Skip to main content
PCB DesignPCB Manufacturing

How to Design a Castellated Circuit Board in Altium Designer and Allegro

Castellation is a technique used by PCB manufacturers to achieve efficient board-to-board connections. Using this approach, you can integrate multiple […]


Author headshot: Christina Sundari

By Christina Sundari

November 16, 2022  |  0 Comments

castellated-hole-deign.jpg

Castellation is a technique used by PCB manufacturers to achieve efficient board-to-board connections. Using this approach, you can integrate multiple castellated circuit boards into a single assembly.

For example, individual modules, like WiFi and Bluetooth, can be mounted together in any given system. The boards are fabricated with semi-plated holes on their edges known as castellated pins. These pins configure the electrical connection of a sub-module to the main board. This can significantly reduce the overall size of the board by eliminating the usage of pin connectors.

How are castellated pins created on a PCB?

castellation-holes-pcb.jpg
Castellation holes for mounting

Castellated pins are manufactured by drilling plated-through holes on the edges of the board. After the drilling process, fabricators need to cut the holes into halves along the edge and attach a pad to it. These plated semi-holes can be used as soldering pads to attach the sub-assembly circuits to the main board. The process of creating these holes is also called edge plating or side plating.

Adhere to the following guidelines to establish a reliable board-to-board connection:

castellation-pins-on-the-board-periphery.jpg
Castellated pins on the edge of the board
  • Ensure no gaps between the two boards. Even a small gap will adversely affect the soldering process.
  • When stacking boards, ensure that the thickness of the upper PCB is one-third the size of the lower one. This will aid in appropriate alignment and assembly.
  • Castellated pins must match the SMD pads it is supporting.

Why should you choose a castellated holes PCB

Opting for a castellated circuit board can help you improve the efficiency of your design. A few of the advantages are listed below.

Quick and affordable assembly: Plated half-hole on the edges eliminate the use of board-to-board connectors. This fastens the board assembly process and reduces the overall cost.

Efficient thermal management: Complex systems such as aerospace and telecommunication devices feature high-temperature components, which increase the overall temperature of the board. Castellated circuit boards offer better heat dissipation when compared to other PCBs.

Improved signal integrity: The metallization of the edges prevents EMI on the inner layers and reduces the risk of electrostatic damage.

Acts as breakout boards: Castellated PCBs can be used as breakout boards for a specific area of a larger PCB. This facilitates the prototyping of integrated circuits and experimentation.

 

Signal Integrity eBook - Cover Image

Signal Integrity eBook

3 Chapters - 12 Pages - 20 Minute Read
What's Inside:
  • Impedance discontinuities
  • Crosstalk
  • Reflections, ringing, overshoot and undershoot
  • Via stubs

 

Design guidelines for castellated circuit boards

design-guidelines-of-castellated-circuit-boards.jpg
Design attributes of a castellated hole
  • Place the exact center of each castellated hole on the edge of your board. These holes must be plated through. Include them in the drill files.
  • Always place the castellated holes on the top or bottom edges.
  • Use pads for copper layers.
  • Make sure you provide an accurate solder mask opening. This will prevent your board from corrosion and physical damage.
  • Maintain the finished hole size [(a) shown in the image above] between 0.5 mm and 0.8 mm.
  • Design the size of the castellated pads as per below:
    • Diameter of the pad = Finished hole size + 0.7 mm
      For example, if the finished hole size is 0.8 mm, then the pad diameter will be 1.5 mm.
    • Maintain sufficient width for the annular ring, or else the plating will break out.
    • The minimum diameter for drilling half-holes is 0.5 mm.
    • You can have a minimum solder mask clearance (c) of 0.1 mm.
    • Keep the solder mask bridge between 0.1 mm – 0.15 mm.
    • Keep the pads at a distance of 2.54 mm (b) from each other.
    • Ensure the annular ring width is 0.3 mm per side. This is calculated as follows:
      • Annular width = (Diameter of the pad-diameter of the finished hole) /2
minimum-annular-width.jpg
Minimum annular width for a castellated hole

Edge plating: A technique to metalize castellated holes

Edge plating is a method used for the metallization of castellated pins. Here, copper will be deposited along the semi-hole walls. Follow these guidelines to ensure manufacturability.

edge-plating.jpg
Typical edge plating specifications
  • Overlap from the board edge should be at least 0.5 mm.
  • A minimum of 0.3 mm of connected copper must be defined on the connected layer.
  • The spacing between the hole wall and the copper feature on a non-connected outer layer should be a minimum of 0.8 mm.

Why ENIG is preferred for edge plating

The surface finish options for castellated holes include ENIG, ENEPIG, HASL, and others. ENIG coating is preferred as it provides a smooth finish and eliminates the formation of lumps during the coating process.

better-dfm-tool.jpg

 

Tolerances of castellation holes

IPC – 6012 defines the tolerances for castellation holes. The values are given in the table below.

Parameters Tolerances
Size of the pad

± 20 %
Castellated hole size± 3 mils
Board thickness10% or ± 3 mils whichever is larger (thickness should be greater than or equal to 31 mils)
Drill diameter± 3 mils
Drill to copperMinimum 8 mils
Hole to hole6 mils

Creating a castellated board using Altium Designer

Let us see the steps involved in designing a castellated board with a finished hole of 0.7 mm, a pad-to-pad distance of 2.54 mm, and a pad diameter of 1.5 mm.

1. Click on Pad from the toolbar and place a dummy pad with a diameter of 1.5 mm.

placement-of-dummy-pad-on-castellated-pcb.jpg
Pad placement on castellated circuit board

2. Select the dummy pad and set the following dimensions:

  • Hole size = 0.8 mm
  • Tolerance =0.076 mm
  • X-size = 1.5 mm
  • Y-size = 1.5 mm
setting-the-pad-dimensions.jpg
Setting the pad dimensions in castellated circuit board

3. Now click on Line, and place the trace with a width of 5 mils.

track-placement.jpg
Place the track around the pad

4. Select Arc(Edge) under the option Place and have the arc on the circumference of the pad.

placement-of-arc-on-the-pad-edge.jpg
Arc placement on the circumference of the pad

5. Now select the pin structure, go to the Tools tab and choose Create Region from Selected Primitives under Convert.

 create-castellated-hole-with-set-primitives.jpg
Create the castellated hole with the set primitives

6. To arrange the board layers, double-click on the selected region, arrange them in the following folder:

  • Top layer
  • Bottom layer
  • Top paste
  • Bottom paste
  • Top solder
  • Bottom solder
layer-arrangement-in-altium-designer.jpg
Layer arrangement in Altium Designer

6. After the layer arrangement, click on the Setup Paste Array. This pops up a window asking you to enter the number of pads. You can define it in the item count section. Enter the pad-to-pad spacing in the linear array section as 2.54 mm.

set-up-paste-array-in-castellated-boards.jpg
Set up paste array in castellated boards

7. The castellated holes are now created on the edge of the board. To align them, go to Edit, select Set Reference and choose Center.

castellated-board-with-pad-diameter-1.5mm.jpg
Castellated board with pad diameter of 1.5 mm

8. Draw the assembly outline and set the line constraint (Line width= 0.15 mm).

assembly-outline-line-constraints.jpg
Line constraints for assembly outline

7. To see the 3D view of the board, go to Tool, and select Manage 3D bodies for Current Component. 

three-dimensional-view-selection.jpg
Choosing the 3D view

You can now examine all the layers and sides of the board in 3D.

3-d-view-of-castellated-board.jpg
3D view of a castellated board

Designing a castellated board using Allegro

1. First you need to select Package Geometry under the active class and subclass section. Now, to draw the outer line of the pin, go to Add, and select Line.

dummy-pad-drawing-using-line.jpg
Creating the dummy pad

2. After creating the outline, go to Add, and select 3pt Arc, to draw the arc. According to the workspace scale (0.25 mm per unit), the diameter of this dummy pad is equal to 1.5 mm.

placement-of-arc-in-allegro.jpg
Placement of arc in Allegro

3. Now, go to Shape and select Compose Shape and click on the dummy pad to save the pad outline.

shape-compose.jpg
Creating a shape to save the pad

4. Next, go to File, Export, choose Sub-Drawing, and save the file with a designated name. Here the file is saved as shp90*32 and the type as a clipboard file.

export-sub-drawing.jpg
Export the sub drawing

5. Go to File, select Import, and choose the saved sub-drawing.

import-saved-drawing-to-workspace.jpg
Import the saved drawing to the workspace

6. Now, you need to open the template that is saved in step 4. Go to file, open, and select the saved clipboard file(shp90*32).  Next, click on the pad symbol on the toolbar to create a dummy pad.

dummy-pad-creation-in-allegro.jpg
Dummy pad creation in Allegro

7. Go to Tools, click on Padstack and choose Modify Design padstack and place the pad.

defining-padstack-of-castellated-circuit-board-in-allegro.jpg
Defining the padstack in Allegro

8. Select Grids from the Setup tab to modify the parameters.

grid-definition.jpg
Defining the grid for pad spacing

pcb-conductor-spacing-and-voltage-calculator.jpg

 

9. Click on Copy to duplicate the created pads.

copy-pad-for-the-board.jpg
Copy the designed pad

10. Now, click on Measure to check the pad dimensions.

measuring-pad-dimensions-in-allegro.jpg
Measuring pad dimensions in Allegro

11. To modify the pad dimensions, right-click on the pad, select Snap pick to, and click on Pad edge. Now, select Setup and choose grid to define the spacing between the pads.

measure-pad-dimensions.jpg
Grid measure for pad

 

pad-spacing.jpg
Spacing of the pads

12. Now, you need to draw the assembly outline. Go to Package Geometry and select Assembly_top. To verify the pad spacing, click on measure.

verifying-pad-to-pad-distance-in-allegro.jpg
Verifying pad-to-pad distance in Allegro

13. Now add a silkscreen to the board with a line width of 0.15 mm. This option is available in Package Geometry.

silkscreen-for-the-board.jpg
Silkscreen placement for the board

14. Designate the 1st pin using the pin indicator. Place it at a distance of 0.05 mm from the board edge.

first-pin-indicator.jpg
Pin 1 indicator on the board

15. To define the board size, go to Edit, click on Package Height Max and set it to 2.5 mm. This depends on the your specifications.

package-height-of-the-board.jpg
Specifying the package height

16. Click on 3D from the toolbar to observe the model in 3-dimensional.

3d-view-in-allegro.jpg
3D view in Allegro
three-dimensional-view-of-castellated-board.jpg
Three-dimensional view of the board

17. A castellated board with the given dimensions is created now.

castellated-board-for-the-given-specifications.jpg
Castellated board with the required specifications

Castellation is a convenient and efficient way to establish board-to-board connections. It allows you to solder a sub-circuit directly to the main module eliminating the need for external connector pins. This significantly reduces the overall cost of the board and also speeds up the assembly process. We hope this tutorial was helpful in designing castellated boards using Altium Designer and Allegro. If you need any assistance in designing castellated PCBs, let us know in the comments section. We will be happy to help you.

 

Design for Manufacturing Handbook - Cover Image

Design for Manufacturing Handbook

10 Chapters - 40 Pages - 45 Minute Read
What's Inside:
  • Annular rings: avoid drill breakouts
  • Vias: optimize your design
  • Trace width and space: follow the best practices
  • Solder mask and silkscreen: get the must-knows

 

What is 1900 + 86?

Subscribe
Notify of
guest
0 Comments
Inline Feedbacks
View all comments
Share this article
Zero Defects guaranteed on all PCB fabrication

Reduce Re-Spins with our Zero Defect Guarantee.

Our platform sources the whole package, creating a thread from design to delivery. Fabricating PCBs. Procuring parts. Assembling your boards.

Once you upload your BOM, Our best-in-class software automatically checks for errors and cleans your file for you. After you place an order, your dedicated CAM engineer will run a full DFM and DFA check to ensure your prototype achieves Zero Defect every time—all at no additional cost to you.

Get to market faster and spend less time troubleshooting.


Start Quote

Talk to a Sierra Circuits PCB Expert today

24 hours a day, 7 days a week.

Call us: +1 (800) 763-7503
Email us: through our Customer Care form