Part. Summary. Modified by Susan Riege on Aug 5, Parent page: Objects

Transcription

1 Part Old Content - visit altium.com/documentation Modified by Susan Riege on Aug 5, 2016 Parent page: Objects Related Resources Net Ties and How to Use Them (PDF) The Part represents the actual physical electronic component. Summary A part is an electrical design primitive. It is a schematic symbol that represents an electronic device, such as a resistor, a switch, an operational amplifier, a voltage regulator, and so on. Parts are stored within components in schematic component libraries. Note that each component can contain one or more parts. As well as a symbolic representation of the component, the part also includes links to models, such as the PCB footprint; and also parameters, used to document detail such as component parameters, supplier information, and so on. How the model links and parameters are added to the part depends on the type of library storage being used. The terms Part and Component are both used to describe the symbol that represents the actual electronic device. The term Part is used because some components contain multiple parts, for example a quad Op Amp component contains 4 separate Op Amps, or a resistor network can contain 8 independent resistors - for these types of devices the designer can create a separate schematic symbol to represent each Part during the component definition, and place each of these parts independently. In this article the terms Part and Component are used interchangeably, unless a multi-part component is being discussed.

2 Availability Parts are available for placement in the Schematic editor only. Use one of the following methods to place a part: Place a part from the Libraries panel, using the Place <ComponentName> button. Click Library tab on the right edge of the schematic editor to display the panel. In schematic editor, click Place» Part Place a part from within the Schematic Library editor, using the Place button in the SCH Library panel. Placement The way in which a part is placed on a schematic sheet depends on how, and from where, placement mode is invoked. Schematic components (and PCB component footprints) can only be placed from Available Libraries. The term Available Libraries includes libraries that are part of the current project being worked on, or libraries currently installed in CircuitStudio - the currently Available Libraries are listed in the Libraries panel. Libraries can be installed and removed via: the Data Management - Installed Libraries page of the Preferences dialog, or the Available Libraries dialog (click the Libraries button on the Libraries panel to open it). Placing from the Libraries Panel In the Schematic editor, the part selection and placement process is done from the Libraries panel (shown below). If the panel is not visible, click System» Library to display it. Note that: The panel displays the contents of the currently selected library, use the dropdown next to the library name to choose another library. Use the mask field (below the currently selected library field) to filter the list and speed the searching process, or scroll and select the required part. Click the Libraries button to open the Available Libraries dialog and add or remove libraries. Click the Search button to open the Libraries Search dialog and search for a part. Click the Place button, double-click, or click and drag to place the selected component onto the active schematic sheet. While the part is floating on the cursor, it can be rotated (press Spacebar), mirrored along an axis (press X or Y), or edited (press Tab) before placement. The columns shown in the list of components in the currently selected library can be reorganized (click and drag) or reconfigured. Right-click and choose Select Columns to do this.

3 The selected Part is about to be placed from the Libraries panel. Searching for a Component If you cannot locate the required part in the Libraries panel, use the Search feature. To do this, click the Search button to open the Libraries Search dialog (as shown below). Note that: The default search Scope is to search for Components in the Available Libraries (as shown by the Scope options in the image below). Alternatively, the Libraries Search dialog also supports searching through Libraries on a path, stored in folders on a drive. To do this enable the Libraries on Path option, then configure the Path options as required. The Filters are logically AND'ed, it can be better to start with a simpler filter and then if there are many results, use the Refine last search mode to search within the results. Search results are presented in the Libraries panel, clustered under Query Results. Re-select a component library to return to browsing in the panel.

4 Search for the Part in the Available libraries, or search Libraries on a path. Placing from the Schematic Library Editor A part can also be placed directly from a library that is open the Schematic Library editor. This is done from the SCH Library panel, as shown below. If the panel is not visible, click the SCH button down the bottom right of the workspace to enable it. Note that: Clicking the Place button in the panel will place the selected part (component) in the last-active schematic sheet. While the part is floating on the cursor, it can be rotated (press Spacebar), mirrored along an axis (press X or Y), or edited (press Tab) before placement. If a part is placed directly from a library, that library does not need to be added in the Available Libraries dialog first.

5 A Part can also be placed directly from an open Schematic Library, using the SCH Library panel. Non-Graphical Editing The following methods of non-graphical editing are available:...via an Associated Properties Dialog This method of editing uses the following dialog to modify the properties of a part object.

6 Edit the properties of the Component (Part) in the Properties for Schematic Component dialog. The Properties for Schematic Component dialog can be accessed prior to entering placement mode, from the Schematic Default Primitives page of the Preferences dialog. This allows the default properties for the part object to be changed, which will be applied when placing subsequent parts. During placement, the dialog can be accessed by pressing the Tab key. After placement, the dialog can be accessed in one of the following ways: Double-clicking on the placed part object. Placing the cursor over the part object, right-clicking and choosing Properties from the context menu. The following sections provide an overview of each of the specific regions of the dialog: Properties

7 This section of the dialog contains editable fields for the component Designator, Comment and Description. Typically the designator is left unassigned until the design is complete, then all designators are allocated on a positional basis using the Annotate command. The arrow buttons located between the Comment and Description fields are used to select a different part in a multi-part component. The Locked check boxes allow the Designator and the component sub-part to be locked from the annoation commands. The Unique Id field is automatically assigned when a schematic component is placed, it does not need to be manually edited. It is this field that is used to link the schematic symbol to the PCB component, allowing designator changes to easily flow between the schematic and PCB. If required, a new Unique Id can be assigned by clicking the Reset button. Note that when a part is copied and pasted the Unique Id is automatically reset. The Type field specifies the type of component being used. The following types are available: 1. Standard - this type of component possesses standard electrical properties. They are always synchronized to the PCB and are always included in the BOM. This is the default type for a new component. 2. Standard (No BOM) - this type of component possesses standard electrical properties. They are always synchronized to the PCB but are not included in the BOM. 3. Mechanical - this is a non-electrical mechanical component, for example a heat sink or mounting bracket. Any net connectivity is synchronized (by component designator) if they exist on both the schematic and PCB, and they are always included in the BOM. Note that the PCB part must be placed manually, it is not automatically placed during initial design transfer. 4. Graphical - this is a non-electrical component used for creating graphical objects on the schematic, for example a company logo. This type is never synchronized and not included in the BOM. 5. Net Tie (In BOM) - this type of component allows two (or more) nets to be connected together, for example a digital ground and an analog ground that must be connected at a specific location on the schematic and in the PCB routing. They are always synchronized to the PCB and are always included in the BOM. Use this Type of Net Tie if a jumper type component is to be fitted as part of the assembly process. When placing components of this Type, use the Verify Shorting Copper option in the Design Rule Checker dialog when performing a DRC in the PCB, to verify the short correctly exists. 6. Net Tie - as above, but used where the net tie-point is to be part of the routing. They are always synchronized to the PCB but are not included in the BOM. When placing components of this Type, use the Verify Shorting Copper option in the Design Rule Checker dialog when performing a DRC in the PCB, to verify the short correctly exists.

8 Link to Library Component Graphical This section of the dialog details the name of the component (Design Item ID) and the Library Name that it was placed from. For certain library types it can also detail the Table Name it was placed from. Use the Choose button to access the Browse Libraries dialog, from where you can choose a different part for this component on the schematic. This section of the dialog defines the Location and Orientation of the component on the schematic sheet, and also if the component is Mirrored or has it's location Locked. Enable the Local Colors option to change the colors of the objects used in this instance of the component. Clear the Lock Pins option to move pins on this instance of the component. Enable the Show All Pins on Sheet option to display any hidden pins the component may have. Hidden pins are typically only used for power pins, which are automatically connected to a net of the same name as the pin during netlisting. It is possible to create different visual presentations of the same component in the Schematic Library editor. Each presentation is called a Mode, with the default Mode being called Normal. Note that each mode must have the same set of pins. Use the Mode dropdown to select an alternate display presentation in the Schematic editor. Parameters List

9 This section of the dialog is used to add Parameter information to the component. Parameters are used to add additional component information, such as the wattage, the tolerance, the component manufacturer, the date the component was created, and so on. Use the buttons to Add, Remove and Edit the parameters. PCB design rules can be included on the schematic by attaching them as parameters to the appropriate schematic object. Use the Add as Rule button to add a component-level design rule directive to this component. When the schematic is synchronized with the PCB the chosen rule will be added in the PCB Design Rules dialog, component-level rules will have a PCB rule scope of InComponent('<ComponentDesignator>'). Models List This section of the dialog is used to define links to the following model types: Footprint Simulation You can add any number of new model links or edit/remove existing ones. Click the Add button to open the Add New Model dialog, where the Model Type is selected. If multiple models of the same type have been added, use the dropdown in the Name column to select which model is to be used. To edit an underlying model definition, select the entry for the link and click the Edit button, or double-click on the entry. The dialog that appears will depend on the type of model you are editing. While models can be added after the component has been placed on the schematic, it is more efficient to add them in the library as part of the component definition.

10 ...via an Inspector Panel An Inspector panel enables the designer to interrogate and edit the properties of one or more design objects in the active 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....via a List Panel A List panel allows the designer to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering, it enables the display of just those objects falling under the scope of the active filter allowing the designer to target and edit multiple design objects with greater accuracy and efficiency. Graphical Editing Graphical part editing is limited to moving, rotating and mirroring. When a part is selected in the workspace, a dashed selection box will appear around it. For each text field associated with the part (Designator, Comment, plus any visible user-defined parameters) a dashed line will be visible, connecting the text field to the body of the part, indicating association. To graphically manipulate a selected component: Press Delete to remove the selected part from the design. Click and hold to move the selected part, the cursor will jump to the nearest electrical hotspot (the wiring end of the nearest pin). While a part is moving on the cursor press the Spacebar to rotate it (Shift+Spacebar to rotate in the other direction). While a part is moving on the cursor press the X or Y key to mirror it along that axis. Click once to select a Component (Part) then click and hold to move it. Press the Spacebar to rotate while moving. When a component is rotated, its text strings are automatically repositioned to suit the new orientation. This behavior can be disabled if required, edit the string and clear the Autoposition checkbox. Note that manually positioned text strings are denoted by a dot,

11 these dots can be hidden if required by clearing the Mark Manual Parameters option in the Schematic - General Editing page of the Preferences dialog. If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the Schematic Graphical Editing page of the Preferences dialog, and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double click on the locked object directly and disable the Locked property or disable the Protect Locked Objects option, to graphically edit the object. Working between the Schematic Component and the PCB Component The software includes tools to help work between the component on the schematic and that same component on the PCB. These tools include: Cross Probing, Cross Selection, and Selecting the PCB Components from the schematic. Cross Probe As the name implies, Cross Probe allows you to click on a component in one editor, and jump to that component in the other editor. To Cross Probe: Click the Cross Probe button, located on the Schematic editor menu at Tools» Cross Probe, and the PCB editor menu at Tools» Cross Probe. When you click the component in the schematic editor it will be centered and zoomed in the PCB editor. Note that the zoom level is set in the System - Navigation page of the Preferences dialog. The default behavior is to remain in the same editor, ready to cross probe another component. To switch to the other editor as you Cross Probe, hold the Ctrl key. Cross probing from the schematic component to locate that component on the PCB (click to enlarge the image). Cross Select Mode Cross Select Mode simply selects the same component in the other editor. Note that it does not zoom and center. Cross Selection is a mode, it is either on or off. To enable Cross Selection:

12 Click the tools menu and toggle Cross Select Mode, located on both editor at Tools» Cross Select Mode. Select multiple components by holding the Shift key as you click to select. Selecting the PCB Components This feature allows you to select multiple schematic components in a specific order, then place those same components in the PCB editor, in the same order. To use this feature: Select the components on the schematic one by one (hold Shift as you click to build up the selection). Switch to the PCB editor and press the I, C shortcuts to launch the Reposition Selected Components command. Source URL: