Parent page: Tutorial - A Complete Design Walkthrough with Altium Designer
Placing from the Components Panel onto the Schematic
When Altium Designer is connected to a Workspace, the Components panel will list all components
available for use in a project design, from this Workspace. For such components, the Components panel supports the same search features that are available in the Manufacturer Part Search panel, including string-based searching, faceted
searching, or a combination of both, and also the Find Similar Components feature.
To open the Components panel, click the Components from the menu.
The panel’s Categories pane (or the drop-down menu in panel's compact mode) lists available Workspace library components under the All category entry. When the panel is in its normal mode, click the Categories list icon « icon to collapse or expand the display
of the list. The structure of categories reflects component types currently defined on the connected Workspace (use the Data Management – Component Types page of the Preferences dialog for viewing
and managing Component Types).
The Components panel being used to browse components stored in a Workspace.
To place a component from the panel, you can:
Click the Place button in the Component Details pane – the cursor automatically moves to be within the bounds of the schematic sheet and the component appears floating on the cursor; position it and
click to place. After placing a component, another instance of the same component will appear on the cursor; right-click to drop out of placement mode.
Right-click on the component and select Place from the context menu. The component appears floating on the cursor; position it and click to place. Note that if the panel is floating over the design space, it will fade to allow
you to see the schematic and place the component. After placing a component, another instance of the same component will appear on the cursor; right-click to drop out of placement mode.
Click, Hold&Drag – click and drag the component from the grid region of the panel onto a schematic sheet. This mode requires that the cursor is held down; the component is placed when the cursor is released. Using this technique
only one component is placed. After placing the component, you are free to select another component or another command.
Placement Tips
While the component is floating on the cursor, you can:
Press Spacebar to rotate it counterclockwise in 90º increments.
Press X to flip it along the X-axis; press Y to flip it along the Y-axis.
Press Tab to display the Properties panel and edit the properties of an object prior to placement. The values entered become the defaults. If the designator has the same prefix, it will be auto-incremented.
During component placement, the software will automatically pan if you touch the window edge. Autopanning is configured in the Schematic – Graphical Editing page of the Preferences dialog.
If you accidentally pan beyond where you want, while the component is floating on the cursor you can:
Ctrl+Mouse Wheel to zoom out and in again, orRight-Click, Hold&Drag to slide the schematic around, orCtrl+PgDn to display the entire sheet again.
If the Components panel is floating over the schematic sheet when you place a part, it will automatically become transparent whenever the cursor+component gets close to it. The transparency of floating panels is configured in the System – Transparency page of the Preferences dialog. Alternatively, all floating panels can be hidden/displayed at any time (while running a command or not) by pressing the F4 shortcut.
► Learn more about Schematic Placement & Editing Techniques
Working with the Properties panel during Placement
During object placement, if you press Tab the editing process will pause and the interactive Properties panel in its appropriate mode will open. The default behavior is for the most commonly edited field to be highlighted,
ready for editing. Because the editing process is paused, you can use the cursor (or press Tab on the keyboard) to move to another field in the panel.
When you have finished editing, click the Pause button ( ) as shown in the image below to return to object placement. Alternatively, press Enter to finish object editing and return to object placement.
Editing is paused when you press Tab during placement – click the Pause icon on the screen to return to placing the component.
Placing the Multivibrator Parts
With the Components panel, components acquired from Manufacturer Part Search will be placed in the Multivibrator circuit. Once you have placed the components, the schematic should look like the image below.
You can proceed to find and place the components. Note that the collapsible sections below include tips on editing during placement, which is more efficient than editing after placement. If you choose to leave the editing until after the components are
placed, click to select the component and edit it in the Properties panel.
All the components have been placed, ready for wiring.
Placing the Transistors
Select View » Fit Document from the main menus (shortcut: V, D ) to ensure your schematic sheet takes up the full editing window.
Open the Components panel if not already – click the Components from the menu.
Click the Components panel and select Refresh from the menu to update the panel's content with the components acquired from Manufacturer Part Search.
Use panel's Search field to search for: transistor BC547.
Display the Component Details pane of the panel using the
Click to select the required transistor in the results grid in the panel then click the Place button (as shown below). The cursor will change to a crosshair and you will have a symbol of the transistor floating on your
cursor. You are now in part placement mode. If you move the cursor around, the transistor will move with it.
Do not place the transistor yet!
Before placing the part on the schematic, you can edit its properties, which can be done for any object floating on the cursor. While the transistor is still floating on the cursor, press the Tab key to open the Properties panel. The default behavior is to automatically highlight the most-used field in the panel, ready for editing; in this case, it will be the Designator. Note that each section of the panel can be individually expanded or collapsed,
which means your panel might look different.
Set the Designator to Q1, and the Comment to be visible.
In the Properties section of the panel, type in the Designator Q1.
Confirm that the visibility control for the Comment field is set to visible (
Leave all other fields at their default values then click the Pause button ( ) to return to part placement.
Move the cursor, with the transistor symbol attached, to position the transistor a little to the left of the middle of the sheet. Note the current snap grid, which is displayed on the left of the Status Bar at the bottom of the application window.
It is 100mil; you can press the G shortcut to cycle through the available grid settings during object placement. It is strongly advised to keep the snap grid at 100mil or 50mil to keep the circuit neat and make
it easy to attach wires to pins. For a simple design such as this, 100mil is a good choice.
Once you are happy with the transistor's location, click the left mouse button or press Enter on the keyboard to place the transistor onto the schematic. The location can be changed later if required.
Move the cursor and you will find that a copy of the transistor has been placed on the schematic sheet, and you are still in part placement mode with the transistor symbol floating on the cursor. This feature allows you to place multiple
parts of the same type.
You are ready to place the second transistor. This transistor is the same as the previous one so there is no need to edit its attributes before you place it. The software will automatically increment the component designator when you place
multiple instances of the same part. In this case, the next transistor will automatically be designated Q2.
If you refer to the schematic diagram shown above, you will notice that Q2 is drawn as a mirror of Q1. To horizontally flip the orientation of the transistor floating on the cursor, press the X key on the keyboard. This flips
the component along the X axis.
Move the cursor to position the part to the right of Q1. To position the component more accurately, press the PgUp key twice to zoom in two steps. You should now be able to see the grid lines.
Once you have positioned the part, click the click the left mouse button or press Enter to place Q2. Once again a copy of the transistor you are "holding" will be placed on the schematic and the next transistor will be floating
on the cursor ready to be placed.
Since both of the transistors have been placed, exit part placement mode by clicking the right mouse button or pressing the Esc key. The cursor will revert back to a standard arrow.
Placing the Capacitors
Return to the Components panel and search for: capacitor 22nF 16V 0603.
Select the found capacitor in the search result grid, right-click on it then select Place from the context menu.
While the capacitor is floating on the cursor, press the Tab key to open the Properties panel.
In the General section of the panel, type in the Designator C1.
Expand the Parameters section of the Properties panel and open the Value drop-down of the Footprint entry. Many of the resistors and capacitors have several footprint models, for
different density levels. Select the A variety as shown in the image below.
Using visibility controls in the Parameters section of the panel, enable the visibility of the Capacitance parameter and disable the visibility of other parameters. Value of the Capacitance parameter
will be shown next to the component in the design space.
Click the Show More link in the panel's Parameters region to show the full list of component parameters.
Leave the other fields at their default values and click the Pause button ( ) to return to part placement; the capacitor will be floating on the cursor.
Press the Spacebar to rotate the component in 90° increments until it has the correct orientation.
Position the capacitor above the transistors (refer to the schematic diagram shown earlier) and click the left mouse button or press Enter to place the part.
Position and place capacitor C2.
Right-click or press Esc to exit the part placement mode.
Placing the Resistors
In the Components panel, search for: resistor 100K 5% 0805.
Select the found 100K resistor in the search result grid and display the footprint in the Models section of the panel.
Many of the resistors and capacitors have several footprint models, for different density levels. Select the M variety as shown in the image below. This selection can be done before the component is placed on the schematic during
schematic placement or after schematic placement.
Right-click on the resistor in the search results grid and select Place from the context menu, as shown below.
While the resistor is floating on the cursor, press the Tab key to open the Properties panel.
In the General section of the panel, type in the Designator R1.
In the Parameters section of the panel, enable the visibility of the Resistance parameter and disable the visibility of other parameters.
Leave all other fields at their default values and click the Pause button ( ) to return to part placement; the resistor will be floating on the cursor.
Press the Spacebar to rotate the component in 90° increments until it has the correct orientation.
Position the resistor above and to the left of the base of Q1 (refer to the schematic diagram shown previously) and click the left mouse button or press Enter to place the part.
Next, place the other 100k resistor, R2, above and to the right of the base of Q2. The designator will automatically increment when you place the second resistor.
Exit part placement mode by clicking the right mouse button or pressing the Esc key. The cursor will revert back to a standard arrow.
The remaining two resistors, R3 and R4, have a value of 1K; search for: resistor 1K 5% 0805 fixed in the Components panel.
Select the found 1K resistor in the search result grid and display the footprint in the Models section of the panel.
Many of the resistors and capacitors have several footprint models, for different density levels. Select the M variety.
Right-click on the resistor in the search results grid and select Place from the context menu.
While the resistor is floating on the cursor, press the Tab key to open the Properties panel.
In the General section of the panel, type in the Designator R3.
In the Parameters section of the panel, enable the visibility of the Resistance parameter and disable the visibility of other parameters.
Leave all other fields at their default values and click the Pause button ( ) to return to part placement; the resistor will be floating on the cursor.
Press the Spacebar to rotate the component in 90° increments until it has the correct orientation.
Position and place R3 directly above the Collector of Q1, then place R4 directly above the Collector or Q2, as shown in the image above.
Right-click or press Esc to exit part placement mode.
Placing the Connector
Return to the Components panel and search for: connector male straight.
Select the found connector in the search result grid, right-click on it then select Place from the context menu.
While the header is floating on the cursor, press Tab to open the Properties panel and set the Designator to P1.
Click the Pause button to return to part placement.
Before placing the header, press Spacebar to rotate it to the correct orientation. Click to place the connector on the schematic, as shown in the image above.
Right-click or press Esc to exit part placement mode.
Save your schematic locally.
Editing in the Properties Panel
One of the powerful features of the Properties panel is that it supports editing multiple selected objects at the same time.
If all objects share a property, that property will be available for editing.
If all objects share the same property value, that value will be displayed.
If objects share the same property but have different values, it will display an asterisk (*).
The value entered or option chosen is applied to all selected objects.
Use the Properties panel to edit the properties of multiple selected objects. The selected components are rotated to force their strings to the default locations.
You have now placed all the components. Note that the components shown in the image above are spaced so that there is plenty of room to wire to each component pin. This is important because you cannot place a wire across the bottom of a pin to get to
a pin beyond it. If you do, both pins will connect to the wire. If you need to move a component, click and hold on the body of the component then drag the mouse to reposition it.
Component Positioning Tips
To reposition any object, place the cursor directly over the object, click and hold the left mouse button, drag the object to a new position then release the mouse button. Movement is constrained to the current snap grid, which is displayed on
the Status Bar. Press the G shortcut at any time to cycle through the current snap grid settings. Remember that it is important to position components on a coarse grid, such as 50 or 100mil.
Once a component has been placed on the schematic, the software will attempt to maintain connectivity (keep the wires attached) if the component is moved. This connective-aware movement is referred to as dragging. To move the component without
maintaining connectivity, hold Ctrl as you click and drag the component. To switch the default behavior from dragging to moving, disable the Always Drag option in the Schematic – Graphical Editing page of the Preferences dialog.
You can also re-position a group of selected schematic objects using the arrow keys on the keyboard. Select the objects then press an arrow key while holding down the Ctrl key. Hold Shift as well to move objects by 10 times the current snap grid.
The grid can also be temporarily set to the minimum 10mil value while moving an object with the mouse; hold Ctrl to do this. Use this feature when positioning text.
The grids you cycle through when you press the G shortcut are defined in the Schematic – Grids page of the Preferences dialog (Tools » Preferences ). The Units controls
on the Schematic – General page of the Preferences dialog are used to select the measurement units; select either Mils or Millimeters . Note that Altium Designer components
are designed using an imperial grid; if you change to a metric grid, the component pins will no longer fall onto a standard grid. Because of this, it is recommended to use Mils for Units unless you
plan on only using your own components.
Wiring up the Circuit
Wiring is the process of creating connectivity between the various components of your circuit. To wire up your schematic, refer to the sketch of the circuit and the animation shown below.
Use the Wiring tool to wire up your circuit. Toward the end of the animation, you can see how wires can be dragged.
The Active Bar
The tools most commonly used in each editor are available on the Active Bar , which is displayed at the top of the editing window.
The buttons on the Active Bar are either single-function or multi-function. Multi-function buttons are indicated by a small white triangle in their bottom-right corner. Click and hold anywhere on a multi-function button for one second
or right-click it – a menu will appear listing other available commands. The last-used command will become the default for that button location.
Wiring the schematic
To make sure you have a good view of the schematic sheet, press the PgUp key to zoom in or PgDn to zoom out. Alternatively, hold down the Ctrl key and roll the mouse wheel to zoom in/out, or hold
Ctrl + Right Mouse button down and drag the mouse up/down to zoom in/out. There are also a number of useful View commands in the right-click View submenu, such as Fit All Objects (Ctrl+PgDn ).
First, wire the lower pin of resistor R1 to the base of transistor Q1 in the following manner. Click the Active Bar (Place » Wire , or Ctrl+W shortcut) to enter the wire placement mode. The cursor will change to a crosshair.
Position the cursor over the bottom end of R1. When you are in the right position, a red connection marker (red cross) will appear at the cursor location. This indicates that the cursor is over a valid electrical connection point on the component.
Left-click or press Enter to anchor the first wire point. Move the cursor and you will see a wire extend from the cursor position back to the anchor point.
Position the cursor over the base of Q1 until you see the cursor change to a red connection marker. If the wire is forming a corner in the wrong direction, press Spacebar to toggle the corner direction.
Click or press Enter to connect the wire to the base of Q1. The cursor will release from that wire.
Note that the cursor remains a crosshair indicating that you are ready to place another wire. To exit placement mode completely and go back to the arrow cursor, you would right-click or press Esc again – but don't do this
just now.
Next, wire from the lower pin of R3 to the collector of Q1. Position the cursor over the lower pin of R3 and click or press Enter to start a new wire. Move the cursor vertically until it is over the collector of Q1 then click
or press Enter to place the wire segment. Again, the cursor will release from that wire and you remain in wiring mode, ready to place another wire.
Wire up the rest of your circuit, as shown in the animation above.
When you have finished placing all the wires, right-click or press Esc to exit placement mode. The cursor will revert to an arrow.
Wiring Tips
Use the Ctrl+W shortcut to launch the Place » Wire command.
Left-click or press Enter to anchor the wire at the cursor position.
Press Backspace to remove the last anchor point.
Press Spacebar to toggle the direction of the corner. You can observe this in the animation shown above toward the end when the connector is being wired.
Press Shift+Spacebar to cycle through the wiring corner modes. Available modes include: 90, 45, Any Angle, and Autowire (place orthogonal wire segments between the click points).
Right-click or press Esc to exit wire placement mode.
Click, Hold&Drag to drag the component together with any connected wires; Ctrl+Click, Hold&Drag to move a placed component.Whenever a wire crosses the connection point of a component or is terminated on another wire, a junction will automatically be created.
A wire that crosses the end of a pin will connect to that pin even if you delete the junction. Check that your wired circuit looks like the figure shown before proceeding.
Wiring cross-overs can be displayed as a small arch if preferred. Enable the Display Cross-Overs option in the Schematic – General page of the Preferences dialog.
Nets and Net Labels
Each set of component pins that you have connected to each other now form what is referred to as a net . For example, one net includes the base of Q1, one pin of R1, and one pin of C1. Each net is automatically assigned a system-generated name,
which is based on one of the component pins in that net.
To make it easy to identify important nets in the design, you can add Net Labels to assign names. For the multivibrator circuit, you will label the 12V and GND nets in the circuit, as shown
below.
Net Labels have been added to the 12V and GND nets, completing the schematic.
Adding net labels
Net Labels, Ports, and Power Ports
As well as giving a net a name, Net Labels are also used to create connectivity between two separate points on the same schematic sheet.
Ports are used to create connectivity between two separate points on different sheets. Off Sheet Connectors can also be used to do this.Power Ports are used to create connectivity between points on all sheets; for this single sheet design, Net Labels or Power Ports could have been used.
Congratulations! You have just completed your first schematic capture. Before you turn the schematic into a circuit board, you need to configure the project options and check the design for errors.
Setting Up Project Options
Project-specific settings are configured in the Project Options dialog shown below (Project » Project Options ). The project options include the error checking parameters, a connectivity matrix, class generation settings,
the Comparator setup, Engineering Change Order (ECO) generation, output paths and connectivity options, Multi-Channel naming formats, and project-level Parameters.
Project outputs, such as assembly outputs, fabrication outputs, and reports can be set up from the File and Reports menus. These settings are also stored in the Project file so they are always available for this project.
An alternate approach is to use an OutputJob file to configure the outputs, with the advantage that an OutputJob can be copied from one project to the next. See Preparing Your Design for Manufacture to learn more about configuring
the outputs.
Dynamic Compilation
The Unified Data Model (UDM) is available from the moment a project is opened and should not require additional compilation, which saves time with increased speed of compilation and persistent listings of nets and components in the Navigator panel. The design connectivity model is incrementally updated after each user operation. This means that manual project compilation is not necessary to see the contents of the Navigator panel, run the Bill of Materials (BOM), or perform
an Electronic Rules Check (ERC). Manual compilation is not needed for:
Navigator and Projects panelsActiveBOM
Cross-probing
Net color highlighting
Pin swapping
Component cross reference
Checking the Electrical Properties of Your Schematic
Schematic diagrams are more than just simple drawings – they contain electrical connectivity information about the circuit. You can use this connectivity awareness to verify your design. When you compile a project (Project » Validate PCB Project ),
the software checks for logical, electrical, and drafting errors between the UDM and compiler settings. Any violations that are detected will display in the Messages panel.
Setting up the Error Reporting
Dialog page: Error Reporting
The Error Reporting tab in the Project Options dialog is used to set up a large range of drafting and component configuration checks. The Report Mode settings show the level of severity of a violation. If you
want to change a setting, click on a Report Mode next to the violation you want to change and choose the level of severity from the drop-down list.
Configure the Error Reporting tab to detect for design errors when the project is compiled.
Configuring the Error Checking
Select Project » Project Options to open the Options for PCB Project dialog.
Scroll through the list of error checks and note that they are clustered in groups; each group can be collapsed if required.
Click on the Report Mode setting for any error check and note the options available.
Setting Up the Connection Matrix
Dialog page: Connection Matrix
As the design is coming along, a list of the pins in each net is built into memory. The type of each pin is detected (e.g., input, output, passive, etc.), then each net is checked to see if there are pin types that should not be connected to each
other, for example, an output pin connected to another output pin. The Connection Matrix tab of the Project Options dialog is where you configure what pin types are allowed to connect to each other. For example, look at the
entries on the right side of the matrix diagram and find Output Pin . Read across this row of the matrix until you get to the Open Collector Pin column. The square where they intersect is orange ,
indicating that an Output Pin connected to an Open Collector Pin on your schematic will generate an error condition when the project is compiled.
You can set each error type with a separate error level, i.e. from No Report to a Fatal Error . Click on a colored square to change the setting; continue to click to move to the next check-level. Set the
matrix so that Unconnected – Passive Pin generates an Error , as shown in the image below.
The Connection Matrix tab defines what electrical conditions are checked for on the schematic; note that the Unconnected – Passive Pin setting is being changed.
Changing the Connection Matrix
To change one of the settings, click the colored box; it will cycle through the four possible settings. Note that you can right-click on the dialog face to display a menu that lets you toggle all settings simultaneously, including an option
to restore them all to their Default state (handy if you have been toggling settings and cannot remember their default state).
Your circuit contains only passive pins. Let's change the default settings so that the connection matrix detects unconnected passive pins. Look down the row labels to find the Passive Pin row. Look across the column labels to
find Unconnected . The square where these entries intersect indicates the error condition when a passive pin is found to be unconnected in the schematic. The default setting is green indicating
that no report will be generated.
Click on this intersection box until it turns orange (as shown in the image above) so that an error will be generated for unconnected passive pins when the project is compiled. You will purposely create
an instance of this error later in the tutorial.
Configuring the Class Generation
Dialog page: Class Generation
The Class Generation tab in the Project Options dialog is used to configure what type of classes are generated from the design (the Comparator and ECO Generation tabs are then used to control
if classes are transferred to the PCB). By default, the software will generate Component classes and Rooms for each schematic sheet, and Net Classes for each bus in the design. For a simple, single-sheet design such as this, there is no need to generate
a component class or a room. Ensure that the Component Classes checkbox is cleared; doing this will also disable the creation of a room for that component class.
Note that this tab of the dialog also includes options for User-Defined Classes .
The Class Generation tab is used to configure what classes and rooms are automatically created for the design.
Configuring Class Generation
Clear the Component Classes checkbox, as shown in the image above.
Other options on this tab can be left at their default states.
Setting Up the Comparator
Dialog page: Comparator
The Comparator tab in the Project Options dialog sets which differences between files will be reported or ignored when a project is compiled. Generally, the only time you will need to change settings in this tab is when you add
extra detail to the PCB, such as design rules, and do not want those settings removed during design synchronization. If you need more detailed control, you can selectively control the comparator using the individual comparison settings.
For this tutorial, it is sufficient to confirm that the Ignore Rules Defined in PCB Only option is enabled as shown in the image below.
The Comparator tab is used to configure exactly what differences the comparison engine will check for.
Configuring Comparator Settings
For this tutorial, it is sufficient to confirm that the Ignore Rules Defined in PCB Only option is enabled, as shown in the image above.
You are now ready to validate the project and check for any errors.
Verifying the Project to Check for Errors
Main page: Verifying Your Design Project
Validation of a project checks for drafting and electrical rules errors in the design documents, and details all warnings and errors in the Messages panel. You have set up the rules in the Error Checking and Connection Matrix tabs of the Project Options dialog, so you are now ready to check the design.
To verify the project and check for errors, select Project » Validate PCB Project Multivibrator.PrjPcb from the main menus.
Use the Messages panel to locate and resolve design warnings and errors; double-click on a warning/error to cross probe to that object.
Checking the project for errors
To validate the Multivibrator project, select Project » Validate PCB Project Multivibrator.PrjPcb from the main menus.
When the validation is complete, all warnings and errors are displayed in the Messages panel. The panel will only open automatically if there are errors detected (not when there are only warnings). To open it manually, click the Messages from the menu.
If your circuit is drawn correctly, the Messages panel should not contain any errors, only the message Compile successful, no errors found. If there are errors, work through each one, checking your circuit, and ensuring that
all wiring and connections are correct.
You will now deliberately introduce an error into the circuit and validate the project again:
Click on the Multivibrator.SchDoc tab at the top of the design space to make the schematic sheet the active document.
Click in the middle of the wire that connects P1 to the emitters wire of Q1 and Q2 (the wire of the GND net). Small, square editing handles will appear at each end of the wire and the selected color will display as a dotted line along
the wire to indicate that it is selected. Press the Delete key on the keyboard to delete the wire.
Validate the project again (Project » Validate PCB Project Multivibrator.PrjPcb ) to check for errors. The Messages panel will display error messages indicating you have unconnected pins in your circuit.
The Messages panel is divided horizontally into two regions as shown in the image above. The upper region lists all messages, which can be saved, copied, cross probed to, or cleared via the right-click menu. The lower region
details the warning/error currently selected in the upper region of the panel.
When you double-click on an error or warning in either region of the Messages panel, the schematic view will pan and zoom to the object in error.
When you hover the cursor over the object in error (not the wiggly line), a message describing the error condition will appear.
Before you finish this section of the tutorial, let's fix the error in our schematic.
Make the schematic sheet the active document.
Undo the delete action (Ctrl+Z ) to restore the deleted wire.
To check that there are no longer any errors, re-compile the project (Project » Validate PCB Project Multivibrator.PrjPcb ); the Messages panel should show no errors.
Save the project to the Workspace – click the Save to Server control next to the project name in the Projects panel, confirm that the Multivibrator.PrjPcb and Multivibrator.SchDoc files
are checked in the Save to Server dialog that opens, enter a comment into the Comment field (e.g., Schematic is created and validated), then click the OK button.
When you double-click on an error in the Messages panel:
The schematic zooms to present the object in error. The Zoom Precision is set by the upper slider in the Highlight Methods section of the System – Navigation page of the Preferences dialog.
The entire schematic fades except for the object in error. The amount that the schematic fades is controlled by the Dimming level, set by the lower slider in the Highlight Methods section of the System – Navigation page of the Preferences dialog. Click anywhere on the schematic to clear the dimming.
To clear all messages from the Messages panel, right-click in the panel and select Clear All .
Configuring the Bill of Materials
Main page: BOM Management with ActiveBOM
Ultimately, every part used in the design must have detailed supply chain information. Rather than requiring that this information be added to each design component, or added as a post-process in an Excel spreadsheet, you can add it at any point through
the design cycle in an ActiveBOM (*.BomDoc).
ActiveBOM is the component management editor included in Altium Designer, which is used to:
Configure the component information so that it is BOM-ready, including adding additional non-PCB component BOM items, such as the bare board, glue, mounting hardware, and so on.
Add additional columns, such as a line number column, to suit the requirements of the assembly house.
Map each design component to a real-world manufacturer part.
Verify the supply chain availability and price for each part, for a defined number of manufactured units.
Calculate the cost to build for the defined number of manufactured units.
ActiveBOM is used to map each design component to a real-world part.
This ability to inject supply chain details directly into the BOM changes the role of the BOM document in the PCB project. No longer a simple output file, ActiveBOM raises the component management process to sit alongside the schematic capture and PCB
design processes, where ActiveBOM's BomDoc becomes the source of all Bill Of Materials data for the PCB project for all BOM-type outputs. ActiveBOM is the recommended approach to BOM management.
ActiveBOM queries the supply chain in real-time, using the Part Providers enabled in the settings of your connected Workspace. Because data is updated in real-time, the availability of the parts used in this tutorial will change over time. The list of
available suppliers also changes over time. For these reasons, the results you get may be different from the results shown and described in this tutorial.
Configuring the BomDoc
To include a BomDoc in the tutorial:
Right-click on the project filename in the Projects panel then select Add New to Project » ActiveBOM . Note that a project can only include one BomDoc.
The ActiveBOM document will appear as a Source Document in the Projects panel. Right-click on the document entry in the Projects panel to select the Save As command and name it Multivibrator.
Note that you do not need to enter the file extension in the Save As dialog; this is automatically appended.
The BomDoc will be created, and the components used in the tutorial listed as BOM Items. The BomDoc is configured in the Properties panel , where the production quantity and currency, supply chain, and
visible BOM Item parameters are defined, along with other settings. Take some time to familiarize yourself with the features available in the Properties panel's two tabs. Note that the panel includes a search field at the top, which
is handy for quickly locating a control or a parameter.
Explore the Columns tab of the panel. Note that the available data to be included in the BOM can be sourced from various locations, controlled by the Sources buttons.
The components are detailed in the main grid area of the BomDoc. By default, there is a column titled Line # . Click the Set Line Numbers button (Refresh button at the top-right of the document to show the Line # values in the grid).
Because the components were saved from the Manufacturer Part Search panel, each part already includes supply chain information. When you click on a part in the BOM Items grid, its supply chain information is displayed in the lower region
of the BomDoc as shown in the image above. Each row displayed in this lower region of the BomDoc is referred to as a Solution, with the manufacturer part + part number (referred to as an MPN) shown on the left, and available suppliers
+ supplier part numbers (referred to as SPNs) are shown in each tile on the right.
Note that the BOM Items grid includes a BOM Status column on the right. Hover the mouse cursor over a status icon for information about any issues detected.
The Status icons should indicate that all of the Items include the error No MPN ranked. This means that the designer (you) has not yet checked through the selected parts (MPNs) and indicated that they are happy with each of them.
An MPN is accepted by assigning it a rank (as shown in the image above). Do this for each of the items that show no other error type. It is possible that the transistor may have other errors; this will be resolved shortly.
The Status of four of the five BOM Items should change to green (
The status of each Item is checked against the current configuration of BOM Checks configured in the Properties panel. The BOM Checks list in the panel details all BOM checks that are currently being
violated. The available BOM checks and their current settings are configured in the Bom Checks dialog (accessed with the BOM Checks list).
Select the transistor Item; it may be flagged as Obsolete . For an Item that does not have an MPN assigned, or has an MPN but that part has no suppliers, you can also create a Manufacturer Link.
The Manufacturer Link feature allows you to connect a Workspace part, or a non-Workspace part with supply chain issues, to your preferred manufacturer part. Using this feature, you can bring the full power of the Altium Parts Provider to all
of your design components directly in the BomDoc, complete with real-time supplier, price, and availability information. The Manufacturer Link is stored in the BomDoc.
To add a Manufacturer Link, select the transistor in the grid, click the Add Solution button and select Create/Edit Manufacturer Links from the drop-down menu.
The Edit Manufacturer Links dialog will open. Click the Add button to add a new Manufacturer Link; the Add Part Choices dialog will open. This dialog is used to search for a suitable manufacturer part
in the same way as the Manufacturer Part Search panel. As well as identifying a suitable part, you can also check the suppliers, price, and availability.
The
Search field in the
Add Part Choices dialog is automatically populated with data from the component you selected in the BomDoc. The field that supplies the search data is determined by the
Suggested Keywords setting in the
Data Management – Part Providers page of the
Preferences dialog. The default is to search using the
Comment field; this can be changed if required.
If the search only returns the same part you already have used, try broadening the search, for example, search for BC547C.
Keep an eye on the vertical colored bar at the edge of the Manufacturer Part column. This indicates the Lifecycle state of that part. Ideally, you will select a part with a green Lifecycle state (Volume Production).
Note that you do not need the part to have models since you already have a symbol on the schematic and a footprint on the PCB.
Choose a part that has a Lifecycle state of Volume Production (hover the cursor over the vertical colored bar to view the lifecycle state) and stock available, then click OK to accept this part.
Added part choices and rankings in the BomDoc are automatically saved back for the component in the Workspace.
You will return to the Edit Manufacturer Links dialog. Click OK to close the dialog and return to the BomDoc.
The Solutions region of the BomDoc will show two solutions: the original part used in the design, and the Solution you just added. The Solutions are listed in the order they will be used in the BOM. Use the Ranking feature to promote the
part you selected to be the primary Solution by hovering over the stars then clicking the desired rank (as shown below).
All parts now include supply chain details. Save the BomDoc and the project locally.
Create a Manufacturer Link to select a part directly in the BomDoc when the schematic part does not include suitable supply chain details.
Save the project to the Workspace – click the Save to Server control next to the project name in the Projects panel, confirm that the Multivibrator.PrjPcb and Multivibrator.BomDoc files
are checked in the Save to Server dialog that opens, enter a comment into the Comment field (e.g., BOM document added), then click the OK button.
