In PCB projects, panelization is an essential step. It involves arranging multiple PCB boards into a larger panel, following specific rules, to facilitate mass production and efficient processing. For designers, how to efficiently and accurately carry out panel layout is a challenge that must be addressed in every project. Fortunately, with the help of specialized computer-aided manufacturing tools like CAM350, the panelization process becomes much more efficient and precise. This article will use a 2-layer PCB designed with Altium Designer (AD) as an example, offering a detailed guide on how to use CAM350 software for panelization. Whether you’re a beginner or an experienced designer, this guide will provide you with practical tips to help you complete panelization tasks more efficiently in your future projects.
1. Building the Panel Layout in AD
First, we need to set up the entire panel layout in Altium Designer. For this example, we’ll use a 2×3 panel layout. As shown in the image, it’s important to set the origin at the lower-left corner of the PCB, rather than the lower-left corner of the manufacturing panel. This is crucial because, once the Gerber files are imported into CAM350, the origin will be accurately aligned with the grid points, which will assist in auto-snapping during subsequent steps, improving precision.
Additionally, it’s recommended to place string identifiers on each layer of the panel. These identifiers will help you easily recognize each layer during the panelization process.
2. Determine the Offset Distances
Next, measure the offset distances between the panels, which are 66.36 mm and 46.00 mm, as shown in the image. Record these values, as they will help you quickly and precisely align the panels in CAM350.
3. Check and Export Gerber Files
Once the panel layout is set up, export the design as Gerber files. Before exporting, run the Design Rule Check (DRC) to ensure that the PCB design is error-free, preventing issues during the manufacturing process.
If the DRC detects any issues, they’re often related to pad and via overlaps. You can resolve these issues by adjusting copper pours or rearranging components. Once you’ve confirmed the design is error-free, export the Gerber files. Typically, this process generates multiple files—24 files in this case.
4. Import Gerber Files and Set Up CAM350
After exporting the Gerber files, open CAM350 and import the files. To do this, click File in the menu bar, select Open, navigate to the folder containing the Gerber files, select all the files, and click Open.
Next, set the appropriate units and precision. Go to Settings, click Units, and ensure the unit is set to millimeters (mm). In the same menu, set the Resolution to maximum precision to ensure detailed operations.
After importing the files, go to the Layer Manager on the left side, find the Board Outline Layer, right-click, and select Hide. This step will clean up the display and make it easier to focus on the actual panelization process.
5. Copying the Design Elements
Now that CAM350 is set up, we can begin the copying process. Press W + C to enter copy mode, and the cursor will change to a selection tool. You can now select the area you want to copy. If it’s hard to select, you can press the S key to turn off grid snapping, allowing for more flexible selection.
Once you’ve selected the area, right-click to confirm your selection. The cursor will change to a rectangular shape.
Next, move the copied design elements to their target locations. First, select the board outline in the File Manager area and right-click to display it. Then, use the mouse middle button to zoom in or out, ensuring you can accurately align the origin.
6. Set the Copy Origin and Precisely Align
To ensure precise alignment of the copy origin, press the F key to toggle the line display to outline mode. Press F again to show the centerlines, which will help you precisely locate the intersection of lines. Zoom in until the cursor perfectly aligns with the intersection point, then click the left mouse button to start copying.
At this point, use relative coordinates for the offset operation. Enter the following coordinates for the copy:
X: 66.36 mm, Y: 0 mm, then press Enter to confirm and copy the first item.
Then, enter the following coordinates sequentially:
- X: 0 mm, Y: 46 mm
- X: 0 mm, Y: 46 mm
- X: -63.6 mm, Y: 0 mm
- X: 0 mm, Y: -46 mm
Press Enter after each entry, and the system will automatically place the copied items at the specified positions.
Once all the elements are copied to their designated positions, right-click to confirm the copy operation, and end the selection. The panel layout is now complete, and you can proceed with the next steps.
7. Export Gerber and Drill Files
After completing the panelization, you’ll need to export the Gerber files and drill files. In CAM350, go to File → Export → Gerber Data, set the format and save path, then click Apply and OK to export.
For the drill files, go to File → Export → Drill Data, configure the format and path, and click Apply and OK to finish exporting. Note: When exporting drill files, make sure the filenames are distinct. The default drill filenames may be identical, and if you don’t change them, you may get an overwrite prompt. It’s advisable to add a distinguishing symbol in the filenames, such as “FileName1” and “FileName2”.
At this point, the panelization is complete. Typically, 13 Gerber files will be generated. To ensure that the files are correct, it’s recommended to open a new CAM350 project, import the Gerber files you just generated, and check each layer carefully to ensure everything is in order.
Ending
Panelization can often be a daunting task for PCB designers, but with the powerful tools offered by CAM350, it becomes a streamlined and precise process. By following this step-by-step guide, you’ve learned how to efficiently set up, copy, and export your panelized PCB designs.
The key to success lies in the careful preparation of your design in Altium Designer and the meticulous attention to detail when aligning your boards in CAM350. This ensures a smooth manufacturing process and a high-quality final product. Whether you are working on small-scale prototypes or preparing for mass production, these techniques will help you optimize workflow and reduce the likelihood of costly errors.
You Might Be Interested
Learn how to efficiently complete PCB panelization with CAM350 in this step-by-step guide. From setting up the layout in Altium Designer to exporting Gerber and drill files, discover key tips to streamline your design process and ensure precision in production.
Discover the power of CAM350 with our comprehensive tutorial! Learn how to optimize PCB design for manufacturing, from file import to drill optimization. Enhance your production process, minimize errors, and improve efficiency. Perfect for engineers and designers!
PCB solder mask openings are crucial for various applications, including test points, heat dissipation, grounding, gold fingers, and current capacity enhancement. Design considerations, like choosing between opening and tenting, are vital to prevent issues such as solder bridging. The implementation process involves defining positions, determining layers, creating opening objects, specifying connections, and ensuring compliance with manufacturing standards.
Learn why PCB trace length matters and how it affects signal integrity. Discover how excessive trace length can lead to issues like signal attenuation, delay, and crosstalk, and how to optimize trace length for better circuit performance and reliability.
Learn how to avoid and suppress signal reflection in PCBs to ensure signal integrity in high-speed circuit designs. This guide covers the principles of signal reflection, its causes, and practical solutions like routing topologies and termination techniques.
PCB thickness is critical for design, affecting mechanics and layout. Standards vary based on needs and manufacturing capabilities. Components include copper, substrate, and pre-preg layers. Increased thickness provides benefits like durability. Designers must evaluate the need, considering factors like flexibility and operating environment, ensuring an optimal design for specific requirements.