This article is intended to assist engineers who are new to LED prototyping and wish to design and obtain a small number of MCPCBs for characterization and prototyping activities. We will walk through designing the starboard shown below.
Designing and sourcing your own MCPCBs gives you complete control over your LED application. This process comprises several interrelated parts, each with many choices:
• PCB layout software
• Cad layout software
• Sourcing and populating the MCPCBs
Sourcing MCPCBs - There are numerous MCPCB suppliers available, with a Google search for "mcpcb suppliers" yielding 411,111 results. To streamline your search, look for the following criteria:
- Quick Turn Service - typically, a lead time of a few weeks for a small number of panels.
- Information about available MCPCB types - PCB fabs have a material qualification process, and each supplier will have a list of qualified MCPCB options. Look for details relevant to your application, with the most important differentiator being the type of dielectric used to isolate the copper foil layer from the (typically) aluminum base layer. Most PCB suppliers have comparable design capabilities (copper foil weight, surface finish options, hole size specifications, etc.). If you require a specific MCPCB type (usually dielectric type), requesting a list of qualified fabricators from the manufacturer of the key element is a good strategy.
- MCPCP variants – the most common MCPCB type is a single layer aluminum base design. There are other options: single layer with copper base, various types of multilayer designs, and pedestal designs where there is a direct contact to the LED thermal pad to achieve the highest heat extraction.
- Certifications - ensure the supplier has the necessary certifications for your application.
- File requirements - the most common set of files used by PCB suppliers is Gerber RS-274-X with a drill file. Some PCB suppliers can accommodate other file formats and/or provide conversion services for CAD files such as the DXF format.
- The option to populate PCBs with components - many suppliers have this capability.
- Luminus maintains a list of PCB suppliers in our Ecosystem at: https://www.luminus.com/resource/ecosystem/printed-circuit-boards
Design Software – Designing an MCPCB involves the use of PCB layout software, 2D Cad software, and 3D Cad software. There are many options with different price points and capabilities. For PCB design, choose a set of software that can accommodate file imports and exports between all of these software packages. For PCB software, the fabrication file is generally Gerber RS-274-X. Import and export files to/from different Cad software are generally STEP and DXF files.
Design Walkthrough
We will walk through the steps to design the starboard shown above for a Luminus SST-10 LED package with a thermal pad. We are using DipTrace for the PCB layout software and DraftSight for 2D design software. Other software packages may have different menu structures but generally work the same way.
First, open the PCB layout app. Since this example only has one LED, we will not use a schematic. Set the units to mm and the snap to 0.1 mm.
Click “Filter Off” to bring up the component placement menu.
Luminus has footprints at SnapEDA so we will use that option. Click “Search at SnapEDA” and type SST-10 in the search field. You need to register for a free account at SnapEDA to download files.
Download and save the 3D model. This is needed later.
Click “Place Component” and place the component anywhere on the screen. Use <esc> to exit the placement mode.
Move the center of the footprint to the origin of the layout. In the Design Manager pane, right click the part (D1) and pick “Properties”. Change the position to X: 0, Y: 0 in the menu.
The layers defined in the footprint can be viewed in the layers tab. You can change the visibility with the checkmarks to see what layers are defined in the footprint.
This is a single sided layout, so the top layers and the board outline are all that are needed. Top and Bottom are the copper signal/trace layers. SMT footprints don’t have a bottom copper layer, but you can’t move it in this menu.
The clickstream Route -> Layer Setup -> Layer Stackup allows you to set the layer properties of your board. This will affect the 3D rendering after the board is designed and will produce a STEP file export with the correct thickness. Here we have defined a typical single sided MCPCB structure.
You can also place a table in the design with your layer stack definitions.
Next, we will create the board cutout in DraftSight, a 2D Cad program. If the cutout were rectangular, we would do this in the PCB layout software. Due to the complex shape of a starboard, it is easier to create a DXF file and import it into the PCB layout software.
Note that starboards cost more than rectangular boards. In many applications, a square or rectangular board with a few drilled holes will work. This can be designed in the PCB layout software and creating a DXF file is not needed.
Start the 2D Cad app and turn on the snap, e-snap, and ortho modes. Ortho mode will only draw orthogonal lines and e-snap will snap to control points (endpoints, centers, etc.) in your graphical elements.
Starboards are hexagonal so we will use the polygon tool. In the command window, enter 6 as the number of sides. Then type in the center point as 0,0 in the command window. Enter “s” for side as the distance option then enter the distance from the center of the polygon to the flat part of the side as 12.5. This will create a 25 wide mm hexagon.
Now we want to construct the notches for the mounting screws. We will use an M2.5 panhead screw. An M2.5 panhead has a head diameter of 5 mm and the thread diameter is nominally 2.5 mm.
Objects imported into PCB design software need to have connected lines. The easiest way to ensure everything is connected is to use construction lines and the trim tool. To create a slot for the screw, use the following procedure.
- Draw a line from 0,0 to the snap point at the top of the hexagon
- Draw a circle centered on the top of the hexagon to create an intersection point where we want to specify the screw location. We used a radius of 3 mm so that the diameter of the screw head is completely inside the starboard.
- Draw a 5 mm diameter circle centered on the intersection of the two objects above. This is a reference for the screw head clearance.
- Draw another circle with 2.5 mm + some clearance for the screw thread clearance hole. We used a 3-mm diameter.
- Offset the vertical reference line by the same amount as the clearance hole circle radius on both sides (1.5-mm). Change the layers if needed.
- Use the pattern function to copy these objects to the rest of the polygon vertices.
- Use the trim function to create the final slot geometry. Use the fillet command to remove sharp intersections.
- Save the outline as a DXF file.
Construction lines for the slot. Red are construction lines, purple is the screw head clearance reference, black is the board outline object we are working on.
Pattern commands
After patterning
One slot after trimming and fillet operations.
Starboard outline after all objects are trimmed and filleted.
Switch back to the PCB layout software and insert the DXF file.
Settings menu for DXF file insertion.
Starboard and footprint after DXF file insertion.
Next, we want to design the solder pads for the starboard. These need to be large enough to accommodate the wires we plan to use at different wire angles. The SST-10-B product has a maximum current rating of 1.5 A which can be used to size the conductors. Looking this up, we find that 20 AWG is the thinnest wire that is rated for 1.5 A and that the wire diameter is nominally 0.81 mm.
We can use the Cad file to figure out a reasonable size and the center-to-center distance for the solder pads. If you are planning on using strings of starboards, it is easiest to solder the wires diagonally in the pad.
In the PCB layout software, click “Place Pad” and add two pads using the settings show below.
Click on each pad and adjust the insertion point to x = +/- 8.5 and y = 0
Starboard with pads inserted.
Inspect the openings in the soldermask by turning off the visibility of everything else. This is one of the advantages of using PCB layout software where the layers are predefined.
Soldermask openings and board outline.
Use a trace width calculator to pick the trace width needed for 2-oz copper at 1.5 A. We used https://www.4pcb.com/trace-width-calculator.html and chose to use 0.3 mm.
Click on “Manual Trace” and set the width to 0.3 mm
Add these two traces. It is a good habit to click near the center of the pads to ensure connections. You can drag the traces around if you want a different layout.
Now connect the thermal pad to a copper pour area.
PCB design software has a native copper pour command, and we will use it here. If you want a more elaborate layout, you can use the DXF creation and import technique used above to draw the board outline. If you use this option, there is a “Fill Closed Areas” checkbox that needs to be clicked. You can export the PCB layout as a DXF file and draw your features using your existing design as reference geometry.
To draw the copper flood with native PCB layout tools, click the “Place Copper Pour” button and add points to the layout. Right click and “enter” on the last point. We will draw a hexagon with vertices aligned with the screw notches.
Next, adjust the coordinates of the vertices. We can use some construction lines in our Cad file to determine appropriate points. In the figure below we construct a 1 mm offset from the screw heads and round to even mm distances from center to get the values 8, 7, 4 mm.
The red circles mark the points we want for the hexagon vertices. Rounding the values to even millimeters gives 4, 8, and 7-mm distances from the center of the hexagon.
Select the copper pour feature (near a vertex) and right click -> properties -> Border. Edit the points.
Now connect the thermal pad to the copper pour feature. This thermal pad does not yet have a net name. To create a new net, manually draw a trace from the LED thermal pad to the copper pour. This will create Net 2 in the sidebar. Now connect the copper pour to Net 2 in the connectivity menu.
The thermal pad is now connected to the heat spreading copper pour. The manual trace we added to create Net 2 is smaller than (and underneath) the traces generated in this step so it is not visible.
If you want a more complex copper pour such as a circular perimeter, this is a good place to export the design as a DXF file and create your own pour layout in 2D Cad software. All of the offsets have been created so less editing is needed.
Luminus recommends connecting the thermal pad to the cathode(-). You can add a trace to connect the thermal pad to the cathode (-) as shown below.
Now add labels. We will add the Luminus logo and the SST-10 designation. Most corporate websites have downloadable logos, and we downloaded the Luminus logo from our website to use as a source file. In raw form, this graphic is too long so we cropped it with graphics software. We will omit the click stream but using the menus under properties you can adjust the lettering size and placement in the same way we did the pad placement.
We will call this done and explore the file export options. For fabrication, you need Gerber files. For 3D modeling you need step files. For dimensional references, a DXF file is useful. The Gerber and DXF export options are here:
To generate a STEP file, there are a few more steps. Click on 3D visualization.
You will likely get this message. If you want a model without an LED package, click OK.
STEP file without LED package.
If you want a file with the LED, download the STEP file from SnapEDA and complete this menu. We downloaded the file early in this walkthrough.
Click the three dots under Edit and tell the software where the step file is located.
Final 3D render. We had to move the logo to the silkscreen layer to get it to show in the rendering.
Once the PCB layout is done, it is easy to modify it. For example, below we rotated the LED 30 degrees to line up with the starboard vertices. Some minor edits were needed but it only took a few minutes.
------------------------------------------------------------------------------------------------------------------
Luminus Website https://www.luminus.com/
Luminus Product Information (datasheets): https://www.luminus.com/products
Luminus Design Support (ray files, calculators, ecosystem items: [power supplies, lenses, heatsinks]): https://www.luminus.com/resources
Luminus Product Information sorted by Applications: https://www.luminus.com/applications
Where to buy Samples of Luminus LEDs: https://www.luminus.com/contact/wheretobuy.
Comments
0 comments
Please sign in to leave a comment.