{"id":17788,"date":"2017-05-19T08:00:06","date_gmt":"2017-05-19T15:00:06","guid":{"rendered":"http:\/\/www.autodesk.com\/products\/eagle\/blog\/?p=1066"},"modified":"2023-09-25T15:11:54","modified_gmt":"2023-09-25T22:11:54","slug":"gerber-nc-drill-pcb-manufacturing-basics-1","status":"publish","type":"post","link":"https:\/\/www.autodesk.com\/products\/fusion-360\/blog\/gerber-nc-drill-pcb-manufacturing-basics-1\/","title":{"rendered":"Gerber & NC Drill: PCB Manufacturing Basics 1"},"content":{"rendered":"

PCB Manufacturing Basics Part 1: How to Generate Your Gerber and Drill Files<\/span><\/h1>\n\n\n

There\u2019s no greater reward than spending hours designing every last detail of your PCB and then finally getting your board back from your manufacturer. The wait can seem like an eternity when you first hand-off your design files, but when you receive that package on your doorstep, it\u2019s like an engineer\u2019s Christmas! In our PCB Basics Series we\u2019ve gone through the entire design process, starting with a visual representation of your circuit in schematic design, and then moving on to squeezing all of that theory into a physical footprint with components and traces. Now it\u2019s time to move on over to the post-design process to get ready for PCB manufacturing.<\/span><\/p>\n\n\n\n

It\u2019s at this juncture where you\u2019re tasked with assembling all of the files and documentation that your manufacturer will need to successfully produce your board. And once they have everything they need, you get to sit back and wait for a package to arrive. But how does a manufacturer know how to make your PCB? They can\u2019t use your native EAGLE files. You\u2019ll have to send them <\/span>Gerber Files<\/b> and <\/span>Excellon Drill Files<\/b>.<\/span><\/p>\n\n\n

Gerbers and Drill Files Explained<\/h2>\n\n\n

If you\u2019ve never had a board manufactured, then hearing about Gerbers, Excellon, and NC Drill Files might sound like a foreign language. After all, can\u2019t you just send your Autodesk EAGLE schematic and layout files directly to your manufacturer and let them handle the rest? If only it were that easy. As we all know, Autodesk EAGLE isn\u2019t the only PCB design software out there. There are a ton of other offerings, all with their own native file format. Imagine if a manufacturer had to keep track of every native file format from each PCB design tool, throughout all time. It would be complete madness!<\/span>
Instead of relying on native file formats, every PCB design tool supports an intermediary manufacturing files, called Gerbers. These files describe the copper of every layer in your PCB in a way that a computer-aided manufacturing system (CAM) can understand. When Gerber artwork was first invented, they were used to provide instructions to a photoplotter machine that would create a picture of your PCB using light on a unexposed piece of film. These days, Gerbers are used to controls a laser plotting machine to make an image of all the traces, holes, vias on your PCB layout.<\/span><\/p>\n\n\n

Gerber Files by Type and Format<\/h3>\n\n\n

The trick with Gerbers is that every file you generate will be associated with a particular layer on your board layout, each with its own unique file extension. The standard file extensions you\u2019ll work within Autodesk EAGLE today include:<\/span><\/p>\n\n\n

File Extension<\/b><\/td>PCB Layer<\/b><\/td><\/tr>
.cmp<\/span><\/td>Top Copper<\/span><\/td><\/tr>
.sol<\/span><\/td>Bottom Copper<\/span><\/td><\/tr>
.stc<\/span><\/td>Top Soldermask<\/span><\/td><\/tr>
.sts<\/span><\/td>Bottom Soldermask<\/span><\/td><\/tr>
.plc<\/span><\/td>Top Silkscreen<\/span><\/td><\/tr>
.pls<\/span><\/td>Bottom Silkscreen<\/span><\/td><\/tr><\/tbody><\/table><\/figure>\n\n\n\n

Another thing to remember about Gerbers is their available formats – Gerber RS-274D and Gerber RS-274X. The D format is the older standard and will use two files per layer on your PCB. The newer X standard has done away with the two file format and contains all of the information about a layer in a single file. Regarding having to manage your design data, this makes it a whole lot easier when you only have to keep track of one file per layer instead of two. We\u2019d always recommend using the Gerber RS-274X format; there\u2019s no reason not to these days. <\/span><\/p>\n\n\n

How About Those Drill Holes?<\/h3>\n\n\n

You might have noticed that one thing missing from the table above is any reference to a drill file. This is actually as a secondary file that you\u2019ll need to send to your manufacturer along with your Gerbers. The NC (Numeric Controlled) Drill File will be used to determine exactly where all of your drill holes are placed on your board and what size they need to be. Just as a heads up, you might also hear of an NC Drill File being referred to as an Excellon file, which is based on the drilling and routing machines that were made by the Excellon corporation back in the day.<\/span><\/p>\n\n\n\n

Now that you\u2019ve got a general idea of what Gerber and Drill Files are about let\u2019s dive into Autodesk EAGLE and see how to generate them.<\/span><\/p>\n\n\n

Generating Your Gerber Files<\/h2>\n\n\n

Autodesk EAGLE includes a handy computer-aided manufacturing (CAM) processor that allows you to load a CAM file and quickly generate the specific files you need for your design. In our example, we\u2019re going to load up the Gerber RS-274X CAM file. This will provide us with five individual Gerber files for the LED Flasher project we completed in our PCB Layout Basics Series <\/span>Part 1<\/span><\/a>, <\/span>Part 2<\/span><\/a>, and <\/span>Part 3<\/span><\/a>. Here\u2019s how to do this:<\/span><\/p>\n\n\n\n

    \n
  1. Open your PCB layout (.brd) file in the <\/span>Autodesk EAGLE Control Panel<\/b>.<\/span><\/li>\n\n\n\n
  2. Next, select the <\/span>CAM Processor \"cam-icon\" <\/b>tool at the top of your interface or select <\/span>File \u00bb CAM Processor<\/b> to open the <\/span>CAM Processor dialog<\/b>.
    <\/span><\/span>\n<\/li>\n<\/ol>\n\n\n\n
    \"cam-processor-dialog-default\"\/
    The default CAM Processor dialog without any CAM jobs loaded.<\/em><\/figcaption><\/figure>\n\n\n\n
  3. There\u2019s no CAM job loaded, so let\u2019s do that. Select <\/span>File \u00bb Open \u00bb Job<\/b>. Then navigate to your default EAGLE cam folder, choose the gerb274x.cam file, select <\/span>Open<\/b>.<\/span><\/li>\n\n\n\n
  4. As you can see there\u2019s now some new tabs added to each CAM file that will be generated with this job. Select the Process Job<\/b> button to create all of your Gerber files.
    <\/span><\/span>\n<\/li>\n\n\n\n
    \"gerber-job-cam-processor\"\/
    After loading the Gerber RS-274X CAM job, you\u2019ll have some new tabs for each layer of your design.<\/em><\/figcaption><\/figure>\n\n\n\n

    And that\u2019s it! Just one simple press of a button and all of the Gerber files you need to send to your manufacturer have been created for you. If you head back into your Autodesk EAGLE Control Panel<\/span>, you\u2019ll see all of these new Gerber files listed alongside your existing project files. <\/span><\/p>\n\n\n\n

    \"control-panel-gerber-files\"\/
    You can find all of your generated Gerber files in the Autodesk EAGLE Control Panel in your project folder.<\/em><\/figcaption><\/figure>\n\n\n

    Generating Your Drill File<\/h2>\n\n\n

    While the Gerber files you just generated contain all of the details a manufacturer needs to know about your individual layers, what they don’t include is information about your drill holes. What you need now is a file that will specify the location and size of each of your drill holes. Luckily the process for making this file in Autodesk EAGLE is just as easy as making Gerbers. Here\u2019s how:<\/span><\/p>\n\n\n\n

      \n
    1. Select the <\/span>CAM Processor \"cam-icon\" <\/b>tool at the top of your interface or select <\/span>File \u00bb CAM Processor<\/b> to open the <\/span>CAM processor dialog<\/b>. <\/span><\/li>\n\n\n\n
    2. You now need to load a drill CAM job to get things started. Select <\/span>File \u00bb Open \u00bb Job<\/b>, and in your default EAGLE cam folder select the excellon.cam file, then select <\/span>Open<\/b>.<\/span><\/li>\n\n\n\n
    3. You\u2019ll now have a single Generate drill data tab available, which will grab the data from layers 44 Drills<\/b> and <\/span>45 Holes<\/b>, just what you need. Select the <\/span>Process Job<\/b> button to generate this file<\/span>.<\/span><\/li>\n<\/ol>\n\n\n\n
      \"ncdrill-cam-processor\"
      Loading the Excellon CAM job will create an NC Drill File based on your Drill and Hole layer data.<\/em><\/figcaption><\/figure>\n\n\n\n

      Just like all of your Gerber files, your NC Drill File will be stored in your project folder that you can access through the Autodesk EAGLE Control Panel or folder directory. Look for the .drd file, that\u2019s the one you just made.<\/span><\/p>\n\n\n

      Time to Pack it Up<\/h2>\n\n\n

      At this point, you\u2019ve got all the files you need to send to your manufacturer to have a bare board made. The key word here being bare board. If you\u2019re also planning to have your manufacturer assemble your components, then you\u2019ll likely need to send some additional files like a Bill of Materials (BOM). We\u2019ll be saving that for PCB Manufacturing Basics Part 2.<\/span><\/p>\n\n\n\n

      One thing to keep in mind is that while we used EAGLE\u2019s standard Gerber CAM file to generate our documentation, some manufacturers also offer their own CAM files that you can download. When you load one of these up, they\u2019ll provide a job template for generating Gerbers in their specific format.<\/span><\/p>\n\n\n\n

      Before you generate Gerber files of your own, be sure to first check with your manufacturer to see if they offer their own CAM file for Autodesk EAGLE or their preferred output format. Otherwise, you should be safe using the standard Gerber RS274-X format available in Autodesk EAGLE.<\/span><\/p>\n\n\n

      You Designed it Right, But Can You Make It?<\/h2>\n\n\n

      The entirety of this blog relied on a big assumption that the design you made in Autodesk EAGLE was actually manufacturable. Sometimes this isn\u2019t the case, whether that\u2019s because you put silkscreen on a pad, or you have an open loop. Whatever the situation, the difference between a completed design and a design that\u2019s ready for manufacturing can be two different realities.  <\/span><\/p>\n\n\n\n

      SO before you ever go about sending any Gerber or NC Drill Files off to your manufacturer, we always recommend doing a thorough check to confirm that what you designed is actually what your manufacturing files show. We\u2019ll be covering this process of validating your design in more detail in PCB Manufacturing Basics Part 3. During this validation process, you\u2019ll also want to officially decide on what manufacturer you\u2019d like to use. Here are a few:<\/span><\/p>\n\n\n\n