Internal Power and Split Planes

Power planes are special solid copper internal layers, typically used to provide an electrically stable ground or power reference throughout the printed circuit board. This article investigates using internal power and split planes.

Plane Basics

The PCB Editor supports up to 16 internal power planes. You can assign a net to each of these layers or share a power plane between a number of nets by splitting it into two or more isolated areas. Pad and via connections to power planes are controlled by the Plane design rules. Power planes are created in the negative. Objects placed on the power plane layer become voids in the copper, the remaining regions will become solid copper.

PCBs are fabricated from an even number of copper layers, so you may need to add another signal or plane layer to return to an even number of layers.

Creating Internal Planes

Internal power planes are added to a PCB design through the Layer Stack Manager dialog (Design » Layer Stack Manager). To add a new internal plane, highlight the existing layer that you want the internal layer created under and press Add Plane. A new internal plane is added to the layer stack. To set or edit the properties of the new internal plane, double-click on the new internal layer name to change the name, copper thickness, net name and pullback via the Edit Layer dialog.

Viewing Planes

To view an internal plane, including power types, you must display the plane layer first by enabling the Show option in the View Configurations dialog (Design » Board Layers & Colors) for that layer. Click the power plane layer tab, for example, at the bottom of the workspace.

If necessary, select Tools » Split Planes » Rebuild Planes on Current Layer or Rebuild Split Planes on All Layers to recalculate and redraw planes. You may find displaying the pad holes layer and multilayer useful as well. Use the SHIFT + S shortcut keys to toggle various Single Layer Mode settings that help highlight objects of interest.

In 3D viewing mode [shortcut: 3 ] you can see physical representations of all internal plane objects. Further to viewing, the 3D environment enables you to travel right through the board, making true internal planes inspection very easy.
If you click on an internal plane, the entire area within the pullback tracks is highlighted. You can also select internal planes and their contents to view using the Split Plane Editor mode available from the list at the top of the PCB panel.

Pullbacks and Power Planes

When a power plane is added, a set of pullback tracks are automatically created around the board shape to pull back the plane from the edge of the board. These tracks are actually twice the pullback setting specified in the Edit Layer dialog and they are placed with half their width inside the board shape and half outside.

Pullback tracks cannot be edited on screen as their width is defined in the Layer Stack Manager dialog only. If the pullback value for an internal plane has been changed, these tracks will be regenerated automatically.

Creating Blow Out Sections

Connecting Pads and Vias to a Power Plane

Connections to pads and vias are displayed on a power plane according the Plane design rules set in the PCB Rules and Constraints Editor dialog (Design » Rules). You can create additional rules for pads and vias that have specific connection or non-connection requirements.

Thermal Relief and Direct Connections

Through hole pads and vias can be connected to a power plane by either a direct connection or a thermal relief connection. Thermal relief connections are used to thermally isolate the connected pin from the solid copper plane when the board is soldered. The design rules in the PCB Editor allow you to define the thermal relief shape of each or all pads connecting to the power plane.
The Power Plane Connect Style design rule specifies the style of the connection from a component pin to a power plane. Three connection options are available

  • direct connections (solid copper to the pin),
  • thermal relief connections, or
  • no connection

Special support is also provided for connecting SMD power pins to power plane layers. SMD pads on a net that is connected to a power plane are automatically tagged as connected to the appropriate plane. The autorouter completes the physical connection for these pads by placing a fanout - a short track and via which is relief or direct connected to the plane layer.

When a net is assigned to a power plane, a small cross will appear at each pad on the net on the appropriate power plane layer. The cross will look like a '+' for a relief connection, or an 'x' for a direct connection. As direct connected pads have solid copper to the pin, they show the plane color up to the pad hole.

{Note} There are limitations to the type of thermal relief shape when a design is output as Gerber files. Two spoke thermal relief connections are not natively supported by the Gerber format RS-274X and so any two spoke thermal reliefs will be converted to four spokes.{Note}

Pads that do Not Connect to a Power Plane

Pads not connecting to the plane are isolated from it by a region of no-copper. This region of no-copper is specified in the Power Plane Clearance design rule as a radial expansion around the pad hole.

Design rules are hierarchical, so you can add new rules to override others. Make sure you set the priority order from the PCB Rules and Constraints Editor dialog, i.e. the order in which multiple design rules of the same type are applied.

Connecting Vias to Power Planes

Like pads, vias automatically connect to an internal power plane layer of the same net name. The via will connect in accordance with the applicable Power Plane Connect Style design rule. If you do not want vias to connect to power planes, add a Power Plane Connect Style design rule with a connection style of No Connect and a scope query of IsVia.

Fabrication Considerations

Check with your fabricator for suitable dimensional properties for any thermal relief connections. Also check that pads or vias that do no connect do not completely surround a connected pad as this may accidentally cause the connected pad to become isolated and disconnected. Ensure not too much copper is removed and that a balance is struck between maximum copper and affordable manufacture.

Disconnecting Pads and Vias from the Plane

You can use queries in the Power Plane Connect Style design rules to further limit which pads or vias connect or not to a power plane. Pads can be targeted by the designator name or physical properties, such the pad size. Since vias have no designators, they must be targeted by physical properties, such as the via diameter.

Scoping Specific Pads & Vias that do not Connect to a Power Plane

To disconnect, for example, only pads with a specific designator name starting with U7-, you could use the (ObjectKind = 'Pad') and (Name Like 'U7-*') query to set the scope for a Power Plane Connect Style design rule. The connection style would be set to No Connect. Another query such as (ObjectKind = 'Pad') and (HoleSize = 25) would target only those pads with a hole size of 25mils.
When working with vias you do not wish to connect, you could modify vias to contain a special property to uniquely identify them, such as a different via diameter, and then scope a new Power Plane Connect Style design rule with a No Connect connection style to match only those vias. The query (ObjectKind = 'Via') And (ViaDiameter = '24') could be used to target vias with a diameter of 24mil, for example. The query InNet('VCC') and IsVia could be used to target just vias that are attached to the net VCC.
Alternatively, if you cannot select vias using the methods above, you can convert them to free pads and then use pad names to set the scope. To do this, select the vias you do not wish to connect, convert them to free pads (Tools » Convert » Convert Selected Vias to Free Pads) and assign the same Designator name to them all, e.g. NoPlaneConnect. Then add a new Power Plane Connect Style design rule and specify the scope (ObjectKind = 'Pad') and (Name = 'Free‑NoPlaneConnect') for the rule. Also select No Connect as the Connect Style. All free pads named NoPlaneConnect will be disconnected from all of the power plane layers.

Removing Internal Power Planes

Before an internal plane may be deleted, all primitives must be removed from the plane and the net must be disconnected from the plane.
To remove an internal plane, select all primitives on the current plane layer [shortcut: S, Y] and delete them. Now disconnect the internal plane's net in the Layer Stack Manager dialog by setting the net name to No Net. The internal plane can then be deleted from the Layer Stack Manager dialog by pressing the Delete button.

{Info}Pullback tracks around an internal plane cannot be removed as they are based on the board shape and are automatically generated.{Info}

Split Planes

A split plane is an enclosed region on an internal plane that divides the plane into separate electrically isolated areas. Each region is defined by placing boundary lines to encompass all the pins on that net. Each area is then assigned to a different net which creates two or more split planes on the one internal power plane layer.
Power planes can be split into any number of separate regions. This splitting process is like cutting or slicing the plane into sections where the width of the line you place defines the separation distance. Power planes are constructed in the negative, so these special boundary lines become a strip of no-copper, thereby creating the separation between this net and the adjacent net(s) on the plane.

Typically, the net with the greatest number of pads is first assigned to the internal plane, then regions are defined (split off) for the other nets that you wish to connect via this plane. Any pads which cannot be encompassed in the split plane region continue to display a connection line, indicating that they must be connected on a signal layer.
Split power planes are fully supported by the Design Rule Checker. However, they are not recognized by Signal Integrity as the power plane is assumed to be a continuous copper layer in Signal Integrity. Netlist extraction in the CAM Editor does not support Altium Designer mode split planes because it is unable to define the polyline that describes each region.

Using Multiple Split Planes in a Design

Splits within splits (nested splits or islands) are supported so you do not need to wrap an outer split around the inner split. If you wish to further divide a split plane, you can continue to add objects on the power plane layer inside an existing split plane to create other electrically-isolated regions.

Display Tips when Defining a Split Plane

When you define a split area in a power plane, it can sometimes be difficult to see all the pads that the split area needs to encompass. To make the pads for the net that you want to connect to the split plane more visible, the following techniques are suggested before you start.

  • Recalculate and redraw internal planes by selecting Tools » Split Planes » Rebuild Planes on Current Layer / Rebuild Split Planes on All Layers .
  • Use 3D mode [shortcut: 3 ] to view physical representation of the planes, including void areas and thermal relief connections. To make travelling through the board in 3D easier, scale the board thickness to increase the vertical distance between layers. This control is found in the Physical Materials page (used by 3D view configurations) of the View Configurations dialog (Design » Board Layers & Colors).
  • Display only a minimum of layers, e.g. the Keep Out layer, the Multilayer, any mechanical layers needed and the power plane which is being used. Disable the other layers in the View Configurations dialog.
  • Hide all the connection lines (View » Connections » Hide All). On occasions, it may useful to display an individual net that you want to create a split plane for (View » Connections » Show Net).
  • Set the color attribute of each net on the split plane to a different color by selecting Nets in the PCB panel and double-clicking on a net name to display the Edit Net dialog.
  • To display all pads associated with a net, click on that net on the internal plane in the PCB panel to mask out all other pads.
  • Assign the net with the largest number of pads to the internal power plane and then use queries such as InNet('A') or InNet('B') in the PCB List panel to show the nets, e.g. some with thermal relief and some without, to distinguish between the pads to be included in a new split plane.
  • To display just the objects and primitives on internal planes, use the query OnPlane in the PCB Filter panel.

Defining Split Planes

In Altium Designer, you can place any configuration of lines, arcs, tracks and fills across an internal power plane to define a split plane. As soon as these isolate a portion of the plane from the rest, a new split plane is created. A net is then associated with the new split plane.
The easiest way to define split planes is to use the Place » Line command and draw the boundary of the split plane on the power plane. This creates a line in the artwork to leave off copper which in turn splits the planes. The line width becomes the separation width. When you right-click to exit line placement mode, the plane is analyzed and the independent split region is created. To change the separation width between the split plane and the internal power plane during line placement, press the TAB key to display the Line Constraints dialog and change the Line Width field.

image028.gif!

To divide a power plane into two split planes, you can draw a line straight across the board from pullback track to pullback track. As long as the lines connect to the pullback tracks, they will form an isolated area and therefore create the polygon type object that identifies the split plane. Make sure the lines connect; the cursor changes to a large circle in a cross when lines connect.

Check with your fabricator if you are unsure of minimum no-copper regions.

You can create an enclosed shape out of the lines, arcs and fills to define an unusually shaped split plane. You can also use existing lines, arcs, fills or tracks on the internal layer to form part of the boundary; as long as they connect to form an enclosed area, a split plane is formed.

Using Arcs, Fills and Tracks

It is recommended if you use arcs to split the plane that you place a short track segment between the arc segments. Note that using a fill (Place » Fill) will not create a split plane; it will only create a void area. You could use fills to create the outside edges of the split plane by placing them instead of lines, for example.
If you place tracks instead of lines using the Place » Interactive Routing command, make sure the tracks are set to No Net and the split plane is associated with the appropriate net name instead.

Assigning a Net to a Split Plane

To check if each split region is correctly defined, click once on a split and, if it is a closed region, only that area will highlight.

If the area highlights, double-click to check or set the net assignment. Select the split plane's net name from the drop-down list in the Split Plane dialog.

The color of the split plane is a darker, semi-translucent shade of the net color. Change the net colors by selecting Nets in the PCB panel and double-clicking on a net name to display the Edit Net

Legacy Split Plane Mode

If you are importing a PCB from earlier versions of Protel, the Protel Import Wizard allows you to operate in legacy split plane mode if you disable the Convert Split Plane Objects To DXP Split Planes option before importing. The old Place » Split Plane command, available in previous versions, then becomes active for you to create a split plane. To take a board with split planes back to a previous version of Protel, you must use the old Split Plane command.

This mode will continue until you convert your board to the new plane mode, which cannot be undone.

Placing Tracks on Power Planes

Since power plane layers are constructed in the negative, a track placed on a power plane layer creates a void in the copper and so no connection is made. Therefore, you cannot use a single track on a plane layer to route a net. If you wish to route a net on a power plane layer, you have to create a very thin island of copper that is the size of the track you want to use. By creating a boundary of lines around the area that will act like a track (Place » Line), you create a split plane that can then be assigned to the net required.
Alternatively, if there are a number of connections to be routed on the same layer as the plane, it is probably more efficient to use a signal layer to route the connections and then use a polygon plane (copper pour) to create the power plane.

Reviewing and Editing Split Planes

You can review and edit split planes in the PCB panel by selecting the Split Planes Editor from the list at the top of the panel. From here, you can select the plane to display by clicking on the plane name, which then lists any split planes and their nets on that power plane.
Click on a split plane name in the Split Planes and Nets section to show the pads and vias on that split plane. Double-click on a split plane name to open the Split Plane dialog, where you can edit the net associated with the split plane, or right-click to select an option from the pop-up menu.
In 3D viewing mode [shortcut: 3 ] you can see physical representations of all internal plane objects. Further to viewing, the 3D environment enables you to travel right through the board, making true planes inspection very easy.
Recalculate and redraw internal planes after editing by selecting Tools » Split Planes » Rebuild Planes on Current Layer or Rebuild Split Planes on All Layers.

Deleting Split Planes

Since a split is formed when a region on a plane is isolated, removing any object that forms the split boundary will remove that split. So, to delete split planes, delete the bounding primitives, e.g. the lines or other primitives creating the outline of the split plane. Remember that pullback tracks can only be deleted by removing the internal plane from the layer stack.

Design Rule Checking Split Planes

You can check and report on split planes during Batch design rule checking (DRC) for the following rules:

  • Broken planes
  • Dead copper regions
  • Starved thermal connections.

These options are available in the Report Options folder in the Design Ruler Checker dialog, accessed through the menu Tools » Design Rule Check, under Split Plane DRC Report options. Enable the desired options to have them checked and reported during Batch DRC.
When the report is created, any breaches of these rules is displayed in the report. You can click them and the associated error is displayed in the PCB Editor.

Broken Planes

Broken planes occur when an area of the plane that has connectivity to the net becomes electrically disconnected from the rest of the plane. An example where this may occur is a connector that is placed across a split plane, but not connected to it. The voids around the pins join to completely cut through the plane copper, effectively breaking it into two parts.

Dead Copper

Dead copper refers to sections of copper that have no connectivity to the net and which also become electrically disconnected from the original plane. An example where this may occur is a connector (not connected to the plane) with closely spaced pins, in which the voids around the pins join to isolate areas of plane copper from the rest of the plane.

Starved Thermal Connections

  • Split plane DRC checks are Batch mode only.
  • You need to run Batch DRC again to remove error markers or use Tools » Reset Error Markers .
  • Recalculate and redraw internal planes after editing by selecting Tools » Split Planes » Rebuild Planes on Current Layer / Rebuild Split Planes on All Layers .
  • Broken planes and dead copper checks require the Un-Routed Net rule (Electrical category) to be Batch enabled.