Component placement is not purely an electrical decision: it also fixes the order in which a PCBA is built. This article explains the basic layout requirements that keep assembly flow logical, and shows how placement choices translate into processing efficiency and first-pass yield.
Highlights:
- Placement must preserve a reasonable, buildable PCBA process sequence.
- The selected process flow should deliver the highest available processing efficiency.
- Six mainstream PCBA process flows form the reference set for layout decisions.
Basic Layout Requirements
Reasonable PCBA Processing Sequence
The component layout of the finished board must guarantee a reasonable manufacturing sequence, so that both processing efficiency and first-pass yield of the assembled board can be improved. The process flow selected during PCB layout should achieve the highest possible processing efficiency. The six mainstream PCBA process flows in common use are summarized in Table 2.
Silkscreen Indication of Board Entry Direction for Wave Soldering
For boards processed by wave soldering, the board entry direction should be marked on the PCB by silkscreen, and the selected direction should be reasonable. If the PCB can be fed from two directions, a double-arrow entry mark should be used. For reflow soldering, a fixture or carrier can be considered to define the reflow direction.
Process Flow Options for Mixed-Technology PCB Assembly
Table 2 lists six common assembly routes and relates each route to its process flow, efficiency, heat-cycle count, and applicable component types. The table is an application guide for selecting a route that matches the board's component mix.
Table 2. Common PCB assembly process flows.
| No. | Assembly method | Process flow | Characteristics | Applicable scope |
|---|---|---|---|---|
| 1 | Single-sided through-hole insertion | Lead forming → insertion → wave soldering | High efficiency; PCB assembly is heated once | THD |
| 2 | Single-sided surface mount | Solder paste printing → pick-and-place → reflow soldering | High efficiency; PCB assembly is heated once | SMD |
| 3 | Single-sided mixed assembly | Solder paste printing → pick-and-place → reflow soldering → THD wave soldering | Relatively high efficiency; PCB assembly is heated twice | SMD, THD |
| 4 | Double-sided mixed assembly | Adhesive printing → pick-and-place → curing → board flip → THD insertion → wave soldering → board flip → hand soldering | High efficiency; PCB assembly is heated twice | SMD, THD |
| 5 | Double-sided SMT and through-hole insertion | Solder paste printing → pick-and-place → reflow soldering → board flip → solder paste printing → pick-and-place → reflow soldering → hand soldering | High efficiency; PCB assembly is heated twice | SMD, THD |
| 6 | Conventional wave-soldered double-sided mixed assembly | Solder paste printing → pick-and-place → reflow soldering → board flip → adhesive printing → pick-and-place → curing → board flip → THD insertion → wave soldering → board flip → hand soldering | Lower efficiency; PCB assembly is heated three times | SMD, THD |
The table makes the process-selection tradeoff explicit. A THD-only board can use single-sided insertion with one heat cycle. An SMD-only board can use single-sided surface mount with one reflow. When both THD and SMD are present, the process must combine reflow and wave soldering. Double-sided processing adds board flips, adhesive printing, curing, and hand soldering, and the heat-cycle count rises from one to two or three. The applicable scope column links each route to THD, SMD, or both. The remaining requirements in this part address the layout constraints that arise when these mixed-technology boards are reflowed twice, wave soldered, or fitted with board-edge connectors.
5.4.3 BOTTOM-Side Component Weight Limits for Double-Sided Reflow
For a PCB that must pass through reflow soldering on both sides, the BOTTOM side should not carry large-volume or overly heavy SMD components. The component weight limits for the first reflow soldering are defined using A, where A is the component weight divided by the lead-to-pad contact area:
- Chip components: A ≤ 0.075 g/mm2
- Gull-wing lead components: A ≤ 0.300 g/mm2
- J-lead components: A ≤ 0.200 g/mm2
- Area array components: A ≤ 0.100 g/mm2
The limits are normalized by the lead-to-pad contact area, so the allowable component weight depends on the attachment area rather than on package size alone. Chip components have the most restrictive limit, while gull-wing lead components allow the highest weight per unit contact area. If an overweight component must be placed on the BOTTOM side, the feasibility of the assembly should be verified by test.
5.4.4 Safe Spacing to Avoid Shadowing in Wave Soldering
For a board that will be wave soldered, components on the back side must not create a shadow effect. The following SMT component spacing requirements take the wave soldering process into account so that back-side components do not interfere with solder access.
Spacing Between Components of the Same Type
For same-type components, see following figures. The spacing relationship uses two dimensions: L, the pad spacing, and B, the component body spacing. Table 3 gives both minimum and recommended values in mm/mil.
Table 3. Relationship between package size and spacing for same-type components.
| Package | Pad spacing L minimum (mm/mil) | Pad spacing L recommended (mm/mil) | Body spacing B minimum (mm/mil) | Body spacing B recommended (mm/mil) |
|---|---|---|---|---|
| 0603 | 0.76/30 | 1.27/50 | 0.76/30 | 1.27/50 |
| 0805 | 0.89/35 | 1.27/50 | 0.89/35 | 1.27/50 |
| 1206 | 1.02/40 | 1.27/50 | 1.02/40 | 1.27/50 |
| ≥1206 | 1.02/40 | 1.27/50 | 1.02/40 | 1.27/50 |
| SOT package | 1.02/40 | 1.27/50 | 1.02/40 | 1.27/50 |
| Tantalum capacitor 3216/3528 | 1.02/40 | 1.27/50 | 1.02/40 | 1.27/50 |
| Tantalum capacitor 6032/7343 | 1.27/50 | 1.52/60 | 2.03/80 | 2.54/100 |
| SOP | 1.27/50 | 1.52/60 | N/A | N/A |
Table 3 shows that 0603 components can use 0.76/30 minimum pad and body spacing, 0805 components use 0.89/35, and 1206, ≥1206, SOT, and tantalum 3216/3528 components use 1.02/40. The recommended value for these cases is 1.27/50. For tantalum 6032/7343, pad spacing increases to a 1.27/50 minimum and 1.52/60 recommended, while body spacing increases to a 2.03/80 minimum and 2.54/100 recommended. For SOP, pad spacing is specified at a 1.27/50 minimum and 1.52/60 recommended, but body spacing is not specified. The table therefore shows that body spacing becomes more demanding for larger tantalum capacitors, while pad spacing remains the controlling dimension for the smaller packages.
Spacing Between Components of Different Types
Table 4 gives the minimum spacing matrix for different package types.
Table 4. Minimum spacing between different package types (mm).
| Package size | 0603 | 0805 | 1206 | ≥1206 | SOT package | Tantalum capacitor 3216/3528 | Tantalum capacitor 6032/7343 | SOIC | Through-hole |
|---|---|---|---|---|---|---|---|---|---|
| 0603 | N/A | 1.27 | 1.27 | 1.27 | 1.52 | 1.52 | 2.54 | 2.54 | 1.27 |
| 0805 | 1.27 | N/A | 1.27 | 1.27 | 1.52 | 1.52 | 2.54 | 2.54 | 1.27 |
| 1206 | 1.27 | 1.27 | N/A | 1.27 | 1.52 | 1.52 | 2.54 | 2.54 | 1.27 |
| ≥1206 | 1.27 | 1.27 | 1.27 | N/A | 1.52 | 1.52 | 2.54 | 2.54 | 1.27 |
| SOT package | 1.52 | 1.52 | 1.52 | 1.52 | N/A | 1.52 | 2.54 | 2.54 | 1.27 |
| Tantalum capacitor 3216/3528 | 1.52 | 1.52 | 1.52 | 1.52 | 1.52 | N/A | 2.54 | 2.54 | 1.27 |
| Tantalum capacitor 6032/7343 | 2.54 | 2.54 | 2.54 | 2.54 | 2.54 | 2.54 | N/A | 2.54 | 1.27 |
| SOIC | 2.54 | 2.54 | 2.54 | 2.54 | 2.54 | 2.54 | 2.54 | N/A | 1.27 |
| Through-hole | 1.27 | 1.27 | 1.27 | 1.27 | 1.27 | 1.27 | 1.27 | 1.27 | N/A |
Table 4 is a minimum-spacing matrix for different package types. It covers 0603, 0805, 1206, ≥1206, SOT package, tantalum capacitor 3216/3528, tantalum capacitor 6032/7343, SOIC, and through-hole. The values are minimum only; no recommended column is provided. For example, 0603 to 0805 is 1.27, 0603 to SOT is 1.52, 0603 to tantalum 6032/7343 is 2.54, and through-hole to any package is 1.27. The largest minimum spacing in the matrix is 2.54, which appears for tantalum 6032/7343 and SOIC combinations. Where both same-type and different-type constraints
Stand-off Requirements for SMT Components Passing Through Wave Soldering
For an SMT component to be placed on the B side and pass through wave soldering, its stand-off must be less than 0.15mm. If the stand-off is greater, the component should not be assigned to B-side wave soldering. When the stand-off is between 0.15mm and 0.2mm, copper foil can be placed under the component body to reduce the distance between the body bottom and the PCB surface.
Minimum Safe Spacing for Backside Test Points During Wave Soldering
To prevent solder bridging at backside test points during wave soldering, the edge-to-edge distance between test points must be greater than 1.0mm. This spacing reduces the risk of a solder bridge forming between adjacent points and helps preserve electrical isolation after soldering.
Through-Hole Component Pad Spacing for Wave Soldering
For PTH components that pass through wave soldering, the edge-to-edge pad spacing should be greater than 1.0mm, including the pads for the component's own pins. A preferred pin pitch is 2.0mm, with a pad edge spacing of at least 1.0mm. Provided that component bodies do not interfere, the pad edge spacing between adjacent components should meet the requirement.
When a through-hole component has many pins in each row and the pad row direction is parallel to the board-entry direction, an adjacent pad edge spacing of 0.6mm to 1.0mm is a special case. In this range, oval pads or solder-thieving pads are recommended.
BGA Keepout: No Components Within 3mm
To maintain repairability, a BGA requires a 3mm keepout area around the device, with 5mm preferred. In general, BGAs should not be placed on the backside. For a board that passes through reflow twice, this means the side reflowed first. If a BGA is placed on the backside, no components may be placed on the front side within the projection of its 5mm keepout area.
5.4.11 Minimum Spacing Between SMT Components
Machine placement imposes minimum spacing between components. For components of the same type, the spacing should be at least 0.3mm. For different types, the spacing should be at least 0.13*h+0.3mm, where h is the maximum height difference between neighboring components. For components that can only be placed by hand, the spacing should be at least 1.5mm.
5.4.12 Component Outer Edge to Conveyor-Contact Board Edges: At Least 5mm
The component outer edge should be at least 5mm from the two board edges that contact the conveyor rail. This prevents the rail clamps from touching components during wave soldering or reflow soldering. If the clearance cannot be met, add a process edge to the PCB; the component-to-V-CUT distance should then be at least 1mm.
5.4.13 Clearance Around Adjustable and Pluggable Components
Adjustable and pluggable components require sufficient space for adjustment, debugging, and maintenance. The layout orientation and adjustment space for adjustable components should be determined from the PCBA mounting layout and the adjustment method. Clearance around a pluggable component should be set according to the height of adjacent components.
5.4.14 Base Requirements for Through-Hole Magnetic Components
All through-hole magnetic components must have a sturdy base. Through-hole inductors without a base are not permitted.
5.4.15 Pin Symmetry on Polarized Transformers
Where possible, the pins of a polarized transformer should not be designed in a symmetrical arrangement, so the polarized orientation remains unambiguous during assembly.
5.4.16 Keepout Around Mounting Holes
Within a mounting-hole keepout, there should be no components and no routing, except for the traces and copper of the mounting hole itself.
5.4.17 Safety Spacing for Metal-Case Components and Metal Parts
Metal-case components and metal parts must maintain spatial separation from other components that satisfies safety requirements.
5.4.18 Layout Requirements for Through-Hole Reflow Components
- For PCBs with a non-conveyor edge dimension greater than 300mm, heavy components should not be placed in the middle of the PCB where possible. This reduces PCB deformation caused by through-hole component weight during soldering and limits disturbance to components already placed on the board during insertion.
- To make insertion easier, components should be placed near the insertion operator side.
- Long components, such as memory-module sockets, should be oriented with their length direction parallel to the conveyor direction.
- For a through-hole reflow component, the distance from the pad edge to the silkscreen of a QFP, SOP, or connector with a pitch of 0.65mm or less, and to the silkscreen of all BGAs, should be greater than 10mm. The distance to other SMT components should be greater than 2mm.
- The body-to-body distance between through-hole reflow components should be greater than 10mm. Pin soldering supported by a fixture is not subject to this requirement.
- The distance from the pad edge of a through-hole reflow component to the conveyor edge should be greater than 10mm; the distance to the non-conveyor edge should be greater than 5mm.
Keepout Requirements for Through-Hole Reflow Components
- Sufficient space must be left around through-hole reflow component pads for solder paste deposition. For a European connector, the direction toward the board interior must have a 10.5mm keepout with no components; within this keepout area there must be no components and no vias.
- Vias that must be placed within the keepout area should be solder-mask plugged.
5.4.20 Board-Level Assembly Interference Must Be Considered in Component Layout
Component layout must consider assembly interference between board and board, and between board and structural parts. This is especially important for tall components and for boards assembled in three dimensions.
5.4.21 Distance Between Components and the Chassis
Components should not be placed too close to the chassis wall, because this can damage them when the PCB is installed. Pay particular attention to edge-mounted components that may move slightly under shock and vibration or that lack a robust outer shape, such as vertically mounted resistors and base-less inductors or transformers. If the clearance cannot be met, add fixing measures to satisfy safety and vibration requirements.
5.4.22 Place Wave-Soldered Components Near the PCB Edge
Components passing through wave soldering should be placed as close as possible to the PCB edge to simplify hole masking. If they are at the edge and the soldering fixture is well designed, hole masking may not be needed.
5.4.23 Design for Wave Soldering and Minimize Hand Soldering
The design should allow components to pass through wave soldering wherever possible. Component selection should minimize parts that cannot pass through wave soldering, and the number of components on the soldering side should be kept low to reduce hand soldering.
5.4.24 Routing of Bare Jumpers
Bare jumpers must not be routed flat against the board across traces or copper, because they can short to the copper. Solder mask is not effective insulation for this purpose.
5.4.25 Inspection and Maintenance After Soldering
During layout, consider that all components must be easy to inspect and maintain after soldering.
5.4.26 Cable Solder Ends Near the PCB Edge
Cable solder ends should be as close as possible to the PCB edge for insertion and soldering. Otherwise, other components may obstruct cable insertion and soldering, or the cable may knock them out of position.
5.4.27 Devices with Multiple Pins in a Straight Line
Devices with multiple pins in a straight line, such as connectors, DIP packages, and TO-220 packages, should have their axis parallel to the wave-soldering direction.
5.4.28 Light Components Such as Diodes and 1/4W Resistors
Light components such as diodes and 1/4W resistors should have their axis perpendicular to the wave-soldering direction. This prevents floating during wave soldering when one end solidifies before the other.
5.4.29 Space Between Cables and Surrounding Components
Leave sufficient space between a cable and surrounding components. Otherwise, the bent portion of the cable can press on and damage nearby components and their solder joints.
Related Reading:
PCB Material and Thermal Design Requirements for Reliable Assembly
PCB Component Library and Footprint Selection Requirements Guide
PCB Routing and Reference Point Design Requirements
PCB Testability Requirements for Reliable ICT and Functional Test
Electrical Clearance, Creepage Distance, and Insulation Levels
