INDUSTRY COMPONENT

Die attach pad (DAP): the leadframe paddle under the die and how to solder it

Leadframe packages (QFN, DFN, ePad) · the paddle the chip is bonded to, exposed under the package

DAP stands for die attach pad, also called the die attach paddle, die pad or die flag. It is the central area of a leadframe on which the semiconductor die is bonded with die attach material, surrounded by the leads or lands that are wire-bonded to the die. In QFN and DFN packages the underside of the DAP is left exposed on the bottom of the package; Amkor describes this exposed die-attach paddle as an efficient heat path when soldered to the board, and as a stable ground through down bonds or a conductive die attach material. On the PCB it is matched by a thermal land, usually with thermal vias and a segmented paste print.

Die attach pads of copper leadframe packages, especially QFN/DFN (MLF) exposed-pad packages, and the matching PCB thermal land, vias and stencil. Die attach on ceramic or organic substrates and the die attach materials themselves are separate topics.

CNFX editorial research · Updated · 4 sources

01

DAP, die paddle, die flag: one part, three names

Renesas describes the construction: the die pad and the perimeter I/O pads of a QFN are made from one planar copper leadframe, encapsulated in plastic with the bottom of the die pad and the I/O pads left exposed, and both the I/O pads and the die pad should be soldered to the PCB. [3] ASE's QFN guide (hosted by Broadcom) calls the same area the die flag and lists electrical, thermal and mechanical connection to the motherboard through the exposed lands and die pad. [4]

Function of the exposed DAPWhat the maker says
Heat pathThe die-attach paddle exposed on the package bottom gives an efficient heat path when soldered directly to the PWB [1]
GroundStable ground through down bonds or through a conductive die attach material [1]
Mechanical anchorSoldering the exposed die pad anchors the package and improves temperature-cycling reliability of the I/O joints [3]
Thermal rating basisTI's published θJA assumes the pad is soldered to a four-layer JEDEC High-K board (JESD51-7) with vias [2]

Amkor's MicroLeadFrame range shows the scale: 1–13 mm bodies, 0.35–1.45 mm maximum height, up to 108 I/O in single-row and 180 in dual-row form, and split-pad designs in which the paddle is divided for more flexibility and I/O count. [1] A down bond is a wire from a die bond pad to the paddle itself, which is how the DAP becomes a ground connection; whether a given device's pad is ground or must be left floating is stated in that device's datasheet.

02

Worked example: 9 × 9 mm, 64-lead QFN

ASE's guide gives one complete package-to-board example. [4]

ItemPackagePCB
Terminal pitch0.5 mm0.5 mm [4]
Terminal width × length0.25 × 0.45 mm0.27 × 0.60 mm [4]
Die flag / thermal pad6.67 × 6.67 mm7 × 7 mm [4]
Thermal vias—4 × 4 array, 1.2 mm pitch, 0.3 mm diameter [4]

The same document gives the stack-up of its standard QFN: total thickness 0.8 or 1.0 mm, mould cap 0.54 or 0.7 mm, leadframe 0.2 mm. [4] The PCB land is slightly larger than the die flag here; ASE's rule is that the thermal land should at least match the exposed flag while keeping 0.15 mm clearance to the perimeter pads. [4]

03

PCB thermal land and vias under the DAP

Three application notes give closely matching numbers; differences are small and worth knowing when a datasheet gives no land pattern.

RuleTI SLUA271CRenesas TB389ASE (Broadcom-hosted)
Thermal land sizeEqual to the exposed pad [2]1:1 with the exposed die pad [3]At least the die flag size [4]
Clearance to I/O landsMinimum 0.2 mm for most designs [2]Use a solder-mask-defined land about 100 µm smaller per side if the gap is small [3]0.15 mm [4]
Via pitchAbout 1.0 mm [2]1.0–1.2 mm grid [3]1.0–1.2 mm [4]
Via diameter0.3 mm drill as a starting point [2]About 0.3–0.33 mm, barrel plated to about 1 oz copper [3]0.3–0.33 mm [4]
Via tentingMask 0.1 mm larger than the hole; tenting from the top gives fewer random voids [2]Mask about 100 µm larger than the via; top tenting gives smaller voids [3]—

TI adds that not every application needs vias, since the need depends on power dissipation, but the centre pad should always be soldered for mechanical strength and reliability. [2] Renesas notes that more vias improve heat flow with diminishing returns, so the practical count is set by land size and board design rules. [3]

04

Paste coverage and voiding on the exposed pad

A full-size aperture over the DAP prints too much solder. TI states that a 1:1 print over the exposed pad deposits enough metal to float the part and cause opens; its typical coverage is about 50–70% of the pad area. [2] Renesas recommends an array of smaller apertures giving 50–80% coverage. [3]

  • Void limit: TI says voiding in the thermal pad joint should stay below 50% in high-power parts, checked by X-ray; on a JEDEC High-K board 25% is the point of diminishing thermal returns, and TI prefers a 50% limit. [2]
  • Stencil thickness: production stencils in TI's note run from 0.100 to 0.150 mm; for 0.5 mm pitch packages it names 0.125 mm as the usual choice. [2]
  • Joint height: Renesas targets about 50–75 µm reflowed standoff on the perimeter lands. [3]
  • Small voids around vias are common and, per Renesas, have little effect on thermal or electrical performance. [3]

05

What to confirm for a part with an exposed DAP

The checklist follows from the land, via and paste rules above. [2] [3]

  • Exposed pad size and tolerance from the package outline drawing; split pad or single pad
  • Electrical role of the pad in the datasheet: ground, a specific pin, or no connection
  • Board used for the published θJA (for example JESD51-7 High-K) versus the real board
  • Thermal land size, clearance to I/O lands, mask-defined or not
  • Via count, pitch, drill, plating, and plugging or tenting method
  • Paste aperture pattern and coverage; void acceptance limit and X-ray inspection

06

Exposed-pad package or board enquiry

Paste it into your enquiry below or into an email to a maker, then replace every bracket.

Package: [type; body size; lead count; pitch]
Exposed pad: [size; single/split; electrical role]
Board: [layers; thermal land size; clearance]
Vias: [count; pitch; drill; plugged/tented]
Stencil: [thickness; paste coverage %]
Void limit: [% by X-ray]
Quantity: [ ]

See manufacturer records Send an enquiry through CNFX

Who makes exposed-pad leadframe packages

Exposed-pad QFN/MLF packages are assembled by outsourced assembly and test houses such as Amkor, whose MicroLeadFrame page lists the exposed-pad option, and by device makers for their own parts. [[amkor-mlf]]

Sourcing Die Attach Pad from China?
Tell us your specification and target quantity — we will match it against manufacturer records and come back with the factories that fit.
Request manufacturers We manufacture this

Explore company information and manufacturing capabilities, then discuss the scope of your project with a relevant supplier.

Related Components

Serial Interface
Serial interface for industrial data transmission between IoT gateways and legacy equipment using RS-232/422/485 protocols.
Marking Ink
Specialized ink for permanent identification on surface mount resistors during manufacturing.
Dielectric Layer
Insulating layer in surface mount capacitors that stores electrical energy through polarization.
Optical Window
Transparent optical component for light transmission in polycarbonate lens housings

Buyer questions

What does DAP mean in die attach?

Die attach pad (or paddle): the leadframe area to which the semiconductor die is bonded; in QFN packages its underside is exposed for soldering to the board. [1] [3]

Should the die attach pad be soldered to the PCB?

Yes. TI says the centre pad should always be soldered for mechanical strength and reliability, and Renesas notes it anchors the package and helps I/O joint life. [2] [3]

How big should the PCB pad be for a DAP?

About the same size as the exposed pad: TI and Renesas say equal or 1:1, with clearance to the I/O lands of 0.15–0.2 mm in the cited guides. [2] [3] [4]

What via pitch is used under an exposed pad?

Typically about 1.0–1.2 mm with 0.3–0.33 mm holes, per TI, Renesas and ASE. [2] [3] [4]

How much solder paste goes on the exposed pad?

Roughly 50–70% coverage per TI and 50–80% per Renesas, printed as several smaller apertures rather than one opening. [2] [3]

Sources and what still needs a direct check

Sources checked 2026-11-08T05:06:25+08:00. Package construction and DAP functions from Amkor's MicroLeadFrame page and Renesas TB389 (Rev. 8.03, 2024); board land, via and stencil rules from TI SLUA271C (2023), Renesas TB389 and ASE's QFN surface-mount requirements hosted by Broadcom.

  1. Amkor Technology — Micro_LeadFrame (QFN) package page ↗ Maker product page Return to text ↑
  2. Texas Instruments — SLUA271C, QFN and SON PCB Attachment (rev. December 2023) ↗ Maker application note Return to text ↑
  3. Renesas — TB389 Rev. 8.03, PCB Land Pattern Design and Surface Mount Guidelines for QFN Packages (2024) ↗ Maker technical brief Return to text ↑
  4. ASE Group — Surface Mount Requirements for QFN Package (hosted by Broadcom) ↗ Assembly house guideline Return to text ↑

Still to check yourself

  • Check the datasheet for the pad's electrical role.
  • Use split paste apertures, not one opening.
  • X-ray the thermal joint for voids.

Request Manufacturing Insight for Die Attach Pad

Thank you. Your request has been sent. We'll respond within 1–3 business days.
Sorry, we couldn't send your message. Please try again, or email us at [email protected].
XOR Gate
Get QuotesChat