembly variant.
Although, when editing, a Schematic document is focused, when you're on the compiled document view you are actually editing the project, and not the schematic document. Anything used to edit the schematic document (panels, scripts, etc..) continue to edit the schematic document, and not the variant information.
Direct Output Generation
The choice of assembly variant from the Assembly Variants toolbar is a project-wide setting. Not only can you make changes to that variant on the schematic compiled document view(s), you will also be able to generate output for that variant directly, using commands from the Schematic and PCB Editors, as an alternative to generation solely from an Output Job Configuration file (*.OutJob).
The following output can be generated directly from the Schematic Editor, based on the chosen assembly variant:
- Schematic Prints (File»Print)
- All Report outputs (from the Reports menu)
The following output can be generated directly from the PCB Editor, based on the chosen assembly variant:
- Assembly drawings (File»Assembly Outputs»Assembly Drawings)
- Pick and Place files (File»Assembly Outputs»Generates pick and place files)
- Testpoint report (File»Assembly Outputs»Test Point Report)
- Bill of Materials for PCB document (Reports»Bill of Materials)
- All project-based reports (from the Reports»Project Reports sub-menu)
Leaving the entry at [No Variation] will mean that any changes made to schematics, or output that is generated directly from them, uses the base design. With this setting, you will only be able to change board-level annotations from the compiled document views.
Graphically Editing Component Inclusion
A command is provided to quickly toggle the Fitted or Not Fitted state of a component for the variant design. Launch this command using the 
button, located on the Assembly Variants toolbar. Simply click the button – the cursor will change to a cross-hair – then click on a component in the workspace to toggle its state between fitted or not fitted.
Those components set as not fitted will be displayed in accordance with options defined in the Schematic Drawing Options region of the Variant Options dialog. Access to this dialog is made from the Variant Drawing Style button in the main Assembly Variant Management dialog. The latter can be quickly accessed using the button, on the Assembly Variants toolbar.
Quickly determine which components are to be fitted or not for the variant, directly in the workspace!
Graphically Varying Component Parameters
You can make changes to the values of component parameters in an assembly variant, including the Comment parameter, simply by editing a displayed value, directly from within the compiled document view of the source schematic.
In-place editing of parameter values is only possible provided the Enable In-Place Editing option is enabled, on the Schematic – General page of the Preferences dialog (DXP»Preferences).
The appearance of any varied parameters can be modified using options available in the Variant Options dialog. Access to this dialog is made from the Menu button in the main Assembly Variant Management dialog, which can be quickly accessed using the button, on the Assembly Variants toolbar.
Simply enable the Modify Text and Font option to use this feature. The options allow you to modify the font and color of the parameter/value text and also add a textual suffix if required. The preview window of the dialog will reflect how the parameter text will appear.
Define how varied parameters will be displayed in a compiled document view and any prints.
Specified options will be applied to all varied parameters. The following image illustrates use of these varied parameter display options in action. In this case, the font remains unchanged (from the default), but a new color has been chosen, together with the suffix Hi-Speed.
With in-place editing, varying component parameter values for an assembly variant is made easy. Applied display options enable you to quickly assess which
parameters have been varied, without having to refer to a dialog!
Component parameters and/or their values, including the Comment field, will need to be made visible within the base design schematic (from the Editor tab), in order to 'see' and graphically edit them in a compiled document view.
Additional Non-Graphical Editing
In addition to the graphical editing abilities for an assembly variant, there are also associated dialogs for the component and parameter objects, allowing you to edit variant information at the component- and parameter-levels.
Component Editing
Double-clicking on a component will give access to the Physical Component Properties dialog. Provided you have selected an assembly variant from the Assembly Variants toolbar, the dialog will present options for Variation and board-level Annotation.
Component variation can be performed, non-graphically, at the individual component-level.
Use the dialog, from a variant perspective, to make changes for that single component only – whether or not it is fitted, and any required variations to the component's Comment, Description and other parameters. Changes made will be reflected in the workspace, in accordance with defined display options.
The ability to quickly update varied parameter values from an existing library component, is provided courtesy of the Choose Values button. Click this button to access the Browse Libraries dialog, from where you can search for the component to be used.
The Comment field is used to define the use of an alternate part, or different value for the same part. Note however, that whole part substitution is not supported. Graphically, the component will appear no different in the compiled document view or subsequently generated prints/drawings.
Parameter Editing
Double-clicking on a component parameter will give access to the Parameter Variation dialog.
Individual parameter-level variation.
Use the dialog to make changes for that single parameter only. The varied parameter will be reflected in the workspace, in accordance with defined display options for parameters that differ in some way from those for the component in the base design.
Editing of Board-Level Annotation Information.
Related article: Understanding Design Annotation
Board-level annotation is the process of annotating the compiled components (the physical view of the components) of your design, through the Schematic Editor. The ability to graphically edit the physical designators for components – directly from the compiled document view – provides a more efficient and intuitive way in which to make changes to individual component designators. This complements well, the traditional Board Level Annotate dialog (Tools»Board Level Annotate) – from where batch annotation changes to multiple components can be performed.
Board-level annotation is enabled through the existence of an Annotation file (*.Annotation) in the project. All annotation changes are stored in this file.
All changes made to physical designators using the graphical editing feature will be reflected in the Board Level Annotate dialog when it is next accessed.
Graphically Changing Physical Designators
To change a component's physical designator, directly within the compiled document view of a source schematic, simply click once on the designator to focus it, then click again to begin editing. Once done, either click away from the designator field or press Enter. That's all there is to it!
Graphical editing of physical designators - fast and efficient and not an ECO in sight!
In-place editing of designators is essentially a graphical shortcut to getting a Locked Physical Designator. To annotate using a defined Naming Scheme, you will need to use the controls found in the associated dialog for a component or designator (see the next section on Additional Non-Graphical Editing).
Also, in-place editing of designators is only possible provided the Enable In-Place Editing option is enabled, on the Schematic – General page of the Preferences dialog (DXP»Preferences).
Additional Non-Graphical Editing
In addition to direct graphical editing of physical (compiled component) designators, there are also associated dialogs for the component and designator objects, in which you can define the annotation required. Double-click on a component or its designator, to access the Physical Component Properties and Designator Annotation dialogs respectively.
Non-graphical editing of physical designators.
The annotation-based content of these dialogs is identical. If an assembly variant is chosen, from the Assembly Variants toolbar, the Physical Component Properties dialog will also contain a region dedicated to Variation.
Use the options to specify either:
- A custom designator, using the Lock Physical Designator option and entering the designator required. This is the option that is set when graphically editing a designator.
- A designator generated using a specified naming scheme. In this case, simply enable the Apply Naming Scheme option and use the Annotate Options button to access the Board Level Annotation Options dialog. From here, you can either choose a predefined naming scheme, or specify your own, custom scheme. The Physical designator will be generated based on the logical designator information and the specified naming scheme.
Use a predefined naming scheme, or your own custom scheme, to generate a physical designator.
The resulting annotation will be reflected in the workspace.
The options defined in the Board Level Annotation Options dialog, when defining a naming scheme, are global to the project and override the naming scheme defined on the Multi-Channel tab of the Options for Project dialog (Project»Project Options).