PCB

BGA Land Pad Calculator

Calculate BGA land pad diameter, solder mask opening, and escape routing per IPC-7351B density levels.

Loading calculator...

Formula

D_{pad} = \text{round}_{0.05}(D_{ball} \times k)

D_pad— Pad diameter (mm)

D_ball— Ball diameter (mm)

k— Density factor (1.0/0.9/0.8)

How It Works

BGA land pad sizing follows IPC-7351B, which defines three density levels based on the ratio of pad diameter to ball diameter. Level L (most land) uses 100% of ball diameter — maximum solder joint volume and reliability. Level N (nominal) uses 90% — balanced routing and reliability. Level M (least land) uses 80% — maximum routing density at the cost of thinner solder joints.

The choice between NSMD (non-solder-mask-defined) and SMD (solder-mask-defined) pads affects self-alignment during reflow. NSMD pads have the solder mask pulled back from the copper edge, so the copper pad defines the joint geometry. SMD pads have mask overlapping the copper, so the mask opening defines the joint. NSMD is strongly preferred for BGA because the exposed copper dome promotes solder self-centring during reflow, correcting minor placement errors.

Escape routing determines how signals exit the BGA array. The channel width (pitch minus pad diameter) dictates how many traces can pass between adjacent pads. At 1.0 mm pitch with nominal density, channel width is typically 0.45 mm — enough for two traces with standard clearance rules. Fine-pitch BGAs (≤ 0.5 mm) often require via-in-pad to escape inner rows.

Worked Example

Given: Ball pitch = 1.0 mm, ball diameter = 0.6 mm, density level = Nominal (N), NSMD pads, no via-in-pad Step 1: Pad diameter

Nominal density factor = 0.9

D_{pad} = \text{round}_{0.05}(0.6 \times 0.9) = \text{round}_{0.05}(0.54) = 0.55

mm Step 2: Solder mask opening (NSMD)

D_{mask} = D_{pad} + 0.1 = 0.55 + 0.1 = 0.65

mm Step 3: Channel width

W_{channel} = P - D_{pad} = 1.0 - 0.55 = 0.45

mm Step 4: Escape routes

One trace needs ≈ 0.2 mm (trace + 2× clearance). Two traces need ≈ 0.38 mm.

0.45 mm ≥ 0.38 mm → 2 traces per channel

Step 5: Max trace width

W_{trace} = \frac{W_{channel} - 2 \times 0.05 \times 2}{2} = \frac{0.45 - 0.2}{2} = 0.125

mm Step 6: Stencil aperture

Pitch ≥ 0.5 mm → no reduction: $D_{stencil} = 0.55$ mm

Result: 0.55 mm pad, 0.65 mm mask opening, 2 escape routes per channel at 0.125 mm trace width.

Practical Tips

✓Start with nominal density (N) — only go to most (L) if solder joint reliability simulations or thermal cycling requirements demand it
✓For 0.8 mm pitch and below, plan via-in-pad for inner BGA rows from the start — dog-bone fanout won't fit
✓Verify your fab can hold 0.075 mm mask-to-pad registration before specifying NSMD with tight clearance
✓Use thermal relief on ground plane BGA pads to prevent tombstoning from uneven heat distribution
✓For prototype runs, use Level L (most land) to maximise process window — optimise to N or M only after first article passes

Common Mistakes

✗Using SMD pads for BGA — solder mask overlap prevents self-alignment during reflow, leading to solder bridges
✗Not rounding pad diameter to 0.05 mm grid — fabricators snap to grid anyway, potentially changing your intended design
✗Ignoring stencil aperture reduction for fine-pitch — below 0.5 mm pitch, full-size apertures deposit too much paste causing bridges
✗Assuming via-in-pad is free — it requires filled and planarised vias, adding $0.50–2.00 per board to fab cost

Frequently Asked Questions

What pad size should I use for a 0.8 mm pitch BGA?

With typical 0.45 mm ball diameter at nominal density: 0.45 × 0.9 = 0.405, rounded to 0.40 mm. This gives 0.40 mm channel — enough for one trace (0.1 mm trace + 0.075 mm clearance each side). Inner rows will need via-in-pad.

Why is NSMD preferred over SMD for BGA?

NSMD exposes the full copper pad dome, allowing solder surface tension to self-centre the ball during reflow. This corrects up to 50% of the pad diameter in placement error. SMD constrains the solder within the mask opening, preventing this self-alignment.

How do I size via-in-pad for BGA?

Maximum via drill = pad diameter − 2 × annular ring minimum. For a 0.55 mm pad with 0.1 mm annular ring: max drill = 0.35 mm. The via must be filled (copper or epoxy) and planarised to be coplanar with the pad surface.

What is the minimum BGA pitch that allows dog-bone fanout?

With standard design rules (0.1 mm trace/space), dog-bone fanout works reliably down to 0.8 mm pitch. At 0.65 mm, only outer two rows can escape with dog-bones. At 0.5 mm and below, via-in-pad is required for all but the outermost row.

Does the IPC standard specify exact pad diameters?

No — IPC-7351B provides the methodology (percentage of ball diameter per density level) but not absolute numbers, since ball diameters vary by package. The manufacturer's datasheet specifies ball diameter and pitch; apply the density factor to calculate pad size.

Shop Components

As an Amazon Associate we earn from qualifying purchases.

PCB Manufacturing (JLCPCB)

Affordable PCB fabrication with controlled impedance options

JLCPCB →

FR4 Copper Clad Laminate

FR4 laminate sheets for custom PCB prototyping

Amazon →

Thermal Paste

Thermal interface material for component heat management

Amazon →

Related Calculators

PCB

Annular Ring

Calculate minimum pad diameter and annular ring per IPC-6012 for through-hole vias and component pads.

PCB

Via Calculator

Calculate PCB via impedance, capacitance, inductance, and current capacity. Get aspect ratio and DFM warnings for through-hole and blind vias. Free, instant results.

PCB

Conductor Spacing

Determine minimum electrical clearance between conductors per IPC-2221B Table 6.1 based on voltage and conductor condition.

PCB

Controlled Z

Calculate characteristic impedance for surface microstrip, embedded microstrip, and stripline PCB traces. Get Z0, effective Er, and target trace width. Free, instant results.