Managing Design Attributes with the Properties Panel in Altium NEXUS

The options in this section of the panel determine which schematic library objects may be selected in the workspace.

• All Objects button – select remove object filtering so that all types of objects may be selected.
• Object buttons – toggle each object button to enable/disable the ability to select that object type.

• Units - select the desired unit. Choose either mm or mils. 
• Visible Grid - enter the desired grid. Use the  or  to show/hide the grid in the workspace.
• Snap Grid - check the box to enable snap grids. Enter the desired grid in the text box.
• Sheet Border - check the box to enable a sheet border then click the colored box to change the border color.
• Sheet Color - click the colored box to change the sheet color.
• Show Hidden Pins - enable to show hidden pins on the workspace.
• Show Comment/Designator - enable to show comments/designators on the workspace.

The options in this section of the panel determine which PCB objects may be selected in the workspace.

• All Objects button – select remove object filtering so that all types of objects may be selected.
• Object buttons – toggle each object button to enable/disable the ability to select that object type.

• Grids -  used to toggle whether the cursor will snap to the active workspace grid. When this option is enabled the cursor will pull, or snap, to the nearest snap grid location. The active snap grid is displayed on the Status bar, and in the PCB editor Heads Up display (Shift+H to toggle on/off).
• Guides - used to toggle whether the cursor will snap to manually placed linear or point Snap Guides. A Snap Guide will override the Snap Grid.
• Axes  - used to toggle whether the cursor will axially-align (in either the X or Y direction) to the enabled Objects for snapping. The Axis Snap Range defines the distance within which X or Y axial-alignment will occur. A dynamic alignment guide line is displayed when alignment is achieved, from the current cursor location to the axially-aligned object snap point (hotspot).
• Snapping - select whether you want to snap to objects on:
  • All Layers - enable this option to allow the cursor to snap to any electrical object on any visible layer.
  • Curent Layer - enable this option to allow the cursor to only recognize and snap to objects placed on the currently selected layer.
  • Off - enable this option to turn off snapping to hotspots.
• Objects for snapping
  • On/Off - check to enable snapping for the desired objects. 
  • Objects - a list of the available objects.

• Snap Distance - when the cursor is within this distance from an enabled object snap point (and snapping is enabled for the active layer), the cursor will snap to that point.
• Axis Snap Range - when the cursor is axially-aligned and within this distance from an enabled object snap point (and the Axes feature is enabled), a dynamic guide line will display to indicate that alignment has been achieved.

• Board Size - displays the horizontal and vertical board dimensions.
• Components/Layers/Nets/Primitives & Others - displays information for each listed category such as the total number of the listed item.
• Reports - click to open the Board Report dialog in which you can specify the content to be included when generating a detailed report for the board.

• Grid Manager - where local customized grids can be defined and managed, as well as the default Snap Grid for the board. 
  • Priority -  in the workspace, priority is distinguished by drawing order. The highest priority grid (priority 1) will be drawn in front of all other grids, then the grid with priority level 2, etc., down to the default Global Board Snap Grid, which is drawn behind all other custom grids.
  • Name - displays the name of the grid.
  • Color - click to open a drop-down to set/change the color of the associated grid.
  • Comp - enable to apply the selected grid to only components.
  • Non Comp - enable to apply the selected grid to objects that are not components.
• Add
  • Add Cartesian Grid - click to add a Cartesian grid.
  • Add Polar Grid - click to add a Polar grid. Polar grids enable you to more easily design non-rectangular features and boards. 
• Properties - click to open the respective grid editor dialog (Cartesian Grid Editor or Polar Grid Editor) to modify properties for the selected grid.
•  - click to delete the currently selected grid.

• Guide Manager - where a range of manual Snap Guides and Snap Points for the board can be defined and managed. 
  • Enabled - whether the guide is visible in the workspace (checked) or not (unchecked).
  • Name - the name of the guide.
  • X - the x-coordinate (where applicable) specified in the workspace that the guide is to pass through or point is to be located at.
  • Y - the y-coordinate (where applicable) specified in the workspace that the guide is to pass through or point is to be located at.

A coordinate can be defined by clicking on the relevant field then entering the value. Alternatively, and where applicable/available, click  to the right of the field then specify the required point directly in the PCB workspace.

• Color - click to open a drop-down to set/change the color of the associated guide.

• Add - click to add a new snap guide or snap point. Choose the corresponding command for the required guide type from the associated menu; an entry for the new guide/point will be added to the grid. The following guide types are available:
  • Add Horizontal Guide - use this command to add a horizontal guideline at the desired Y-coordinate location in the workspace.
  • Add Vertical Guide - use this command to add a vertical guideline at the desired X-coordinate location in the workspace.
  • Add +45 Guide - use this command to add a 45 degree (y=x) guideline that passes through the desired X,Y coordinate location in the workspace.
  • Add -45 Guide - use this command to add a -45 degree (y=-x) guideline that passes through the desired X,Y coordinate location in the workspace.
  • Add Snap Point - use this command to add a point snap guide. This is a hotspot that you manually mark within the confines of the default snap grid. During an interactive process such as placing or moving an object, that objects' hotspot will 'snap' to a point snap guide when it passes into close proximity with it.
• Place - click to place a guide. Select the guide type from the drop-down:
  • Place Horizontal Guide - use this command to place a horizontal guideline at the desired Y-coordinate location in the workspace.
  • Place Vertical Guide - use this command to place a vertical guideline at the desired X-coordinate location in the workspace. 
  • Place +45 Guide - use this command to place a 45 degree (y=x) guideline that passes through the desired X,Y coordinate location in the workspace.
  • Place -45 Guide - use this command to place a -45 degree (y=-x) guideline that passes through the desired X,Y coordinate location in the workspace.
  • Place Snap Point -  use this command to place a point snap guide. This is a hotspot that you manually mark within the confines of the default snap grid. During an interactive process such as placing or moving an object, that objects' hotspot will 'snap' to a point snap guide when it passes into close proximity with it.
• - click to delete the currently selected guide.

• Units - use to select the default measurement units for the current PCB document. Default units are used to display any distance related information on screen or in reports. The default units are always used if a unit's suffix (mm or mil) is not entered when specifying any distance related information. 
• Polygon Naming Scheme - select a naming system from the dropdown menu. There are four choices of naming templates:
  • NET NAME_LXX_PXXX
  • LXX_NET NAME_PXXX
  • NET NAME_LAYER NAME_PXXX
  • LAYER NAME_NET NAME_PXXX

where:

• NET NAME - name of the net to which the polygon is connected. If the polygon is not connected to a net, the name NONET is used.
• LAYER NAME - user-defined name of that layer from the Layer Stack.
• LXX - system assigned copper layer number based on the current order of layers in the Layer Stack where Top Layer is L01. This value is updated whenever the order of copper layers is changed.
• PXXX - system-assigned numerical index; unique for each polygon on the board.

• Designator Display - use this field to determine how designators are to be displayed. It can be difficult positioning the designator strings in a multi-channel design, as they can end up being quite long. As well as choosing a naming option that results in a short name, another option is to display just the original, logical component designation instead. For example, C30_CIN1 would display as C30. This would of course necessitate some other notation being added to the board to indicate the separate channels, such as a box being drawn around each channel on the component overlay. The following options are available:
  • Physical - choose to display the physical designators. These are the designators displayed on the compiled tab views of the schematic source documents. For multi-channel designs, designator format is determined by the Designator Format field on the Multi-Channel tab of the Project Options dialog. Physical designators are unique, e.g., R1_CH1.
  • Logical - choose to display the logical designators. These are the designators displayed on the Editor tab views of the schematic source documents. Logical designators are not unique; for example, the R1_CH1 physical designator will become simply R1.
• Sheet Settings - use this region to configure the PCB sheet.
  • X/Y - enter the X and Y coordinates for the bottom left corner of the sheet. This distance is measured from the absolute origin, which is the bottom left corner of the workspace. The distance can be defined in either metric or imperial units regardless of the default units (which are determined by the Units setting). To specify the units when entering a size, add the mm or mil suffix to the value.
  • Width - enter a width for the sheet here. The sheet provides an area that emulates the traditional drawing sheet and is useful for placing information such as dimensions, notes and title blocks. Information placed on mechanical layers can be linked to the sheet so that they only display when the sheet is being displayed. Sheet size can be defined in either metric or imperial units regardless of the default units (which are determined by the Units setting). To specify the units when entering a size, add the mm or mil suffix to the value.
  • Height - eEnter a height for the sheet here. The sheet provides an area that emulates the traditional drawing sheet and is useful for placing information such as dimensions, notes and title blocks. Information placed on mechanical layers can be linked to the sheet so that they only display when the sheet is being displayed. Sheet size can be defined in either metric or imperial units regardless of the default units (which are determined by the Units setting). To specify the units when entering a size, add the mm or mil suffix to the value.
  • Get Size From Sheet Layer - enable this option to size the sheet from the sheet layer.

The options in this section of the panel determine which PCB library objects may be selected in the workspace.

• All Objects button – select remove object filtering so that all types of objects may be selected.
• Object buttons – toggle each object button to enable/disable the ability to select that object type.

• Grids -  used to toggle whether the cursor will snap to the active workspace grid. When this option is enabled the cursor will pull, or snap, to the nearest snap grid location. The active snap grid is displayed on the Status bar, and in the PCB editor Heads Up display (Shift+H to toggle on/off).
• Guides - used to toggle whether the cursor will snap to manually placed linear or point Snap Guides. A Snap Guide will override the Snap Grid.
• Axes  - used to toggle whether the cursor will axially-align (in either the X or Y direction) to the enabled Objects for snapping. The  Axis Snap Range defines the distance within which X or Y axial-alignment will occur. A dynamic alignment guide line is displayed when alignment is achieved from the current cursor location to the axially-aligned object snap point (hotspot).
• Snapping - select whether you want to snap to objects on:
  • All Layers - enable this option to allow the cursor to snap to any electrical object on any visible layer.
  • Curent Layer - enable this option to allow the cursor to only recognize and snap to objects placed on the currently selected layer.
  • Off - enable this option to turn off snapping to hotspots.
• Objects for snapping
  • On/Off - check to enable snapping for the desired objects. 
  • Objects - a list of the available objects.
• Snap Distance - when the cursor is within this distance from an enabled object snap point (and snapping is enabled for the active layer), the cursor will snap to that point.
• Axis Snap Range - when the cursor is axially-aligned and within this distance from an enabled object snap point (and the Axes button is enabled), a dynamic guide line will display to indicate that alignment has been achieved.

• Grid Manager - where local customized grids can be defined and managed, as well as the default Snap Grid for the board. 
  • Priority -  in the workspace, priority is distinguished by drawing order. The highest priority grid (priority 1) will be drawn in front of all other grids, then the grid with priority level 2, etc., down to the default Global Board Snap Grid, which is drawn behind all other custom grids.
  • Name - displays the name of the grid.
  • Color - click to open a drop-down to set/change the color of the associated grid.
  • Enabled - check to enable the associated grid.
• Add
  • Add Cartesian Grid - click to add a Cartesian grid.
  • Add Polar Grid - click to add a Polar grid.  Polar grids enable you to more easily design non-rectangular features and boards. 
• Properties - click to open the respective grid editor dialog (Cartesian Grid Editor or Polar Grid Editor) to modify properties for the selected grid.
•  - click to delete the currently selected grid.

• Guide Manager - where a range of manual Snap Guides and Snap Points for the board can be defined and managed. 
  • Enabled - whether the guide is visible in the workspace (checked) or not (unchecked).
  • Name - the name of the guide.
  • X - the x-coordinate (where applicable) specified in the workspace that the guide is to pass through or point is to be located at.
  • Y - the y-coordinate (where applicable) specified in the workspace that the guide is to pass through or point is to be located at.

A coordinate can be defined by clicking on the relevant field then entering the value. Alternatively, and where applicable/available, click  to the right of the field, then specify the required point directly in the PCB Library workspace.

• Color - click to open a drop-down to set/change the color of the associated guide.

• Add - click to add a new snap guide or snap point. Choose the corresponding command for the required guide type from the associated menu; an entry for the new guide/point will be added to the grid. The following guide types are available:
  • Add Horizontal Guide - use this command to add a horizontal guideline at the desired Y-coordinate location in the workspace.
  • Add Vertical Guide - use this command to add a vertical guideline at the desired X-coordinate location in the workspace.
  • Add +45 Guide - use this command to add a 45 degree (y=x) guideline that passes through the desired X,Y coordinate location in the workspace.
  • Add -45 Guide - use this command to add a -45 degree (y=-x) guideline that passes through the desired X,Y coordinate location in the workspace.
  • Add Snap Point - use this command to add a point snap guide. This is a hotspot that you manually mark within the confines of the default snap grid. During an interactive process such as placing or moving an object, that objects' hotspot will 'snap' to a point snap guide when it passes into close proximity with it.
• Place - click to place a guide. Select the guide type from the drop-down:
  • Place Horizontal Guide - use this command to place a horizontal guideline at the desired Y-coordinate location in the workspace.
  • Place Vertical Guide - use this command to place a vertical guideline at the desired X-coordinate location in the workspace. 
  • Place +45 Guide - use this command to place a 45 degree (y=x) guideline that passes through the desired X,Y coordinate location in the workspace.
  • Place -45 Guide - use this command to place a -45 degree (y=-x) guideline that passes through the desired X,Y coordinate location in the workspace.
  • Place Snap Point -  use this command to place a point snap guide. This is a hotspot that you manually mark within the confines of the default snap grid. During an interactive process such as placing or moving an object, that objects' hotspot will 'snap' to a point snap guide when it passes into close proximity with it.
•  - click to delete the currently selected guide.

• Units - use to select the default measurement units for the current PCB Library document. Default units are used to display any distance related information on screen or in reports. The default units are always used if a unit's suffix (mm or mil) is not entered when specifying any distance related information. 
• Route Tool Path - use the drop-down to choose the mechanical layer (from all those currently enabled for use in the design) on which to define the route tool path for the board. 

• Net Name - displays the name of the net to which the interactive routing is connected.
• Net Class - displays the net class that the interactive routing belongs to (if it is a member of a net class).
• Length - displays the length.

• Layer - use the drop-down to specify on which layer the routing is located.
• Via Template - if the via is associated with a template, the template name is displayed here.
• Via Hole Size - specify the via hole size.
• Via Diameter - specify the via hole diameter.
• Width - specify the width. Use the slider to specify the width. Farther to the left (Min) signifies that the design rule minimum width defined for the current net will be used. Preferred signifies that the design rule preferred width defined for the current net will be used. Farther to the right (Max) signifies that the design rule maximum width defined for the current net will be used.
  • Pickup From Existing Routes - enable to use the existing track width when routing from a placed track. That is, even if the current routing width is different to the existing track, the existing track width will be adopted when you continue the route from it.

• Routing Mode - use the drop-down to select the desired routing mode. The following choices are available:
  • Ignore Obstacles - select to ignore existing objects (routing can be freely placed). Violations are highlighted. 
  • Walkaround Obstacles - select to have the Interactive Router route around existing tracks, pads and vias. If this mode cannot walk around an obstacle without causing a violation, an indicator appears to show that the route is blocked. 
  • Push Obstacles - select to have the Interactive Router move existing tracks out of the way. This mode can also push vias to make way for the new routing. If this mode cannot push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
  • HugNPush Obstacles - select to have the Interactive Router hug existing tracks, pads, and vias as closely as possible and where necessary, push obstacles to continue the route. If this mode cannot hug or push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
  • Stop At First Obstacle - in this mode, the routing engine will stop at the first obstacle that gets in the way.
  • AutoRoute Current Layer - select to enable auto-routing only on the current layer.
  • AutoRoute MultiLayer - select to enable auto-routing on multiple layers.

• Corner Style - select the desired routing corner style.
  • Restrict to 90/45 - enable to restrict the routing to 90 degrees and 45 degrees only.
• Routing Gloss Effort - select the desired gloss level from the following choices:
  • Off - in this mode, glossing is essentially disabled. Note, however, that cleanup is still run after routing/dragging occurs to eliminate, for example, overlapping track segments. This mode is typically useful at the end stage of board layout when the ultimate level of fine-tuning is required (for example, when manually dragging tracks, cleaning pad entries, etc.).
  • Weak - in this mode, a low level of glossing is applied with the Interactive Router considering only those tracks directly connected to or in the area of the tracks that you are currently routing (or tracks/vias being dragged). This mode of glossing is typically useful for fine-tuning track layout or when dealing with critical traces.
  • Strong - in this mode, a high level of glossing is applied with the Interactive Router looking for shortest paths, smoothing out tracks, etc. This mode of glossing is typically useful in the early stages of the layout process when the aim is to get a good amount of the board routed quickly.
• Automatically Terminate Routing - when enabled, when you complete a route to the target pad, the routing tool does not continue in routing mode from the target pad but rather resets and is ready for you to click on the next source pad from which to route. If this option is disabled, after you route to the target pad, the tool will remain in routing mode and use the previous target pad as the source for the next route.
• Automatically Remove Loops - enable to automatically remove any redundant loops that are created during manual routing. This allows you to re-route a connection without having to manually remove redundant tracks. However, there are times when you need to route nets such as power nets and you need loops. You can toggle this option for a selected net by using the hotkey Shift+D to override this global setting for the same net.
• Remove Net Antennas - enable this option to remove any track or arc end that is not connected to any other primitive and forms an antenna.
• Allow Via Pushing - check this option to allow pushing a Via when in Push Obstacles or HugNPush Obstacles mode.
• Follow Mouse Trail - enable this option to activate routing through the mouse trail.
• Pin Swapping - check this option to enable pin swapping. A  appears when a project compilation is required. 
• Subnet Jumper Length - specify the desired Subnet Jumper length.

• Width Rule - click to open the Edit PCB Rule - Max-Min Width Rule dialog in which you can define PCB rules for routing width.
• Via Rule - click to open the Edit PCB Rule - Routing Via-Style Rule dialog in which you can define PCB rules for via.

• Display Clearance Boundaries - enable to have the no-go clearance area defined by the existing objects and the applicable clearance rule displayed as shaded polygons within a local viewing circle. This option is not available in the Ignore Obstacles routing mode.
  • Reduce Clearance Display Area - enable to use a smaller clearance boundary. This option is available only when the Display Clearance Boundaries option is enabled.
• Show Length Gauge - enable to display the length gauge.

• The Help section displays some of the shortcuts that are available while Interactive Routing.

• Diff. Pair - displays the differential pair name.
• Diff. Pair Class - displays the differential pair class that the routing belongs to (if it is a member of a differential pair class).

• Layer - use the drop-down to specify on which layer the routing is located.
• Via Template - if the via is associated with a template, the template name is displayed here.
• Via Hole Size - specify the via hole size.
• Via Diameter - specify the via hole diameter.
• Gap 
  • Min - select to specify the minimum permissible clearance between primitives on different nets within the same differential pair.
  • Preferred - select to specify the preferred clearance between primitives on different nets within the same differential pair.
  • Max - select to specify the maximum permissible clearance between primitives on different nets within the same differential pair.
• Width - specify the width. Use the slider bar to specify the width. Farther to the left (Min) signifies that the design rule minimum width defined for the current net will be used. Preferred signifies that the design rule preferred width defined for the current net will be used. Farther to the right (Max) signifies that the design rule maximum width defined for the current net will be used.
  • Pickup From Existing Routes - enable to use the existing track width when routing from a placed track. That is, even if the current routing width is different to the existing track, the existing track width will be adopted when you continue the route from it.

• Routing Mode - use the drop-down to select the desired routing mode. The following choices are available:
  • Ignore Obstacles - select to ignore existing objects (routing can be freely placed). Violations are highlighted. 
  • Walkaround Obstacles - select to have the Interactive Router route around existing tracks, pads and vias. If this mode cannot walk around an obstacle without causing a violation, an indicator appears to show that the route is blocked. 
  • Push Obstacles - select to have the Interactive Router move existing tracks out of the way. This mode can also push vias to make way for the new routing. If this mode cannot push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
  • HugNPush Obstacles - select to have the Interactive Router hug existing tracks, pads, and vias as closely as possible and where necessary, push obstacles to continue the route. If this mode cannot hug or push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
  • Stop At First Obstacle - in this mode, the routing engine will stop at the first obstacle that gets in the way.
  • AutoRoute Current Layer - select to enable auto-routing only on the current layer.
  • AutoRoute MultiLayer - select to enable auto-routing on multiple layers.

• Corner Style - select the desired routing corner style.
  • Restrict to 90/45 - enable to restrict the routing to 90 degrees and 45 degrees only.
• Routing Gloss Effort - select the desired gloss level from the following choices:
  • Off - in this mode, glossing is essentially disabled. Note, however, that cleanup is still run after routing/dragging occurs to eliminate, for example, overlapping track segments. This mode is typically useful at the end stage of board layout when the ultimate level of fine-tuning is required (for example, when manually dragging tracks, cleaning pad entries, etc.).
  • Weak - in this mode, a low level of glossing is applied with the Interactive Router considering only those tracks directly connected to or in the area of the tracks that you are currently routing (or tracks/vias being dragged). This mode of glossing is typically useful for fine-tuning track layout or when dealing with critical traces.
  • Strong - in this mode, a high level of glossing is applied with the Interactive Router looking for shortest paths, smoothing out tracks, etc. This mode of glossing is typically useful in the early stages of the layout process when the aim is to get a good amount of the board routed quickly.
• Automatically Terminate Routing - when enabled, when you complete a route to the target pad, the routing tool does not continue in routing mode from the target pad but rather resets and is ready for you to click on the next source pad from which to route. If this option is disabled, after you route to the target pad, the tool will remain in routing mode and use the previous target pad as the source for the next route.
• Automatically Remove Loops - enable to automatically remove any redundant loops that are created during manual routing. This allows you to re-route a connection without having to manually remove redundant tracks. However, there are times when you need to route nets, such as power nets and when you need loops; you can toggle this option for a selected net by using the hotkey Shift+D to override this global setting for the same net.
• Remove Net Antennas - enable this option to remove any track or arc end that is not connected to any other primitive and forms an antenna.
• Allow Via Pushing - check this option to allow pushing a Via when in Push Obstacles or HugNPush Obstacles mode.
• Follow Mouse Trail - enable this option to activate routing through the mouse trail.
• Pin Swapping - check this option to enable pin swapping. A  appears when a project compilation is required. 
• Subnet Jumper Length - specify the desired Subnet Jumper length.

• Differential Pair Rule - click to open the Edit PCB Rule dialog to view/edit the rule.
• Via Rule - click to open the Edit PCB Rule dialog to view/edit the rule.

• Display Clearance Boundaries - enable this option to have the no-go clearance area defined by the existing objects and the applicable clearance rule displayed as shaded polygons within a local viewing circle. This option is not available in the Ignore Obstacles routing mode.
  • Reduce Clearance Display Area - enable this option to use a smaller clearance boundary. This option is available only when the Display Clearance Boundaries option is enabled.

• The Help section displays some of the shortcuts that are available while routing.

• Layer - use the drop-down to specify on which layer the routing is located.
• Via Template - if the via is associated with a template, the template name is displayed here.
• Via Hole Size - specify the via hole size.
• Via Diameter - specify the via hole diameter.
• Width - specify the width. Use the slider bar to specify the width. Farther to the left (Min) signifies that the design rule minimum width defined for the current net will be used. Preferred signifies that the design rule preferred width defined for the current net will be used. Farther to the right (Max) signifies that the design rule maximum width defined for the current net will be used.
  • Pickup From Existing Routes - enable to use the existing track width when routing from a placed track. That is, even if the current routing width is different to the existing track, the existing track width will be adopted when you continue the route from it.
• Bus Spacing - enter the desired bus routing.
  • From Rule - click to assign bus spacing based on the existing design rule. 

• Routing Mode - use the drop-down to select the desired routing mode. The following choices are available:
  • Ignore Obstacles - select to ignore existing objects (routing can be freely placed). Violations are highlighted. 
  • Walkaround Obstacles - select to have the Interactive Router route around existing tracks, pads and vias. If this mode cannot walk around an obstacle without causing a violation, an indicator appears to show that the route is blocked. 
  • Push Obstacles - select to have the Interactive Router move existing tracks out of the way. This mode can also push vias to make way for the new routing. If this mode cannot push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
  • HugNPush Obstacles - select to have the Interactive Router hug existing tracks, pads, and vias as closely as possible and, where necessary, push obstacles to continue the route. If this mode cannot hug or push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
  • Stop At First Obstacle - in this mode, the routing engine will stop at the first obstacle that gets in the way.
  • AutoRoute Current Layer - select to enable auto-routing only on the current layer.
  • AutoRoute MultiLayer - select to enable auto-routing on multiple layers.

• Corner Style - select the desired routing corner style.
  • Restrict to 90/45 - enable to restrict the routing to 90 degrees and 45 degrees only.
• Routing Gloss Effort - select the desired gloss level from the following choices:
  • Off - in this mode, glossing is essentially disabled. Note, however, that cleanup is still run after routing/dragging occurs to eliminate, for example, overlapping track segments. This mode is typically useful at the end stage of board layout when the ultimate level of fine-tuning is required (for example, when manually dragging tracks, cleaning pad entries, etc.).
  • Weak - in this mode, a low level of glossing is applied with the Interactive Router considering only those tracks directly connected to or in the area of the tracks that you are currently routing (or tracks/vias being dragged). This mode of glossing is typically useful for fine-tuning track layout or when dealing with critical traces.
  • Strong - in this mode, a high level of glossing is applied with the Interactive Router looking for shortest paths, smoothing out tracks, etc. This mode of glossing is typically useful in the early stages of the layout process when the aim is to get a good amount of the board routed quickly.
• Automatically Terminate Routing - when enabled, when you complete a route to the target pad, the routing tool does not continue in routing mode from the target pad but rather resets and is ready for you to click on the next source pad from which to route. If this option is disabled, after you route to the target pad, the tool will remain in routing mode and use the previous target pad as the source for the next route.
• Automatically Remove Loops - enable to automatically remove any redundant loops that are created during manual routing. This allows you to re-route a connection without having to manually remove redundant tracks. However, there are times when you need to route nets such as power nets and you need loops - you can toggle this option for a selected net by using the hotkey Shift+D to override this global setting for the same net.
• Remove Net Antennas - enable this option to remove any track or arc end that is not connected to any other primitive and forms an antenna.
• Allow Via Pushing - check this option to allow pushing a Via when in Push Obstacles or HugNPush Obstacles mode.
• Follow Mouse Trail - enable this option to activate routing through the mouse trail.

• The Help section displays some of the shortcuts that are available while routing.

• Net Name - name of the net that the accordion is part of. Displays the * character if multiple accordions are currently selected.
• Net Class - net class that this net belongs to (if it is a member of a net class).

The objective of placing an accordion is to achieve a specific target length for the route whose length is being tuned. That target length is displayed in the Target Length field. The Source buttons are used to control from where that target length value is sourced, and the grid below the buttons displays details about the current choice.  

• Source - source of the maximum length value that the Interactive Length Tuning command is attempting to achieve.
  • Manual - required length can be entered directly into the Target Length field. A list of Recently Used Lengths will appear when this mode is selected. Click to use one of these lengths.
  • From Net - required length is defined by selecting a net name. The list of net names region will include all nets in the design.
  • From Rules - applicable Length and/or Matched Length design rules will be listed. If the net is targeted by multiple rules, the most conservative rule is chosen.
• Source List - this grid region changes based on the user-selected Source mode as described above.
• Target Length - overall length that the Interactive Length Tuning command is attempting to achieve with the addition of the accordion being placed.
• Clip to Target Length - if enabled, the accordion length is automatically clipped once the target length is achieved.

• Style - select the required shape used to create the accordion.
  • Mitered Lines - accordion shape is created from vertical and horizontal track segments with the corners mitered by diagonal track segments.
  • Mitered Arcs - accordion shape is created from vertical and horizontal track segments with the corners mitered by a 90 degree arc segment. 
  • Rounded - accordion shape is created from 180 degree arc segments.
• Max Amplitude - the maximum accordion amplitude the software is permitted to create as shown by the Max Amplitude label on the image in the panel. The amplitude is automatically decreased if there are placement obstacles. The amplitude can be interactively decreased during length tuning by pressing the  key, or increased by pressing the  key.
  • Increment - the step value that the Amplitude will be increased/decreased by when the shortcuts are pressed, or when it is automatically resized due to an obstacle.
• Gap - the distance between the zero-crossings of the accordion shape as indicated by the Space label on the image in the panel. The Gap can be interactively decreased during length tuning by pressing the  key, or increased by pressing the  key.
  • Increment - the step value that the Gap will be increased/decreased by when the shortcuts are pressed.
• Miter - percentage of the corner that is removed by the diagonal miter track/arc. The Miter can be interactively decreased during length tuning by pressing the  key, or increased by pressing the  key.
  • Increment - the step value that the Miter will be increased/decreased by when the shortcuts are pressed.

• The Help section displays some of the shortcuts that are available while interactive length tuning.

• Name - the name of the differential pair.
• Class Name - the class the pair belongs to (if available).

• Source
  • Manual - use the manual mode to enter the length in the Target Length field. The Recently Used Lengths region keeps track of the values you have typed in so that you can easily use them again.
  • From Rules - one or both of the Length and Matched Length design rules must be defined to use this mode. The software will then obey the most stringent combination of these rules. Double-click on a rule listed in the Display Name region to examine its properties in detail.
  • From Diff. Pairs - lists the differential pairs and their lengths on the current PCB. The currently selected differential pair length value is shown in the Target Length field.
  • Target Length - enter the target length.
  • Clip to Target Length - enable to ensure that the final length does not exceed the target length. 

• Style - select the desired amplitude wave pattern from the selections below. Three pattern styles are available: Mitered Lines, Mitered Arcs, and Rounded. The PCB Editor will attempt to match the target length by adding segments to the length according to the defined target length.
  Rounded is the most compact and Mitered Lines is the least compact.
• Max Amplitude - shows the current maximum allowed amplitude of tuning segments. While routing, the PCB Editor will attempt to match the target length by adding segments according to the defined target length. The value can also be adjusted automatically if the Clip to Target Length option is enabled in the Target Length region. You can decrease or increase the amplitude interactively with the "," (comma) and "." (period or full stop) keys. Edit this field to change the maximum allowable amplitude, which can be defined in either mm or mil units. To specify the units when entering a number, add the mm or mil suffix to the value.
• Increment - shows the current step in amplitude when you increase or decrease it during interactive length tuning. Use the "," (comma) or "." (period or full stop) keys while tuning to change the amplitude by the step value. For example, if the maximum amplitude is 100mil and the amplitude increment is 20mil and you pressed the "," key twice during routing, you will get an amplitude of 60mil. Edit this field to change the amplitude step, which can be defined in either mm or mil units. To specify the units when entering a number, add the mm or mil suffix to the value. 
• Space / Radius - shows the current distance between "legs" of the amplitude pattern. The Interactive Length Tuning tool will attempt to match the length by adding wave pattern segments to the existing track to reach the defined target length. Use the shortcut keys 3 or 4 to decrease or increase the gap while you are length tuning. You can also use the Increment field to control the gap size steps. View relevant shortcut keys by pressing the "~" (tilde) key while routing and tune the length interactively. Edit this field to change the gap, which can be defined in either mm or mil units. To specify the units when entering a number, add the mm or mil suffix to the value.
• Increment - shows the current step in wave length when you increase or decrease it during interactive length tuning. Use the 3 or 4 keys while tuning to change the gap by the step value. For example, if the gap is 100mil and the amplitude increment is 20mil and you pressed the 4 key twice during routing, you will get an gap of 140mil. Edit this field to change the gap step, which can be defined in either mm or mil units. To specify the units when entering a number, add the mm or mil suffix to the value.
• Miter - shows the current miter percentage. Enter the desired percentage or use the + and - to change the miter percentage. This option is not available if Rounded style is selected.
• Increment - shows the increment in which the Miter region increases or decreases.

The Help section displays some of the shortcuts that are available while routing.

The Stackup tab allows you to edit the layer properties of the Layer Stack.

The Layer Stack Manager mode of the Properties panel: an Overlay layer (left image), an inner layer (middle image), and a dielectric layer (right image).

• Layer
  • Name - the name of the layer.
  • Manufacturer - the layer manufacturer. 
  • Material - the layer material. This can be pre-defined in the Altium Material Library dialog (Tools » Material Library) in the Constructions field, or user-defined in the Layer Stack. Click  to open the Select Material dialog to choose the desired material for the currently selected layer in the layer stack.
  • Thickness - the thickness of the signal layer.
  • Dk - this is the Dielectric Constant (also referred to as εr in electromagnetics). This indicates the relative permittivity of an insulator material, which refers to its ability to store electrical energy in an electric field. For insulating purposes, a material with lower dielectric constant is better and in RF applications, a higher dielectric constant may be desirable. In addition, the lower the relative dielectric constant, the closer the performance of the material to that of air. This property is critical to matching the impedance requirements of certain transmission lines.
  • Df - this is the Dissipation Factor. This indicates the efficiency of an insulating material by showing the rate of energy loss for a certain mode of oscillation, such as mechanical, electrical, or electromechanical oscillation. In other words, this is the property of a material that describes how much of the energy transmitted is absorbed by the material. The greater the loss tangent, the larger the energy absorption into the material. This property directly impacts the signal attenuation at high speeds.
  • Process - displays the copper plating process that is applied to the base copper that makes up the outer signal layers of the PCB (the Top Layer and Bottom Layer). 
  • Weight - the weight of the copper per unit area, usually expressed in ounces/square foot (e.g., 0.5 oz/ft²).
  • Orientation - this defines which way the components point (orient) on that layer. For the top and bottom sides, this is set automatically in a new board. For other signal layers, it is used for:
    • Rigid flex designs, where components mount on an inner signal layer that becomes a surface layer on a flex section, the software needs to know which way those components point. Use the drop-down to select the required orientation. Choices include: Not allowed, Top, and Bottom.
    • For a design that includes embedded components, the software needs to know which way a component points. Refer to the Embedded Components page for information regarding setting the component orientation in the layer stack. Use the drop-down to select the required orientation. Choices include: Not allowed, Top, and Bottom.
  • Description - enter a meaningful description.
  • Constructions - for dielectric layers, this displays the contructions of the layer. The numerical reference relates to the structure of the woven glass fabric used in the dielectric layer material; these are standard references used by PCB fabricators.
  • Resin - displays the resin percentage of the layer.

• Frequency - this is the frequency at which the material is tested and the value that Dk / Df correspond to a certain frequency. Frequency is also taken from material references.
• GlassTransTemp - this is the Glass Transition Temperature (also known as T_G) and is the temperature at which the resin changes from a glass-like state to an amorphous state changing its mechanical behavior, i.e. expansion rate.
• Note - enter any pertinent notes for the layer.
• Comment - enter any necessary comments for the layer.

• Board
  • Stack Symmetry - enable to add layers in matching pairs, centered around the mid-dielectric layer. When enabled, the layer stack is immediately checked for symmetry around the central dielectric layer. If any pair of layers that are equidistant from the central dielectric reference layer are not identical, the Stack is not symmetric dialog opens.
    When Stack Symmetry is enabled:
    - An edit action applied to a layer property is automatically applied to the symmetrical partner-layer.
    - Adding layers will automatically add matching symmetrical partner-layers.
     

• Library Compliance - when enabled, for each layer that has been selected from the Material Library, the current layer properties are checked against the values of that material definition in the library. 

• Substack - this information is for the currently selected substack (layers, dielectric, thicknesses, etc.,). As you switch from one substack to another, this information will update accordingly (for the currently selected substack).

• Stack Name - enter the substack name. Naming the substack is useful when the X/Y stackup region is being assigned a layer substack.
• Is Flex - enable if the substack is flex.
• Layers - the number of conductive layers.
• Dielectrics - the number of dielectrics.
• Conductive Thickness - this is the sum of the thicknesses of all signal and plane layers (all copper or conductive layers).
• Dielectric Thickness - the thickness of dielectric layer(s).
• Total Thickness - the total thickness of the finished board.

Use the Impedance tab to configure the Impedance Profile requirements. The required Impedance Profile can then be selected in the Routing Width or Differential Pairs Routing design rules.

• Impedance Profile
  • Description - enter a meaningful description. This field is optional and will be displayed wherever the Impedance Profile name is displayed.
  • Type - use the drop-down to choose the impedance type. Choices are: Single and Differential.
  • Target Impedance - enter the impedance you want to achieve.
  • Target Tolerance - enter the tolerance you want to achieve. You should consult with the fabricator to find a realistic value for tolerance that the fabricator can deliver. 
• Transmission Line
  • Etch Factor - the Etch Factor is = T/[(W1-W2)/2], which reduces the total cross-section area of the trace by the thickness of the copper squared. Consult the board fabricator for information about the Etch Factor created by their processes.

• Trace Width - there is a forward/reverse calculation feature available for trace width. The default is for the width to be calculated based on the Target Impedance you entered (forward calculation). That width will probably be a value that the fabricator will not be able to deliver, such as 5.978, and they will want a more sensible value, such as 6.0. You can enter 6.0 into the Trace Width field and press Enter to recalculate the calculated values (Calculated Impedance, Impedance Deviation, etc.). The  button turns gray (becomes inactive) and you are now in reverse calculation mode. If you click the button to make it active, you are again in forward mode and the Trace Width will revert to the calculated value. This feature lets you explore realistic fabricatable width options.
• Calculated Impedance - the software calculates the impedance based on the properties of the materials used to make the board (copper, core and prepreg), and the cross-sectional area of the trace (determined by the width, thickness and etch factor of the trace).
• Impedance Deviation - this is a measure of the difference between what you wanted (target impedance) and what you got (calculated impedance). The software calculates the impedance deviation (what you will actually get based on the material and dimensions entered) based on the properties of the materials used to make the board (copper, core and prepreg), and the cross-sectional area of the trace (determined by the width, thickness and etch factor of the trace).
• Propagation Delay - this is the amount of time it takes for the signal to travel from the sender to the receiver.
• Inductance p.u.l. - the impedance calculator uses the Calculated Impedance value to calculate the inductance per unit length. 
• Capacitance p.u.l. - the impedance calculator uses the Calculated Impedance value to calculate the capacitance per unit length.

• Board
  • Stack Symmetry - enable to add layers in matching pairs, centered around the mid-dielectric layer. When enabled, the layer stack is immediately checked for symmetry around the central dielectric layer. If any pair of layers that are equidistant from the central dielectric reference layer are not identical, the Stack is not symmetric dialog opens.

• Library Compliance - when enabled, for each layer that has been selected from the Material Library, the current layer properties are checked against the values of that material definition in the library. 
• Layers - the total number of layers.
• Dielectrics - the total number of dielectrics.
• Conductive Thickness - the thickness of conductive layer(s). Copper signal layers are referred to as conductive layers.
• Dielectric Thickness - the thickness of dielectric layer(s).
• Total Thickness - the total thickness of the board.

The Via Types tab is used to define the allowed Z-plane layer-spanning requirements of the via(s) used in the design.

• Via Type
  • Name - the name of the via. The software automatically detects the type based on the layers that have been chosen, and names the via accordingly.
  • First layer - the first layer the via spans.
  • Last layer - the last layer the via spans.
  • µVia - enable if a microvia is required.
  • Mirror - when enabled, a mirror of the current via that spans the symmetrical layers in the layer stack is created. This option is available only if the Stack Symmetry option is enabled.
• Board
  • Stack Symmetry - enable to add layers in matching pairs, centered around the mid-dielectric layer. When enabled, the layer stack is immediately checked for symmetry around the central dielectric layer. If any pair of layers that are equidistant from the central dielectric reference layer are not identical, the Stack is not symmetric dialog opens.

• Library Compliance - when enabled, for each layer that has been selected from the Material Library, the current layer properties are checked against the values of that material definition in the library. 
• Substack - this information is for the currently selected substack (layers, dielectric, thicknesses, etc.,). As you switch from one substack to another, this information will update accordingly (for the currently selected substack).

• Stack Name - enter a meaningful substack name. This field is useful when the X/Y stackup region is being assigned a layer substack.
• Is Flex - enable if the substack is flex.
• Layers - the total number of layers in the substack.
• Dielectrics - the total number of dielectrics in the substack.
• Conductive Thickness - the thickness of conductive layer(s) in the substack. Copper signal layers are referred to as conductive layers.
• Dielectric Thickness - the thickness of dielectric layer(s) in the substack.
• Total Thickness - the total thickness of the substack.

The Back Drills tab is used to define the layer-spans that are required to be back drilled. 

• Back Drill
  • Name - the name of the back drill. 
  • First layer - the first layer the back drill spans.
  • Last layer - the last layer the back drill spans.
  • Mirror - when enabled, a mirror of the current back drill that spans the symmetrical layers in the layer stack is created. This option is available only if the Stack Symmetry option is enabled.
• Board
  • Stack Symmetry - enable to add layers in matching pairs, centered around the mid-dielectric layer. When enabled, the layer stack is immediately checked for symmetry around the central dielectric layer. If any pair of layers that are equidistant from the central dielectric reference layer are not identical, the Stack is not symmetric dialog opens.

• Library Compliance - when enabled, for each layer that has been selected from the Material Library, the current layer properties are checked against the values of that material definition in the library. 

• Substack - this information is for the currently selected substack (layers, dielectric, thicknesses, etc.,). As you switch from one substack to another, this information will update accordingly (for the currently selected substack).

• Stack Name - enter the substack name. Naming the substack is useful when the X/Y stackup region is being assigned a layer substack.
• Is Flex - enable if the substack is flex.
• Layers - the number of conductive layers.
• Dielectrics - the number of dielectrics.
• Conductive Thickness - this is the sum of the thicknesses of all signal and plane layers (all copper or conductive layers).
• Dielectric Thickness - the thickness of dielectric layer(s).
• Total Thickness - the total thickness of the finished board.

The Printed Electronics Stackup tab allows you to edit and configure the layer properties of the Layer Stack for a printed design. 

• Layer
  • Name - the name of the layer.
  • Manufacturer - the layer manufacturer. 
  • Material - the layer material. This can be pre-defined in the Altium Material Library dialog (Tools » Material Library) in the Constructions field, or user-defined in the Layer Stack. Click  to open the Select Material dialog to choose the desired material for the currently selected layer in the layer stack.
  • Thickness - the thickness of the signal layer.
  • Dk - this is the Dielectric Constant (also referred to as εr in electromagnetics). This indicates the relative permittivity of an insulator material, which refers to its ability to store electrical energy in an electric field. For insulating purposes, a material with lower dielectric constant is better and in RF applications, a higher dielectric constant may be desirable. In addition, the lower the relative dielectric constant, the closer the performance of the material to that of air. This property is critical to matching the impedance requirements of certain transmission lines.
  • Df - this is the Dissipation Factor. This indicates the efficiency of an insulating material by showing the rate of energy loss for a certain mode of oscillation, such as mechanical, electrical, or electromechanical oscillation. In other words, this is the property of a material that describes how much of the energy transmitted is absorbed by the material. The greater the loss tangent, the larger the energy absorption into the material. This property directly impacts the signal attenuation at high speeds.
  • Frequency - this is the frequency at which the material is tested and the value that Dk / Df correspond to a certain frequency. Frequency is also taken from material references.
  • Description - enter a meaningful description.
  • Color - this is the required color of the solder mask. Click to open a drop-down to set/change the color.
  • Solid - N/A
  • Material Frequency - N/A
  • GlassTransTemp - this is the Glass Transition Temperature (also known as T_G) and is the temperature at which the resin changes from a glass-like state to an amorphous state changing its mechanical behavior, i.e. expansion rate.
  • Note - enter any pertinent notes for the layer.
  • Comment - enter any necessary comments for the layer.
• Board
  • Library Compliance - when enabled, for each layer that has been selected from the Material Library, the current layer properties are checked against the values of that material definition in the library. 

• Substack - this information is for the currently selected substack (layers, dielectric, thicknesses, etc.,). As you switch from one substack to another, this information will update accordingly (for the currently selected substack).

• Stack Name - enter the substack name. Naming the substack is useful when the X/Y stackup region is being assigned a layer substack.
• Is Flex - enable if the substack is flex.
• Layers - the number of conductive layers.
• Dielectrics - the number of dielectrics.
• Conductive Thickness - this is the sum of the thicknesses of all signal and plane layers (all copper or conductive layers).
• Dielectric Thickness - the thickness of dielectric layer(s).
• Total Thickness - the total thickness of the finished board.

• Net - net to have shielding vias placed around.
  • Stagger alternate rows - alternate rows of shielding vias are offset by half of the Grid value when this option is enabled.
• Row Spacing - spacing between rows of shielding vias (edge to edge separation) when the Rows setting is greater than 1.
• Distance - separation from the edge of the shielded net track segments, to the edge of the shielding vias.
• Grid - the distance between the edges of adjacent shielding vias. Shielding vias will not be placed in violation of applicable design rules; if a potential via site would result in a violation then that site is skipped.
• Rows - number of rows of shielding vias.
  • Add Shielding - place a polygon over the area occupied by the shielding vias, connected to the net specified in the Via Net field. The polygon is defined in accordance with the applicable Clearance constraint and Polygon Connect Style design rules.
  • Add Clearance Cutout - include a polygon cutout around the shielded net, set back from the net by the distance specified in the Distance field. Use this when you require a different clearance from the applicable Clearance constraint design rule.

• Net - the net being shielded by the shielding vias.
• Net Class - if the chosen Net is a member of a Net Class, it will be displayed in this field.

• Template - displays the currently chosen via template. Use the dropdown to change the assigned via template.
• Library - displays to which library the via template is linked and includes the option to Unlink the template from said library.

• Net - net that the shielding vias are connected to.
• Via Type - use the drop-down to select the type of via from those available in the layer stack.
• Via Types - click to open the Layer Stack to configure the required via types for the active layer stack.

• Hole Size - size of the hole in the shielding vias.
• Tolerance - negative and positive hole size tolerances allowed for the shielding vias.

• Size and Shape - vias are one of three styles:
  • Simple - the via diameter is the same on all layers
  • Top-Middle-Bottom - the via diameter can be specified for the Top layer, Middle (all internal layers), and Bottom layer.
  • Full Stack - the via diameter can be specified for every signal layer.
• Diameter - diameter of the shielding vias.
• Thermal Relief - check the Direct box then click the  to open the Connect Style dialog to specify the Connect Style.

• Rule - enable this option to allow the existing solder mask expansion rule to take effect on the shielding vias. Check the Mask design category from the PCB Rules and Constraints Editor dialog.
• Manual - enable this option to edit the mask expansion values (below) for these shielding vias.
• Top - enter the required mask expansion for the Top Layer.
• Bottom - enter the required mask expansion for the Bottom Layer.
• Top Tented - if this checkbox is enabled, the mask is closed on the Top Layer for these shielding vias.
• Bottom Tented - if this checkbox is enabled, the mask is closed on the Bottom Layer for these shielding vias.
• Linked - if the Linked option is enabled, the same expansion value is used for both the Top and Bottom layers.
• From Hole Edge - enable this option to calculate the mask expansion from the edge of the drill hole instead of the edge of the via donut.

• Constrain Area - enable to constrain via stitching to a specific area. After selecting the option, you will be taken to the design space. After using the cross-hair cursor to define the constrain area, right-click to return to the dialog.
• Edit Area - click to edit the constrain area.
• Offset (X/Y) - enter the X and Y offset distance(s). The stitching pattern will placed within the constrain area, starting at an offset of the specified X and Y amount.
• Grid - the distance between the center of adjacent stitching vias. Stitching vias will not be placed in violation of applicable design rules; if a potential via site would result in a violation that site is skipped.
  • Stagger alternate rows - alternate rows of shielding vias are offset by half of the Grid value.
• Default Via/Pad - stitching vias are only placed on potential stitching sites if this much clearance exists. Since potential stitching sites are determined by the stitching grid, it is likely they will be further than apart than this setting.
• Min Boundary - stitching vias are only placed on potential stitching sites if this much clearance exists to the edge of Polygon/Fill/Plane regions.

• Net - the net to which the via stitching is currently assigned. Change the net assignment by clicking in the field and choosing a net from the drop down list.
• Net Class - if the chosen Net is a member of a Net Class, it will be displayed in this field.

• Template - displays the currently chosen via template. Use the dropdown to change the assigned via template.
• Library - displays to which library the via template is linked and includes the option to Unlink the template from said library.

• Via Type - use the drop-down to select the type of via from those available in the layer stack.
• Via Types - click to open the Layer Stack to configure the required via types for the active layer stack.

• Hole Size - size of the hole in the stitching vias.
• Tolerance - negative and positive tolerances allowed for the stitching vias.

• Size and Shape - vias are one of three styles:
  • Simple - the via diameter is the same on all layers
  • Top-Middle-Bottom - the via diameter can be specified for the Top layer, Middle (all internal layers), and Bottom layer.
  • Full Stack - the via diameter can be specified for every signal layer.
• Diameter - diameter of the stitching vias.
• Thermal Relief - check the Direct box then click the  to open the Connect Style dialog to specify the Connect Style.

• Rule - enable this option to allow the existing solder mask expansion rule to take effect on the stitching vias. Check the Mask design category from the PCB Rules and Constraints Editor dialog.
• Manual - enable this option to edit the mask expansion values (below) for these stitching vias.
• Top - enter the required mask expansion for the Top Layer.
• Bottom - enter the required mask expansion for the Bottom Layer.
• Top Tented - if this checkbox is enabled, the mask is closed on the Top Layer for these stitching vias.
• Bottom Tented - if this checkbox is enabled, the mask is closed on the Bottom Layer for these stitching vias.
• Linked - if the Linked option is enabled, the same expansion value is used for both the Top and Bottom layers.
• From Hole Edge - enable this option to calculate the expansion from the edge of the drill hole instead of the edge of the via donut.

The options in this section of the panel determine which multi-board objects may be selected in the workspace.

• All Objects button – select remove object filtering so that all types of objects may be selected.
• Object buttons – toggle each object button to enable/disable the ability to select that object type.

• Units – select the measurement units that apply to the multi-board document and its graphic elements.
• Grid Size – set the measured distance between each sheet grid line. Note: this option is not editable in multi-board documents.
• Show Grid – check to display grid lines at the default Grid Size in the document sheet. Click the associated color button () to specify the color of the grid lines in the color selector drop-down, which includes options for preset colors, HEX/RGB color values, and the graphic selection of color shades.
• Snap – when checked, the ghost/preview cursor will snap (jump) to grid line intersections while the editor is in object placement mode. The cursor will also snap to graphic object vertices (corners, etc.,), line midpoints and circle centers.
• Snap Distance – set the distance at which the preview cursor will snap onto the targets outlined above. The preview cursor changes to an orange dot when a midpoint, vertex, or center is snapped to.
• Document Font – set the font size, style and any additional font attributes that will be used for the text associated with all objects in the document sheet. For any given object, the font settings may be overridden in its corresponding Properties panel mode, which is enabled when that object is selected.
• Sheet Border – click the associated color button to set the zone border line and character color for the document sheet.
• Sheet Color – click the associated color button to set the background color for the document sheet.

Formatting and Size

• Template mode – set the page size and format by selecting from a range of predefined schematic sheet templates. The list includes templates found in the location specified in the Data Management - Templates page of the Preferences dialog. Note that a default schematic sheet to be used for new multi-board documents may be defined in the System - New Document Defaults page of the Preferences dialog.
  • Template – use the drop-down menu to select from a list of standardized page templates, and if required, use the  button to refresh the template and drawing.
  • Width/Height – the dimensions of the current page size shown in the current document units (see the General section above).
  • Source – use the browse button () to navigate to and select an alternative template source in the schematic *.SchDot format.
• Standard mode – set the sheet size to a standard page format.
  • Sheet Size – use the drop-down menu to select from a list of standard page dimensions.
  • Width/Height – the dimensions of the current page size in the current document units.
• Custom mode – set the sheet size to specified custom dimensions.
  • Width – enter the required sheet width measurement.
  • Height – enter the required sheet height measurement.

Margin and Zones

Defines the size of the sheet border graphics and its zone divisions. Uncheck the Show Zones box to hide the zone divisions in the border graphics.

• Vertical – set the number of divisions (rows) in the vertical sheet margin. The alpha-numeric zone labeling type is defined by the Origin and Letter Position settings.
• Horizontal – set the number of divisions (columns) in the horizontal sheet margin.
• Origin – sets which corner of the document sheet(s) the perimeter zone alpha-numeric indicators will begin from (zone position A-1 or 1-A).
• Letter Position – set where the letter zone indicators are placed on the document sheet, either in the horizontal perimeter zones (columns) or the vertical zones (rows).
• Margins – set the distance (in the current units) between the page edge and each of the four border lines as indicated by the arrows associated with each entry field.

• Dash Pattern – the line/spacing definitions for the dashed Line options in units of 0.02mm (when in metric mode). For example, a pattern Value of 20,10,20 defines a repeating 0.4mm, 0.2mm, and 0.4mm dash arrangement with a cycle length of 1mm (50 units in total). A custom dashed line option can be created through the button and removed with the button. Use the button to restore the default entries and their values.
• Line Thickness – the weight or thickness of the available Line style options. A custom line thickness option can be created through the button and removed with the button. Use the button to restore the default entries and their values.

The Properties panel Parameters tab lists all available User and System parameter Name/Value pairs available in the current project document.

• Parameter Name and Value columns – lists the available parameters grouped by type, where User and System parameters are indicated by their associated icons.
  • User parameters () – parameters included in the document sheet template or those manually added through the panel. Both the Name and Value of User parameters can be edited directly in the list.
  • System parameters () – parameters included in the applied project template or those added through the Parameters tab of the Project Options dialog (Project » Project Options). System parameters cannot be edited through the Properties panel list.
• List filter options – select the icon to enable/disable Project level parameters in the list. Select the icon to enable/disable System parameters in the list.
• Add button () – select to add a new User parameter to the Parameters list. Use the button to remove a selected User parameter from the list.

• Production Quantity - the number of boards to be built. It is important to define this field as this is used during supply chain searching to check component availability from the suppliers.
• Currency - the preferred currency to display component prices. Exchange rates for currency conversion are refreshed daily provided you are signed in to your Altium account. When you disconnect from Altium (on the System - Account Management  page of the Preferences dialog), access to these updated rates is lost. In this situation, there is an option in the BOM reports dialog to use cached data.
• Price Per Board / Order Price grid - Price per Board is the sum of the prices of each individual item detailed in the BOM Items grid; the Order Price grid is this value times the Production Quantity. If target prices have been defined for each BOM Item, the Target column reflects these. To enter a target price for each BOM Item, enable the TargetPrice column on the Columns tab of the panel, then enter the price of each item in the Item grid.

Supply Chain information is presented in the lower region of the ActiveBOM interface, showing a manufacturer component on the left with one or more colored supplier tiles to the right of it. This region displays data when valid supply chain information can be identified for a BOM Item. Each of these Manufacturer & Supplier(s) Details rows is referred to as a Solution. The manufacturer details are abbreviated to MPNs (Manufacturer Part Numbers) and the supplier details are abbreviated to SPNs (Supplier Part Numbers).

• Solutions per Item - the number of manufacturer parts you would like to be located for each BOM Item.
• Suppliers per Solution - the number of suppliers you would like to be located for each manufacturer part.
• Solutions
  • Exclude Invalid SPNs - select to exclude invalid SPNs.
  • Favorite Suppliers List - opens the Favorite Suppliers dialog in which the overall list of Suppliers can be configured for this BomDoc.
  • Manufacturer Link - opens the Define Manufacturer Link Fields dialog in which the schematic component parameters that hold the Manufacturer Name and Manufacturer Part Number are identified. If there are unmanaged parts present in the design (parts not placed from a managed content server that also do not have supplier details), ActiveBOM can query the Altium Parts Provider and attempt to find that part.

This region is used to configure how the BOM Items should be grouped in the BOM Items grid.

• Items
  • Show not Fitted - if the PCB project includes variants and the chosen variant has parts set to Not Fitted, enable this to display the Not Fitted items in the BOM Items grid.
  • Designator Grouping - the Base and Consolidated view modes show common parts on a single row in the BOM Items grid. Use this option to configure if the designators are displayed individually or in ranges when a row displays multiple parts.
  • Component Grouping - opens the Component Grouping dialog. In Base view or Consolidated view, ActiveBOM identifies components as being the same when they share the same ItemID (managed) or LibRef (unmanaged). Enable parameters in the dialog to further refine how components are to be grouped.

BOM Sets provide a way of capturing the layout and configuration of the BOM Items grid and saving it as a named Set. Any number of BOM Sets can be defined.

• Current BOM Set - click the icon to apply that BOM Set to the BOM Items grid.
• Add - configure the visibility, order, and width of the columns, then click Add to capture that configuration as a BOM Set. To edit the BOM Set name click once to select it, then click a second time to edit the string.
• Update - if the configuration of the BOM Items grid is changed, click Update to re-save this configuration.
• Delete - click the button to remove the currently select BOM Set.

ActiveBOM performs comprehensive checking of each BOM Item and any supply chain data that has been detected for that item.

• Violation Type grid - displays a list of each type and quantity of violations currently present in the BomDoc. Click the filter icon to display only those BOM Items that fail that BOM Check. Note that a BOM Item can fail multiple BOM Checks.
• BOM Checks  - click the icon to open the BOM Checks dialog in which the Report Mode can be configured for each possible Violation Type.

This region of the panel is used to configure which parameters are displayed for each BOM Item and the data sources that are available for those parameters.

• Sources - in addition to the data added directly into the BomDoc ( ), the default data sources available in ActiveBOM are the schematic component parameters ( ) and the content server component parameters for managed Items ( ). From these sources, ActiveBOM generates the main project BOM Item grid. The BOM also can also include information taken from the following additional data sources:
  •  PCB - enable to include PCB location / rotation / side of board data in the available Columns for the each of the components.
  •  Database - enable to load additional component parameters from an external database (*.DbLib, *.SVNDbLib, or *.DbLink).
  •  Document - enable to include all detected schematic document parameters across all schematics in the PCB project in the available Columns.
  •  Altium Cloud Services - enable to access a broad range of additional component data for those BOM Items that have been identified by the Altium Parts Provider and show a supply chain solution.

• Columns - list of all available sources of part information available to ActiveBOM. The Columns region can be sorted by clicking on any of the heading fields.
  • Visibility - each row has an eye icon; click to control the visibility of that column in the main BOM Items grid.
  • Source - displays an icon to show from where that parameter is sourced.
  • Column Name - the name of the property/parameter as defined in the source document or as entered for a user-created BomDoc column.
  • Alias - if required, an alias can be defined to rename a column.
  • Source display checkboxes - below the column grid is a row of checkboxes, one checkbox for each data source currently enabled for the ActiveBOM . Clear the checkbox to remove all parameters from that source from the BOM Items grid.
  • Add - click to add a new Custom Column to the BOM Items grid.