Coupons
Help
  • FAQ
    browse most common questions
  • Live Chat
    talk with our online service
  • Email
    contact your dedicated sales:

Plated Drill Holes in PCB Manufacturing: PTH Design and DFM Requirements

What This Video Covers

This video explores why PCB manufacturers verify plated hole attributes before starting fabrication and how drill file information affects plating decisions. Through three real manufacturing cases, it demonstrates the relationship between plated through-holes (PTH), copper pads, and annular ring requirements.

In one case, 450 holes were marked as plated in the drill file but had copper pads on only one side. The CAM team requested clarification because the missing pad could affect the reliability of the hole-wall-to-pad connection. The final decision was to retain plating, add bottom-side annular rings, and open the solder mask. Another case demonstrates how plated holes connect thermal pads to inner copper layers, while an isolated hole with insufficient annular ring support may be better classified as non-plated.

These examples highlight the importance of accurate drill file attributes and early design-for-manufacturing (DFM) reviews. Before requesting an instant PCB quote, engineers should verify PTH and NPTH definitions, copper pad geometry, and manufacturer-specific annular ring requirements. For projects requiring multiple fabrication stages, coordinating these details with PCB assembly services can also help prevent downstream production issues.

 

Key Highlights

  • Plated holes require reliable copper connections: PTH designs must account for the relationship between the plated hole wall, copper pads, and annular rings on the relevant board surfaces.
  • Drill file attributes must match the actual PCB design: Incorrect PTH/NPTH classifications or missing pad geometry can trigger CAM clarification and fabrication delays.
  • Annular ring requirements influence manufacturing decisions: Thermal connection holes, one-sided pad designs, and isolated small holes require different evaluations based on their electrical and mechanical functions.

 

Why PCB Manufacturers Check Plated Hole Attributes in Drill Files

PCB drill files communicate the location, size, and manufacturing attributes of holes that need to be created during fabrication. One of the most important distinctions is whether a hole should be plated or non-plated.

A PTH hole in PCB receives a conductive copper layer along its drilled barrel. This copper can connect copper features on different PCB layers, allowing electrical signals, power, or ground connections to pass through the board. By comparison, a non-plated through-hole (NPTH) does not receive conductive barrel plating and is generally used for mechanical purposes such as mounting, positioning, and component clearance.

The challenge occurs when the drill file identifies a hole as plated but the copper artwork does not provide the expected pad geometry. In the featured manufacturing case, 450 holes were marked as plated, but the top side contained pads while the bottom side did not. This discrepancy required the CAM team to confirm the intended design before production.

From a manufacturing perspective, the drill file and copper layer data must be evaluated together. A plated designation alone does not establish whether the surrounding copper geometry is sufficient for reliable fabrication. The manufacturer must also consider annular ring requirements, layer connectivity, solder mask openings, and the intended function of the hole.

PCB drill file showing plated through-hole locations and missing bottom-side copper pads during CAM review

 

How Annular Ring Requirements Affect Plated Through-Hole Reliability

The annular ring is the copper area surrounding a drilled hole. It provides the connection between the plated barrel and the copper pad or land on the PCB surface.

During PCB fabrication, drilling creates the hole through the board. Subsequent desmear, electroless copper deposition, and electroplating processes establish a conductive copper layer along the hole wall. The resulting barrel must connect properly with the copper features designed around the hole.

If the annular ring is too small, drilling misregistration or other manufacturing variations can reduce the remaining copper around the hole. In severe cases, this can result in breakout, where the drilled hole extends beyond the intended pad boundary.

The risk is particularly important for multilayer PCB designs. A plated hole may need to connect multiple copper layers, and inadequate capture geometry can compromise the intended connection. Depending on the design, this may contribute to open circuits, reduced connection reliability, or manufacturing yield problems.

However, the annular ring requirement is not a universal fixed value. It depends on the fabricator's drilling tolerances, finished hole requirements, layer registration capability, board thickness, and applicable design standards.

For this reason, engineers should confirm minimum annular ring requirements with their PCB manufacturer rather than relying on a single generic design value.

Annular Ring Design Considerations

Design condition Manufacturing concern Recommended action
Adequate annular ring on both sides Better support for the plated barrel connection Confirm against fabricator specifications
Pad exists on one side only Missing surface copper land may affect connection geometry Request CAM review and confirm intended design
Very small annular ring Increased risk of breakout due to drilling misregistration Increase pad diameter where possible
Plated hole connecting inner layers Requires reliable layer-to-barrel connectivity Verify copper capture on connected layers
Isolated hole without copper connection Plating may provide no intended electrical benefit Confirm whether NPTH is appropriate

 

Real PCB Manufacturing Cases: When Should a Hole Be Plated?

The correct plating decision depends on the hole's electrical function, surrounding copper geometry, and mechanical requirements. The video presents three practical examples that demonstrate why manufacturers cannot rely on drill file attributes alone.

Case 1: 450 Plated Holes With Pads on Only One Side

In the first order, the drill file classified all holes as plated. However, 450 holes had copper pads on the top side only, with no corresponding pads on the bottom side.

The CAM team identified this discrepancy and contacted the customer before fabrication. The concern was whether the missing bottom-side copper geometry was intentional or an incomplete design.

The customer confirmed that the holes should remain plated. The agreed solution was to add annular rings on the bottom side and open the solder mask in those locations.

This case illustrates an important DFM principle: a plated hole must be evaluated together with its copper artwork. If the intended plating function requires surface copper connections, the manufacturer needs sufficient pad geometry to support the design.

For engineers, the lesson is to avoid treating the drill file as an independent manufacturing document. Hole attributes, copper layers, and solder mask data should be reviewed together.

450 holes were marked as plated

Case 2: Plated Holes Connecting a Thermal Pad to Inner Copper

The second order involved five small holes positioned within a thermal pad. These holes connected the surface copper to an inner copper layer.

Unlike purely mechanical holes, these features had a functional role in the PCB's thermal and electrical design. Maintaining their plated status was therefore important.

The manufacturer confirmed that the holes should remain plated and added the required annular rings to support the connections.

This type of design is common in power electronics and thermal management applications. Plated thermal vias can transfer heat from surface-mounted components toward internal or opposite-side copper planes, helping distribute heat across the PCB structure.

For power supply PCB designs, engineers should consider thermal via placement, copper plane connectivity, finished hole size, and manufacturing tolerances during the layout stage.

A sufficient annular ring helps maintain the connection between the plated barrel and surrounding copper features, supporting the intended thermal and electrical path.

PCB thermal pad with five plated thermal vias connecting surface copper to an inner copper layer

Case 3: An Isolated Hole With Only a 2-Mil Annular Ring

The third example involved a small isolated hole with an annular ring of only 2 mils and no connection to any copper feature.

Although the original drill data identified the hole as plated, its actual design did not provide a meaningful electrical connection.

After reviewing the design intent, the customer confirmed that the hole should be non-plated.

This decision highlights the importance of distinguishing between electrical vias and mechanical holes. Plating should be selected based on the intended function and manufacturing requirements, not simply because a hole appears in a drill file with a particular attribute.

An isolated hole with inadequate copper support may also create unnecessary fabrication complexity if plating is not required.

However, changing a PTH to NPTH must never be done automatically. The designer must confirm the intended function, particularly when the hole is used for grounding, shielding, component mounting, or mechanical reinforcement.

PCB isolated drilled hole with a 2 mil annular ring and no electrical copper connection

 

PTH vs. NPTH: Manufacturing Comparison

Feature Plated Through-Hole (PTH) Non-Plated Through-Hole (NPTH)
Hole wall Conductive copper plating No conductive barrel plating
Electrical connectivity Can connect multiple copper layers Does not provide electrical layer connectivity
Typical applications Through-hole components, vias, grounding, thermal vias Mounting holes, positioning holes, mechanical clearance
Copper pad requirements Depends on the intended connection and fabricator's design rules Depends on mechanical design and surrounding copper clearance
Manufacturing process Drilling followed by hole-wall metallization and plating Drilling without conductive barrel plating
Main design concern Barrel connectivity, annular ring, plating requirements Hole tolerance, mechanical clearance, copper-to-hole spacing

 

PCB DFM Checklist Before Submitting Drill Files

Correct drill file preparation helps reduce CAM questions, avoid unnecessary engineering revisions, and prevent fabrication problems.

For multilayer PCB projects, these checks become especially important because plated holes may connect multiple internal copper layers. A mismatch between drill attributes and copper artwork can affect electrical connectivity and manufacturing feasibility.

1. Verify PTH and NPTH Attributes

Check that every drill tool and hole classification matches the intended manufacturing requirement. Avoid using the same drill designation for plated and non-plated holes without clear identification.

2. Check Copper Pads on Both Board Surfaces

For plated holes, verify that the top and bottom copper artwork supports the intended design. If a hole has a pad on only one side, confirm whether the missing pad is intentional and discuss the geometry with your manufacturer.

3. Confirm Minimum Annular Ring Requirements

Compare the designed annular ring against the fabricator's minimum requirements. Consider drilling tolerance, registration accuracy, finished hole diameter, and board construction.

4. Review Inner Layer Connectivity

For multilayer boards, check whether plated holes connect to the intended internal copper layers. Thermal vias, grounding vias, and signal vias may have different connection requirements.

5. Check Solder Mask Openings

Ensure that solder mask openings match the intended exposed copper areas. If the CAM team adds or modifies a pad, the corresponding solder mask data may also require revision.

6. Obtain Manufacturer Confirmation Before Fabrication

When drill attributes conflict with copper artwork, resolve the issue during engineering review. Do not assume the manufacturer will automatically determine whether the hole should be plated or non-plated. 

 

FAQ

Q1: Can a PCB plated through-hole have a pad on only one side?

A1: It depends on the hole's intended function and the fabricator's process requirements. Some designs may require additional copper geometry on the opposite surface to maintain reliable barrel-to-pad connectivity. The manufacturer should review the complete copper artwork before approving the design.

Q2: Does changing a PTH hole to NPTH reduce PCB manufacturing cost?

A2: Potentially, but the savings depend on the number of affected holes and the overall fabrication process. NPTH holes do not require conductive barrel plating, but changing the classification may also affect mechanical tolerances, copper clearances, and design functionality. Cost savings should be confirmed with the fabricator.

Q3: What happens if a plated PCB hole has an insufficient annular ring?

A3: Insufficient annular ring can increase the risk of copper breakout during drilling, potentially compromising the connection between the plated barrel and the surrounding copper pad. The actual risk depends on drilling registration tolerances and the remaining copper geometry.

Q4: Can a manufacturer automatically add missing annular rings during CAM processing?

A4: Manufacturers may identify missing pads and propose copper artwork modifications during CAM review. However, changes affecting electrical connectivity, thermal performance, or exposed copper areas should receive designer approval before fabrication.

Q5: Are thermal vias required to be plated?

A5: Thermal vias designed to transfer heat through the PCB generally use plated barrels to connect surface copper with internal or opposite-side copper. However, the appropriate structure depends on the thermal design, electrical requirements, and fabrication process.

AIVON

Leading PCB Manufacturer for PCB Prototype and Mass Production

Get instant quote

2026 AIVON.COM All Rights Reserved
Intellectual Property Rights | Terms of Service | Privacy Policy | Refund Policy