Electronics Production
[Add the goal/objectives of this week here]
Test LED Board
Before milling my actual board design, my instructor, Mr. Dubick, wanted me and my peers to prepare and mill a test board. More specifically, he wanted us to practice utilizing the MakeraCAM software to generate toolpaths and using those toolpaths to mill our design on the Carvera Air CNC Machine.
To begin this process, I started with a pre-made PCB Gerber file. Since this board was meant to help me practice the workflow rather than design a board from scratch, beginning with a completed Gerber file allowed me to focus entirely on learning the CAM and machining process. This was helpful because it let me concentrate on how to prepare a PCB for milling, which is ultimately the most important part of electronics production.
The first step was to open MakeraCAM and start a new project. When creating the project, I selected the 3-Axis project type. After that, I went to the Stock Setup panel and clicked Edit so that I could define the size of the PCB material I would be working with. I set the dimensions of the stock to 127 mm in the x direction, 101 mm in the y direction, and 1.7 mm in the z direction.
This step was important because the stock setup defines the physical size of the material that the machine expects to cut. If these dimensions are incorrect, the toolpaths may be placed in the wrong area or extend beyond the board itself. By entering the correct stock dimensions at the start, I made sure that the project space in MakeraCAM matched the actual PCB blank I would be milling on the Carvera Air.
Once the stock was set up, the next step was to import the Gerber files. For this design, I only imported the Edge_Cuts and F.Cu files. This was because the board did not require any drilled holes since all of the components were surface-mount (SMD) components. Because of this, I did not need to import any drill files and could focus only on the copper traces and board outline.
After importing the files, I noticed that the design was slightly off-screen. To fix this, I selected every component in the design and clicked the M key, which opened the move panel. From there, I changed the anchor point to the lower-left corner, set the X-location to 6.00 mm, and set the Y-location to 6.00 mm. Doing this repositioned the board so that it sat more cleanly within the workspace and gave it a more reasonable margin from the edge of the stock.
With the files imported and positioned correctly, I could then move on to setting up the toolpaths.
2D Pocket Toolpath
The first toolpath I created was the 2D Pocket Toolpath. In electronics production, a pocket toolpath is used to remove material from within a selected area rather than simply tracing along the edge of a line. For PCB milling, this is useful because it removes copper around the traces and helps isolate them from the rest of the copper surface. In other words, this toolpath helps define the actual conductive paths by carving away the copper surrounding them.
To begin creating this toolpath, I first needed to define the correct cutting boundary. To do this, I deselected the outermost line of the design's outline. This was important because I did not want the first toolpath to include the exterior edge of the board. Instead, I wanted it to focus only on the internal copper geometry. Once I had the correct geometry selected, I went to the top toolbar and selected 2D Pocket Toolpath.
With the menu open, the next step was to set the cutting settings. I started by setting the Start Depth to 0.000 mm and the End Depth to 0.05 mm. Since PCB milling only requires removing a very thin layer of copper from the surface, this shallow depth made sense. The goal of this cut was not to go deep into the board, but rather to isolate the traces cleanly.
After that, I added two tools to the toolpath. The first was the 0.8 mm Corn tool, and the second was the 0.2 mm 30 degree Engraving (Metal) tool. I made sure that the 0.8 mm tool came first. This ordering was important because the larger tool could clear the broader open areas more efficiently, while the smaller engraving tool could then reach the tighter spaces and finer details that the first tool could not access.
I then set the Path Strategy to Parallel. This created a consistent back-and-forth cutting pattern across the selected area. For PCB milling, this was helpful because it created a clean and systematic clearing path around the traces. From the toolpath panel, I kept the other visible settings as they appeared, and after calculating the path I could clearly see the generated fill pattern spread throughout the selected copper-clearing regions.
Once all of those settings were in place, I clicked Calculate to generate the final pocket toolpath.
2D Contour Toolpath
With the pocket toolpath complete, the next step was to create the 2D Contour Toolpath. The purpose of the contour toolpath was to cut the actual board out from the surrounding stock. While the pocket toolpath only removed a shallow amount of copper around the traces, the contour toolpath followed the perimeter of the board and cut all the way through the PCB material so that the final board could be separated from the rest of the blank.
To begin creating this toolpath, I first hid everything in the visibility panel except for the Edge.Cuts layer. This made it much easier to focus on only the board boundary without accidentally selecting any of the internal copper geometry. Once only the edge cut layer was visible, I went to the top panel and selected 2D Contour Toolpath.
After that, I selected the outline of the design and deselected the outermost outside line so that only the inside line was selected. In the workspace, this selected line appeared dotted. This step was important because it ensured that the machine would follow the correct board boundary rather than the wrong exterior edge.
With the geometry selected, I then moved on to the cutting settings. I set the Start Depth to 0.000 mm and the End Depth to 1.7 mm. Since the PCB material itself was 1.7 mm thick, setting the end depth equal to the board thickness ensured that the contour cut would go all the way through the stock.
For the tool, I added the 0.8 mm Corn tool. From the settings visible in the MakeraCAM panel, this tool had a diameter of 0.800 mm, a Step Down of 0.300 mm, a Feed Rate of 500 mm/min, and a Plunge Rate of 300 mm/min. I also left the visible Clearance Height and Retract Height at 15.000 mm. I then scrolled down to the strategy section and selected Outside, which meant the machine would cut around the outer side of the chosen contour.
From there, I continued to the Tabs section. I selected Custom, clicked Add, and then placed 3 tabs around the edge of the board outline. These tabs were important because they kept the board attached to the surrounding stock during the cut. Without them, the board could come loose too early and shift while the machine was still cutting.
Once all of those settings were complete, I clicked Calculate to generate the final contour toolpath.
After generating both toolpaths, I confirmed them by clicking the Preview Toolpath icon. This step was important because it allowed me to visually check whether the cuts looked correct before exporting anything. If the preview worked and the board geometry looked right, then I knew the file was ready for export.
I then went to the export menu, selected both toolpaths, and clicked Export. I saved the result as a .nc g-code file so that it could be used directly for milling.
The next section of this documentation will be about actually milling the board.