创建原理图符号

Parent page: Building & Maintaining Your Components and Libraries

The schematic symbol typically includes a shape that can reflect the function of the component and one or more pins. How a component is represented, i.e. the look of the symbol and arrangement of component pins, is up to the designer. This should be done to comply with the requirements of your organization and the design standards you choose to adopt. One component symbol can represent the entire physical component, or the component can be defined by multiple sub-parts where each sub-part represents some logical entity within the physical component (e.g., each AND gate in a quad AND gate component, or the coil and contact sets in a relay). This type of component is also called a multi-part component.

Creating a New Schematic Symbol

Schematic symbols can be created directly in your connected Workspace:

1. Select File » New » Library from the main menus, then in the New Library dialog that opens, select Create Library Content » Symbol from the Workspace region of the dialog.

   
   Create a new Workspace Symbol using the New Library dialog

2. In the Create New Item dialog that opens, enter the required information, make sure that the Open for editing after creation option is enabled and click OK. The Workspace Symbol will be created, and the temporary schematic symbol editor will open, presenting a .SchLib document as the active document. This document will be named according to the Item-Revision, in the format: <Item><Revision>.SchLib (e.g., SYM-001-0001-1.SchLib). Use the document to define the symbol as described below.

   
   Example of editing the initial revision of a Workspace Symbol – the temporary schematic symbol editor provides the document with which to define your schematic symbol.

3. When the symbol is defined as required, save it to the Workspace using the Save to Server control to the right of the symbol's entry within the Projects panel. The Edit Revision dialog will appear, in which you can change Name, Description, and add release notes as required. The document and editor will close after saving.

A saved Workspace Symbol can be used when defining a component using the Component Editor in its Single Component Editing mode or Batch Component Editing mode.

Workspace Symbols can be browsed using the Components panel. Enable visibility of models by clicking the  button at the top of the panel and selecting Models, then select the Symbols category.

To edit a Workspace Symbol, right-click its entry in the Components panel and select the Edit command. Once again, the temporary editor will open, with the symbol opened for editing. Make changes as required, then save the document into the next revision of the Workspace Symbol.

Defining a Schematic Symbol

Schematic symbols are created by placing drawing objects to represent the component body and pins that represent the physical pins on the actual component. Schematic symbols are created in Altium Designer's schematic symbol editor.

Notes about symbol creation:

• Objects placed in the library editor are stacked in the order they are placed. Use the Edit » Move commands to change the display order if the pins become hidden behind the component body.
• Only one end of a pin is electrical. This end is referred to as the hotspot. Make sure the hotspot (the end by which you hold the pin) is away from the component body. Refer to the Pin object for more information.
• In the schematic library editor, the properties of the currently active symbol, such as the default designator and the description, are edited in the Properties panel in Symbol mode. The panel displays in this mode when nothing is selected. If you double-click on a primitive placed as part of the component symbol, the Properties panel will display the properties of that primitive rather than the parent component.
• The option used to display the designator and comment on the symbol editor sheet (Show Comment/Designator) is enabled/disabled for the current library in the Library Options mode of the Properties panel. Select the Tools » Document Options command to display the Properties panel in this mode.
• The fonts can be configured individually for each object as they are placed, or you can set your preferred fonts for new objects by editing each of the appropriate objects on the Schematic - Defaults page of the Preferences dialog.
• Install the Schematic Symbol Generation Tool extension to quickly build high-pin count components. The tool also supports importing pin details from a spreadsheet via the right-click menu.
• Multiple pins can be imported from a spreadsheet into the current symbol via the Smart Grid commands on the right-click menu in the SCHLIB List panel – learn more.

Preparing the Design Space

Always draw the component symbol close to the sheet origin (the center of the sheet). If necessary, relocate the origin of the sheet to the center of the design window by selecting Edit » Jump » Origin (shortcut J, O). Check the Status bar at the bottom left of the screen to confirm that you have the cursor at the origin. Components supplied by Altium are created around this point, marked with a crosshair through the center of the sheet. You should always create your components close to this origin. When you place a component on the schematic, the component will be 'held' by the electrical hot spot (pin end) that is nearest to this origin.

The default units for schematic and schematic library grids are imperial. Since all Altium components are designed on this imperial grid, it is important to appreciate the impact of deciding to switch to a metric sheet grid as it becomes difficult to correctly wire to components created on different grids. Note that imperial grids can be used with metric sheet sizes, such as A3, so it is not necessary to change to a metric grid when working with metric-sized sheets. The units for the current sheet are defined on the General tab in the General region of the Properties panel in Library Options mode (use the Tools » Document Options command from the main menus to access this mode of the Properties panel).

Use the General region of the Properties panel in Library Options mode to set the units for the current sheet.

If desired, enable the Show Comment/Designator option in the Properties panel to display the Comment/Designator strings for the current component in your library document.

Objects are placed on the current snap grid. The current grid is displayed at the bottom of the design space on the left-hand end of the Status bar.

The Snap Grid and Visible Grid can also be set in the Properties panel in Library Options mode. Rather than opening the Properties panel whenever you need to change the grid, you can press G to cycle the snap grid through the available settings. Available settings can be edited on the Schematic – Grids page of the Preferences dialog.

Properties Panel

When the active document is a Schematic Library document (*.SchLib), choose the Tools » Document Options command from the main menus – the Properties panel presents the Library Options. The following collapsible sections contain information about the options and controls available:

When a design object is selected, the panel will present options specific to that object type. The following table lists the object types available for placement within the library design space. Click a link to access the properties page for that object.

Creating the Schematic Symbol Body

After setting up the design space options as required, the next step is to capture the graphical representation of the component, i.e. to create the symbol graphics that will represent that component when placed on a schematic sheet. It is important to decide upon a standard for the graphical schematic symbols by which to adhere. This will provide a formal template when designing the symbol graphics and result in a guaranteed level of consistency. Altium's design methodology follows standard IEEE 315, which not only covers the most common circuit elements but also clearly defines how semiconductor elements can be combined to symbolize any number of silicon device types.

The body of the symbol is created by placing graphical design objects in the schematic library editor design space by using the Place menu, the Utilities bar, or the Active Bar. Double-click the placed schematic symbol to open the Properties panel to further define each shape.

Altium Designer includes a variety of closed symbol shapes including rectangle, polygon, ellipse, and round rectangle as shown below. 

Line-type shapes include arc, line/polyline, bezier, and elliptical arc. Lines/polylines can include arrowheads and tails. Double-click to open the Properties panel to define the heads and tails.  

Adding Pins to the Symbol

It is the component pins that give the component its electrical properties and define connection points on the component for directing signals in and out. A pin is placed to represent each pin on the actual physical component.

A pin can be added to the component that is currently visible in the schematic library document design space using one of the following methods. In each case, the pin appears floating on the cursor held by the electrical end. Rotate and/or flip the pin as required and click to effect placement.

• Use the Place » Pin command (or shortcut P, P).
• Click the  button on the design object drop-down of the Utilities toolbar.
• Click the  button on the Active Bar.
• With the Properties panel in Component mode (active when no object is selected in the design space), click the  button on the Pins tab to open the Component Pin Editor dialog. The dialog provides a single, convenient location for you to modify certain properties of any pin associated with the symbol. In addition to providing a means of editing pin properties, the dialog also allows you to add new pins or delete existing ones.

Access the Component Pin Editor dialog with which to manage all of the pins for your created symbol.

Configuring Pin Properties

Press Tab to open the Component mode of the Properties panel to edit the pin properties before placement. Numerical values will auto-increment on subsequent pin placements. Auto-increment behavior is configured in the Auto-Increment During Placement settings on the Schematic – General page of the Preferences dialog. Use negative values to auto-decrement.

Use the Schematic - General page of the Preferences dialog to define auto-increment behavior.  During placement or whenever a pin is moved, the pin is held by the electrical end (also called the hot end of the pin). The pin must be positioned so that the electrical end is away from the component body. Press the spacebar to rotate a pin while it is being moved.

Pins also can be placed to represent electro-mechanical points on the component, such as the tab on a voltage regulator.

A pin has a number of properties including a Name and a Designator. It is the pin Designator that is used to match the symbol pin to the PCB footprint pad. The default distance that the pin's Designator and Name appear from the end of the pin is a system-wide setting for the Schematic and Schematic Library editor. Configure the Pin Margin on the Schematic – General page of the Preferences dialog.

Individual settings for the Name can be configured in the Component Pin Editor dialog.

A pin has an Electrical Type that is used by Altium's electrical rules check system to verify that pin-to-pin connections are valid. Set this option in the Component Pin Editor dialog to suit the electrical type of that component pin. The default Pin Length should suit the chosen snap grid (typically 10 or 5). The default length is 30; typical lengths are 20 or 30.

Symbols can be added in the Component Pin Editor dialog to different positions of the Pin to represent electrical information from the pin.

Pasting Array

In addition to the standard cut, copy and paste commands, you can also use the Edit » Paste Array command from the main menus when creating a component symbol to place the current clipboard contents onto the current document, as a vertical or horizontal object array. This can be particularly useful when the component symbol being created should include multiple pins.

After launching the command, the Setup Paste Array dialog will appear.

The Setup Paste Array dialog

Set up the various options as required and click OK.

You will be prompted to select a start location on the document, where the array will be inserted. Simply position the cursor at the desired location and click or press Enter. The array will be pasted at the chosen start location.

Adding IEEE Symbols

For representing logic functions or devices, IEEE symbols can be used in a schematic symbol. These symbols enable users to understand the logic characteristics of these functions or devices without requiring specific knowledge of their internal characteristics.

The IEEE Symbols available for placement are shown in the image below.

Defining Symbol Properties

Symbol properties, such as the designator and description of the symbol, are edited in the Symbol mode of the Properties panel.

• Designator - enter the required designator prefix followed by a ?.
• Name and Description - these strings are helpful when symbol searches are performed.
• Type defines what type of component this symbol represents. Non-standard components, such as a company logo (Graphical) or a heatsink (Mechanical) can be created as schematic symbols and placed into a project.

The Component Type

In a design environment, you may also need to create design entities that are not necessarily components that will be mounted on the finished PCB. For example, there might be an external module that connects to the board that you would like to draw as a component and include on the schematic for design clarity but you do not want this to be included in the BOM for this board. Or there might be mechanical hardware, such as a heat sink and mounting screw that must be included in the BOM, but you do not want to include on the schematic.

These situations are managed by setting the component's Type. For the example just described, the component type could be set to Graphical. Another special class of components is a test point – this component is required on both the schematic and the PCB. It should be checked during design synchronization but is not required in the BOM. In this case, the component Type is set to Standard (No BOM).

For a non-standard type of component, set the Type accordingly.

As well as being used to determine if a component should be included in the BOM, the Type field is also used to determine how that component is managed during component synchronization. All of the Standard, Net Tie and Jumper Types are fully synchronized, meaning the component is passed from the schematic to the PCB and the net connectivity is checked. For the Mechanical and Graphical Type, the component is not passed from schematic to PCB. If a component with one of these types has been placed manually in the PCB and the matching Type option has been chosen, then component-level synchronization is performed but no net-level connectivity checks are performed.

Refer to the Component mode of the Properties panel for detailed information about the various Type options.

Breaking the Component into Multiple Parts

In some instances, it is more appropriate to divide the component into a number of symbols, each of which is referred to as a Part. Examples include resistor networks that contain eight individual resistors and each can be used independently of the others, the coil and contact sets in a relay, or each pin in a connector, for example, if you prefer to place connector pins throughout the sheet, rather than routing the wiring to a single connector symbol. Another example would be a 74F08SJX quadruple 2-input AND gate - in this device, there are four independent 2 input AND gates. While the component could be drawn as a single symbol showing all four gates, it would be more useful if it is drawn as four separate gates, where each gate can be placed independently of the others anywhere on the schematic.

These components are referred to as multi-part components. Each part is drawn individually in the schematic library editor and pins are added accordingly. The image below shows the same resistor network drawn as a single part then as four separate parts.

The same resistor network is shown as a single part on the left and as four separate parts on the right.

Notes on working with multi-part components:

• In the schematic symbol editor, use the Tools » New Part command from the main menus to add another part to the current component. Alternatively, click the  button on the Active Bar or right-click in the design space and choose Tools » New Part from the context menu. A new part is added to the component and a blank sheet for that part is opened and made active in the design window. Use this sheet to add the primitives that will constitute the part's graphical representation.

• Use the SCH Library panel to move between parts in a multi-part component, as shown below.

  

  You can also use the Tools » Next Part and Tools » Previous Part commands from the design space's right-click menu to show the next or the previous part.

• To remove the active part from the open multi-part component in the current document, choose Tools » Remove Part from the main menus or right-click and choose Tools » Remove Part from the context menu. You can also remove parts from a multi-part component directly from the SCH Library panel.

  Parts of components that have been removed cannot be restored by using the Undo command.
• If the component parts differ slightly, you can copy and paste the content between parts and update, for example, only the pin information in new parts.
• The schematic symbol editor allows an unlimited number of parts per component and each part may support different graphical representations, through the use of the component-level Alternate Display Mode feature.
• The designator of a multi-part component includes a suffix to identify each part. The suffix can be alpha or numeric and are set in the Alpha Numeric Suffix region on the Schematic - General page of the Preferences dialog. Note that this option is a software installation environment setting. It does not get stored in the library or the schematic file, and therefore, does not travel with the design files.

• Multi-part components are considered homogeneous, that is, all parts are equivalent during design annotation and can potentially be swapped during the annotation process. For example, a relay coil might be swapped with a set of relay contacts, depending on their relative locations on the schematic sheet. To lock a specific part in a placed component, enable the  in the Properties panel as shown below.

  

• During schematic annotation, the parts in a multi-part component are packed together to complete a component in accordance with the Matching Options configured in the Annotate dialog (as shown below). The enabled checkboxes on the left determine which component properties must match for parts to be eligible to be packed together. If you need to control the packing of specific parts so they are together in the same physical component, for example, a pair of op-amps in a filter design, and do not want to assign and lock them manually, add an additional parameter to that component and enter a value that defines which parts are to be packed together. The top image below shows the Annotate dialog matching options. The enabled parameters are used for multi-part component matching, the ResPack parameter has been added in the Properties panel (bottom image) to control the packaging of resistors into packages (when the parts have the same parameter value, they can be packaged together into the same physical component). Note the Strictly option. If this option is enabled, the parts must include this parameter to be packed together. Be careful of this option if you have different types of multi-part components that you are controlling the packaging of - all of them must include that parameter if Strictly is enabled.

  

  

• PCB part swapping can only be performed on a component whose parts are defined as a multi-part component. Learn more in the Pin Pair and Part Swapping document.
• To define the power pins, you can create an additional part for the component and place the VCC and GND pins on that part. Remember to enable the  option in the Properties panel to ensure that it cannot be swapped with any of the gates during re-annotation.

Display Modes - Multiple Presentations of the Same Component

The software supports different display representations of the same component. These representations can contain different graphical representations of the component, such as a DeMorgan or an IEEE representation. Or, for example, some of your customers might prefer to have their resistors drawn as a rectangle, while others prefer a wavy line.

Each of these representations is referred to as a display Mode. If an alternate view of a part has been added, it is displayed for editing in the schematic symbol editor by selecting the alternate mode from the Tools » Mode sub-menu in the main menus and the Mode drop-down in the Mode toolbar. The current graphical representation for the active component is denoted by an enabled 'tick' icon beside its entry in the main menus or the Mode drop-down list on the Mode toolbar. Note, however, that only the first 20 Alternate graphical modes are listed on the menu and toolbar.

In addition to selecting the normal or an alternate mode from the main menus or from the toolbar's drop-down, you can also use the Tools » Mode » Previous and Tools » Mode » Next commands from the main menus (the and buttons on the Mode toolbar) to show the previous/next mode for the active component.

A resistor created with two display modes. The library editor includes a Mode toolbar that can be used to add/remove and step through the modes.

To add an alternate view mode, with the component part displayed in the design window of the schematic symbol editor, select Tools » Mode » Add or click on the  button on the Mode toolbar. A blank sheet for Alternate N displays  (N is the next available number in the range 1-255). Typically, you would copy the part you created in the Normal mode and paste it into the new Alternate mode. Use Edit » Copy and Edit » Paste to copy and paste the Normal mode to the Alternate mode. This gives you the correct set of pins and you can modify the graphical elements and position the pins as required.

To rename the current alternate mode, choose the Tools » Mode » Rename command from the main menus or click Rename on the Mode toolbar. After launching the command, the Rename Alternate Representation dialog will appear. Enter the new name for the selected symbol and click OK. This alternate mode will then be represented with the defined name in the main menus and in the Mode toolbar.

To remove the current graphical representation (mode) for the active component, choose the Tools » Mode » Remove command from the main menus or click the button on the Mode toolbar. You can remove any of the graphical representations (Normal and Alternate) that exist for a component. If the component has one or more Alternate representations and you remove the Normal representation, the first Alternate (Alternate 1) will become the Normal representation. All other Alternates will be renumbered accordingly. If the component has no Alternate representations and you remove the Normal representation, the confirmation dialog will ask for confirmation to remove the component from the library - clicking Yes will effectively delete the component from the library.

The required mode is chosen when the component is placed from the library onto the schematic sheet using the Mode selector in the Graphical region of the Properties panel. The default placement mode is the mode that was displayed in the library editor when the library was last saved.

Generating a Component Report

The Component Report lists information about the active symbol.

1. Select Reports » Component (shortcut R, C).

2. A report titled <LibraryName>.cmp opens as the active document. The file includes the component name and the number of parts contained in the component. For each part, the pin details are given for each of the graphical representations (Normal and any Alternates).

   

3. Close the report to return to the schematic editor design space.

Support for Jumper Components

Jumpers, also referred to as wire links, allow you to replace routing with a Jumper component, which is often an essential ingredient to successfully designing a single-sided board. Altium Designer supports use of jumper components through a special component type of Jumper.

While you can start by placing the Jumper footprints directly onto the PCB, a suggested workflow starts at the schematic. To learn more, refer to the Working with Jumper Components section of the Creating a PCB Footprint page.

Using the Schematic Symbol Generation Tool

The task of creating a component library symbol and its pin data has become an increasingly involved undertaking as components have advanced in complexity. With current large-scale BGA devices requiring the placement and configuration of hundreds of pins, for example, substantial time and effort are often required to create viable component symbols.

To ease the workload associated with creating component symbols, Altium Designer provides an advanced Schematic Symbol Generation Tool, based on a symbol wizard interface and pin editor dialog. This features automatic symbol graphic generation, grid pin tables and smart data paste capabilities.

The Schematic Symbol Generation Tool is provided as a software extension - Schematic symbol generation tool - which must be installed to enable the tool’s features.

Extension Access

Functionality is provided courtesy of the Schematic symbol generation tool extension (a Software Extension).

The Schematic symbol generation tool extension.

The Symbol Wizard functionality can only be accessed provided the Schematic symbol generation tool extension is installed as part of your Altium Designer installation. This extension is installed by default when installing the software, but in case of an inadvertent uninstall, it can be found back on the Purchased tab of the Extensions & Updates page (accessed from the  drop-down then choose Extensions and Updates). If reinstalling, you will need to restart Altium Designer once the extension has been successfully downloaded and installed.

Creating a Symbol

The Schematic Symbol Generation Tool becomes available from the Schematic Library editor by choosing the Tools » Symbol Wizard command from the main menus. It can also be accessed when creating a Workspace component using the Component Editor in its Single Component Editing mode by clicking the drop-down icon on the button below the symbol model and selecting Wizard from the menu.

To create a new component symbol using the tool, first, add a new component to the active library document. The new symbol can then be developed through the tool's interface - the Symbol Wizard dialog - which opens when the command is launched. Use the dialog to interactively define the component symbol as required, including number of pins, layout of those pins, and pin data.

• Number of Pins - manually type or use the up and down arrows to increase or decrease the desired number of pins.
• Layout Style - choose from a set of predefined patterns for where the pin positioning is automatically assigned. Use the drop-down to select the preferred arrangement. The Preview image to the right and the data in the Side column will be updated accordingly. Selections include:
  • Dual in-line
  • Quad side 
  • Connector zig-zag 
  • Connector 
  • Single in-line 
  • Manual
    The Manual configuration denotes that pin positions are not automatically assigned. The layout style will revert to this setting when the pin positioning of a standard style (Quad side, Connector zig-zag, and Single in-line) has been edited.

Grid

• Position – the reference position index of a symbol pin. This data is not editable.
• Group – a manually entered string used to define a collective group of pins.

• Display Name – the component pin’s display name attribute string.

  Pin names entered with slashes will be recognized as alternate pin names and added to the generated symbol's pin properties. Note that use of the slash character to delimit each pin function is hard-coded, so if a pin name should contain a slash but without creating custom pin names for it (e.g., I/O), you can remove these extra pin names using the Pin mode of the Properties panel after creating the symbol.
• Designator – the pin’s designator attribute string. This will automatically match the pin Position by default.
• Electrical Type – use the drop-down in the field to select the electrical type for the pin. Selections include Input, I/O, Output, Open Collector, Passive, HiZ, Open Emitter, and Power.
• Description – the pin’s description string attribute.
• Side – use the drop-down in the field to select the position of the symbol. Select from Left, Bottom, Right, and Top. When this region has been changed, the Layout style setting changes to Manual.

Right-click Menu

• Move Up - use to move the selected data up one row.
• Move Down - use to move the selected data down one row.
• Copy - use to copy the selected data to the clipboard.
• Paste - use to paste the most recent data that was copied to the clipboard to the cursor position.
• Smart Paste - use to open the Pin Data Smart Paste dialog to copy several columns of external source data into matching columns in the grid. Use the dialog to configure the column data and delimiters, then click Paste. Learn more about Smart Paste.
• Clear - use to delete the pin data.

Preview

This region displays a preview of the symbol graphic and dynamically represents the current settings and pin data. Use the slider bar or - and + to zoom in/out on the graphic.

Additional Controls

• Continue editing after placement - if checked, the dialog will remain active (allowing further editing) once the component has been placed.
• Place - use to place the completed symbol and pin data. Choices include:
  • Place Symbol
  • Place New Symbol
  • Place New Part

Pasting Pin Data

While the pin data in the table can be edited to a common value for multiple cells, the dialog's Paste and Smart Paste features provide an advanced way to populate all cell data by bringing in large amounts of different data from external sources.

Within the table, standard copy and paste techniques can be used to populate data from one group of cells to another. For example, by selecting three cells in a column, copying the data (right-click - Copy), then selecting three target cells to paste into (right-click - Paste).

The same technique can be used to copy and paste a data selection from an external source, such as a spreadsheet, text file, or PDF file.

An example of pasting data copied from an external spreadsheet, into the Pin data table.

Smart Paste

Beyond standard copy and paste techniques, Smart Paste offers the capability to populate multiple columns of data from an external source, using an automated column mapping approach.

To copy several columns of source data into matching columns in the Pin data table, right-click in the table and choose the Smart Paste command from the context menu. This opens the Pin Data Smart Paste dialog, which will be populated with the source data. A range of data delimiters are available, which can be selected to match the delimiters used in the source data.

The Pin Data Smart Paste dialog

Symbol Placement

With its settings and pin data configured as required, the symbol can then be placed into the design space for the active library component. Placement can be in terms of a single component, or as one section of a multi-part component, using the respective commands available from the context menu associated to the dialog's Place button. Note that if the Continue editing after placement option is enabled, the Symbol Wizard dialog will remain active (allowing further editing) once the component/part has been placed.

Accelerating Schematic Symbol Creation with the Smart Grid Insert Tool

The Smart Grid Insert tool available in the SCHLIB List panel lets you map current clipboard data to Altium Designer object properties. These tools greatly simplify the schematic symbol creation process and in a few steps you can create the pins of a component directly from external data like a spreadsheet, a PDF, or an ASCII file.

While you could copy straight from the source pin data into Altium Designer, it is worth doing a small amount of preparatory work to achieve an optimal result. A spreadsheet is the right place to do that. Typically you will only need to perform a few steps, including:

• Adding a header row to make the column-to-column mapping easier. Don’t worry about getting the column names exactly the same, Altium Designer does a good job of automatically inferring the correct mapping.
• Adding an Object Kind column, so that Altium Designer knows that it is has to create pin-type objects.
• Adding a Type column, to specify each pin’s electrical type.
• Including X and Y pin locations. Spreadsheets have excellent tools for filling cells with values, for example if you right-click and drag to select a set of cells in Microsoft Excel, you can specify the numeric series you want, making it easy to space the pins out in the schematic library.

High-pin count and regularly sectioned components, such as FPGAs, lend themselves to implementation as multipart components in Altium Designer. The easiest way to do that is to create all the pins in the first part of the Altium Designer component, and then cut and paste the blocks of pins to the other parts.

To get the pins into neat, part-ready groups, try leaving a couple of empty rows between the pins for each part in the spreadsheet. Not only does it make it easy to see where you might need to restart coordinate values, you can also automatically add X, Y values to a large selection and then remove the redundant X, Y values in the empty rows. This will result in no pins in those deleted locations, neatly spacing the part-ready groups.

Use the tools in the spreadsheet to add suitable X and Y coordinates for the pins.

Select and copy the required cells in your spreadsheet. Don’t worry if there are columns in the selection that you don’t need, the Smart Grid tools can ignore these.

In Altium Designer, right-click in the SCHLIB List panel and select Smart Grid Insert from the menu to open the Smart Grid Insert dialog. If your source data includes a header row Altium Designer will attempt to automatically identify the object kind, then build a list of created objects. A point to keep in mind, before you map columns the list of created objects will have the properties of the current Altium Designer default pin object. So for example, if you wanted all the pins placed at 180 degrees with a length of 20, then set the default values in Altium Designer before starting the smart grid process. That way you don’t need to worry about adding those settings into the spreadsheet, or editing them in Altium Designer after the creation process. Not sure how to set the defaults? Just select Place » Pin from the menus, then before you place a pin press Tab to edit the default values, then place and delete that one pin.

Another big advantage of including a header row is that you get to use the Automatically Determine Paste button. This is a great feature – it will search and compare fields in the created object against source data column titles, and make intelligent choices about how they should be mapped. Don’t worry if the automatic feature gets one wrong, you can use the Undo Paste button to undo a mapped column. To manually map, select a column in the source data and its corresponding column in the created objects, then click the Paste Column button.

As soon as you click OK, the set of created objects will appear in the design space. Add a suitable body to each part, then cut and paste to create the individual parts, and your symbol is ready.

 
The Smart Grid Inserted pins, and the parts with the component bodies added.