Controlled Depth Drilling (CDD), also known as back drilling, is a technique used to remove the unused portion, or stub, of copper barrel from a thru-hole in a printed circuit board. When a high-speed signal travels between PCB layers through a copper barrel, it can be distorted. If the signal layer usage results in a stub being present and the stub is long, that distortion can become significant.
These stubs can be removed by re-drilling those holes with a slightly larger drill after the fabrication is complete. The holes are back drilled to a controlled depth close to, but not touching, the last layer used by the via. Allowing for fabrication and material variations, a good fabricator can back drill holes to leave a 7mil stub; ideally, the remaining stub will be less than 10mil.
Most commonly used for vias, and also for press-fit backplane connectors, back drilling provides a cost-effective solution to help manage the signal quality for high-speed signal paths. It offers a lower cost than the sequential lamination technique used for blind and buried vias.
Back drilling is achieved by:
Via/Pad hole size + 2 x Oversize setting in the applicable Maximum Via Stub Length (Back drilling) design rule.
Instruct the software that there are holes to be back drilled by adding a Maximum Via Stub Length (Back drilling) design rule. The scope of the design rule defines which vias or pads are to be drilled. Typically you only back drill selective nets, such as the high-speed nets, in which case the scope could be something like
For example, if the scope is
InNetClass('IO'), then all vias and pads in those nets can potentially be back drilled. The holes that are actually back drilled will depend on which layers those signals are routed on, and which back drill pairs have been defined. If a hole has no connections on the layers within the back drill layer range, that hole will be back drilled.
To further limit the back drilling operation, tighten the rule scope. For example, if you only want to back drill the vias and not the thru-hole pads, you could change the rule scope to
InNetClass('IO') and IsVia.
When you back drill a thru-hole barrel, an oversized drill bit is used to remove the unwanted copper.
All layer-to-layer drill actions are defined by adding a start layer-stop layer drill definition in the Back Drills tab of the Layer Stack Manager. The tab is not available until the Back Drill feature is enabled in the Layer Stack Manager, select Tools » Features » Back Drills to enable it, or click the button and choose Back Drills.
Once the feature has been enabled, switch to the Back Drills tab and click the button to add a new Back Drill definition.
The next step is to configure the layers that are to be back drilled, as described below.
The back drilling depth is a calculated value, not a number you enter into a dialog. You define the first and last layers and the software calculates the drill depth required to back drill through all layers between the first and last layers, including the first layer thickness, but not the last layer thickness (back drilling stops at that layer). The First layer and Last layer are defined in the Properties panel in Layer Stack Manager mode (with the Back Drills tab selected). There must be defined back drills in the layer stack in order to access the Back Drill region of the Properties panel as shown below.
The hole is drilled up to, but not touching, the last layer specified in the Last layer field. The depth of the drill action is defined by:
Depth = Sum of all layer thicknesses from first layer to last layer - last layer thickness
The layer thicknesses are the values entered into the Layer Stack Manager.
When the Back Drills tab of the Layer Stack document is active, the Properties panel is used to define the layer-spans that are required to be back drilled.
The drill diameter calculated from:
Back Drill Size = Via/Pad hole size + 2 x Design Rule Backdrill Oversize
Rather than entering a specific drill size for back drilling, define how much larger the back drill is over the original via or pad hole size. The oversize is specified as a radial amount in the design rule, along with any tolerance requirements for the back drilled holes, as shown below.
The display of holes that are back drilled includes an additional two-color ring with the following properties:
Back drills can also be located and viewed via the Hole Size Editor set the mode in the PCB panel.
In the image below, the 14mil sized back drill has been clicked on in the panel. The display zooms to those back drilled holes, highlighting them with the start and stop layers. Note that there are seven back drilled vias shown in the panel, but only five are shown in the design space. That is because the second and third vias are back drilled from both the top side and the bottom side, and since the top layer is the active layer, those vias are currently shown as a top-side back drill.
The Maximum Via Stub Length (Back drilling) design rule is used for both locating potential back drill sites, and also for testing for remaining stubs.
During a design rule check, all applicable vias and pads are tested for stubs of a length greater than the Max Stub Length configured in the design rule. Note that all pads and vias targeted by Maximum Via Stub Length (Back drilling) design rules are tested, not just those that are back drilled or those that have not been back drilled.
The rule is checking the length of any remaining stub. In the image below, even though the via has been back drilled (in accordance with the defined back drills), the remaining stub is greater than the 7mil allowed by the applicable design rule, so a rule violation is flagged.
Generating output for back drilling is transparent. If additional drill-type output files are needed, these are automatically generated.
Back drilling is very similar to using blind vias (these also require a first/last layer pair to be defined in the Layer Stack Manager), which specifies the drilling requirements between this pair. The difference is that blind vias are plated, whereas back drilled vias or pads are an unplated drill event. Un-plated holes are essentially a post-fabrication process, i.e. the drilling occurs after the etching, lamination, drilling, and thru-hole plating.
To generate a summary report of all back drill events in the design, right-click in the Unique Holes region of the PCB panel in Hole Size Editor mode then select Backdrill Report from the context menu.
The Report Preview dialog will open. Click the Export button to select the file type, the location in which you want the file located, then enter the file name.
Drill symbols are automatically assigned and can be reconfigured in the Drill Symbols dialog. The symbols are displayed on the Drill Drawing layer in the PCB design space if the Show Drill Symbols option is enabled in the Drill Symbols dialog. The dialog can be accessed by right-clicking in the Unique Holes region of the panel or on the Drill Drawing layer tab, as shown below.
Because back drilling involves drilling at the same location with different sized drill bits, drill symbols will appear stacked at these locations. Use the layer-pair selector to control which layer pair is currently being displayed, as shown in the images below.
A placed drill table can be configured to show all drill layer pairs, or it can be configured to show a specific layer pair. The image below is from a design with back drilling from both the top and bottom sides of the board, so three tables have been placed. Note the Drill Layer Pair column; it indicates the function of each table.
For each drill pair defined, NC drill output will produce a unique drill file. Note that it also produces a separate file for each hole-shape type (round, rectangular or slotted).
The drill report file (<ProjectName>.DRR) includes a summary of the drill tool assignments, their sizes, and the role and name of each of the various drill files generated.
The NC Drill Setup dialog includes a Generate separate NC Drill files for plated & non-plated holes option. The NC drill output files always include all drill events. If this option is enabled, the plated and non-plated drill events are instead output into separate files. They are identified by an additional string in their filename in the format <DesignName>-Plated, or <DesignName>-NonPlated.
Back drill events are always output to their own files, each identified by a unique file extension. For example, these could be named <DesignName>-BackDrill.TX3 for the top-side back drill events and <DesignName>-BackDrill.TX4 for the bottom-side back drill events.
Rather than just being a standard for outputting fabrication data for a set of PCB layers (which requires the addition of NC drill files for bare-board fabrication), Gerber X2 outputs all of the data needed to input the design into the fabricator's CAM process. Gerber X2 is configured in the Gerber X2 Setup dialog.
If there are back drilled holes in the design, the Gerber X2 output will automatically include additional drill files with a filename, such as:
These back drill files include Gerber X2 format instructions, such as:
This line instructs the CAM software to treat the contents of this file as non-plated blind drill events, between signal layers 1 and 3.
Drill sizes are defined using apertures, whose definition is preceded by an instruction that declares them as drill sizes.
For ODB++ output, there will be an additional drill folder created for each back drill layer pair defined. These will have names such as \drill1, \drill2. These folders include the standard ODB drill files.
Support for IPC-2581 will be added in a future update.
Draftsman is an ideal tool for creating high-quality documentation for your design. If there are back drill type layer-pairs defined in the design, the Layer Stack Legend will display these, making it easy to quickly establish their presence.
You can also configure the drill table to show each back drill layer-pair, making it easy to quickly identify the drill sizes and hole count required for back drilling.