Importing Gerber and drill files

To create a product, you need to do the following:

  1. Using the CAD system of your choice, generate Gerber and Drill files for your product. See Gerber file generation tips for info on generating files from some commonly used CAD systems.
  2. Prepare for a new product. Open the Import Module, or choose File|New product if you have previously been working with a different product.
  3. Open the data files. Choose File|Open files to open files and add them to the files listed in the Files tab. If a single zip file is added, then this will be unpacked and its contents added to the Files tab. You may select multiple files from the same folder. You can also choose File|Open files again to add additional files to the Files tab.
  4. Link files to their corresponding board layers. If Autolinking is on, and the Import Module recognizes the filenames as matching one of the defined filters, then recognized files will be linked automatically to their corresponding layers. Files which are not autolinked must be linked manually. This is done by clicking on the blue text in the Layer column of the Files tab and selecting the desired layer from the layer menu. The file image is displayed, in order to help select the correct layer. Right-click on a file to view the file as text or change the file type.
  5. Review drill holes. In the Layer overview, set check marks by the drill layers and a copper layer, then go to the Drill tools tab. This tab lists the drill files and drill tools which have been linked. Ideally, the drill holes will be displayed centered on their corresponding copper pads. If not, see the user manual for information on how to make offset or scaling adjustments. Drill tool sizes are listed, rounded to the nearest actual tool size at the manufacturer. If tool sizes could not be extracted from the drill file, these must be entered manually by clicking in the Manuf. size column and typing in the correct size. Be sure to also check/correct plating for each tool, and drill depth for each file.
  6. Define the board contour. Go to the Contour tab. The Active layer (by default, the Board layer) is shown in blue and other layers are shown in gray. Ideally, selecting a segment of the outer contour, causes the entire contour to be highlighted. If necessary, use the + and – icon buttons to select/deselect the remainder of the contour (and no other segments). If the selected segments form a closed loop, then the Outer button in the Contour tab will be enabled. Click on the Outer button to define the outer contour. Select and define any additional cutouts, routed tracks, or scoring lines.
  7. Enter product specifications. Go to the board specs tab. You must specify a product name and select or define a stackup. In addition, you may choose non-standard surface finish, solder mask color and notation color. If the product is to have electrolytic (hard) gold applied to connector surfaces, then the gold area (in cm²) must also be specified. Then go to the board stats tab. Here you must specify minimum track width, clearance and annular ring for the product.
  8. Place the manufacturer's identifier. The manufacturer adds a product/batch number to the board as part of the production process. You may select the position of the identifier by clicking on the No. toolbar button and placing the rectangle at the desired position on the board. The identifier will appear on the Notation Top layer. If you do not place the identifier, then the manufacturer will choose an appropriate location prior to production.
  9. Add symbols (optional). Click on the Symbols toolbar button. Choose the desired symbol by clicking on the appropriate toolbar button. Select the desired layer and then draw a bounding rectangle for the symbol.
  10. Publish the product. Choose File|Publish to Product Browser to publish the new product:
    • Go through each item in the approval checklist to insure that you haven't forgotten anything. Click the OK button to continue.
    • Once the product has been published to the server, the new product number will be displayed. You'll find the product in the Never Ordered folder of the product browser.

Specifying custom buildups in Macaos Enterprise

Specifying custom buildups in Macaos Enterprise

A custom buildup may be specified either as a free build or as a constrained build. With a free build, only the copper thicknesses, the total thickness, and the dielectric material are specified. With a constrained build, the individual dielectric thicknesses and materials are also specified. An aluminium carrier or core may be added to a free build. Use the radio buttons to switch between the two modes. Note: Constrained builds may only be defined for multi-layer buildups.

In either case, there will be one metal specification for each layer, and each layer is separated by one dielectric specification. In addition (for 2 or more layer builds) plating is automatically added at the top and bottom. Additional plating layers may be added (for buried vias or sequential buildup) where necessary (see below).

The total buildup thickness is shown (for constrained builds) or specified (for free builds) at the bottom of the stackup builder. The default thickness tolerance is ±10%. You should not choose a different tolerance unless specifically required for your application, since this can greatly increase manufacturing costs and lead time.

The dielectric material for the build is also specified at the bottom of the stackup builder. This specification applies to all dielectric layers, unless otherwise specified for a specific layer. Select one of the commonly used material descriptions, or enter your own description. If left blank, standard FR-4 (IPC-4101C/21) will be specified.

When specifying a constrained build, if you start at the top layer and work downward, then the stackup builder will automatically help to create a symmetric buildup by inserting the same layer specifications from the bottom layer upwards. These automatic specifications may be changed later, if necessary.

Metal layers

Metal layers are specified as base (unplated/unfinished) thickness, since plating is specified as a separate layer.
Plated layers should therefore typically be specified as ½ ounce (20μm) less than the desired plated/finished thickness. The thickness may be specified as follows:

  • select a thickness from the drop-down list
  • enter a thickness in μm as an integer value
    for example: 105 specifies a thickness of 105μm (3 ounce)
  • enter a thickness in mm as a real number value
    for example: 0.105 specifies a thickness of 105μm (3 ounce)

Metal layers are normally copper. A material description for the layer should only be added if some other conductive material than copper is to be used.

Plating

Plating is automatically added to the outer layers of buildups with 2 or more layers. For buildups with plating on inner layers (i.e. for buried vias or for sequential buildup), plating layers should be added by right-clicking on the word Metal and selecting whether the plating should be added above or below the metal layer. Plating should always be added to the "outside" of the set of layers to be plated.

If plating is not correctly specified for inner layers, then buried vias will not be correctly drawn in the product stackup drawing.

Note: When specifying plated inner layers, the inner layer (foil) thickness should be specified as 20 μm less than the desired layer thickness.

The plating thickness may not be specified. For IPC Class 1 or 2, plating shall be at least 20 μm thick. For IPC Class 3, plating shall be at least 25 μm thick. Note that actual plating thickness can vary greatly from one place to another on the board, subject to plating process conditions. It is therefore not advisable to use a plated layer for impedance critical signal paths.

Dielectric layers

Dielectric layers are specified as a thickness or as a combination of prepreg plies (sheets). The thickness may be specified as follows:

  • select prepreg(s) or a thickness from the drop-down list
  • enter a thickness in μm as an integer value
    for example: 105 specifies a thickness of 105μm (3 ounce)
  • enter a thickness in mm as a real number value
    for example: 0.105 specifies a thickness of 105μm (3 ounce)
  • enter a prepreg combination, such as 1x7628 or 2x2116+1x1080

A prepreg is specified as qty x type. Valid prepreg types are 106, 1080, 2112, 2113, 2116, 2125, and 7628. To specify a combination of prepreg types, separate the prepreg specifications with a + symbol. There should be no spaces in the prepreg specification.

The dielectric material for individual layers should only be specified in cases where the material differs from the
overall material description specified at the bottom of the stackup builder.

Note: The finished thickness of a prepreg dielectric layer will often be less than the nominal thickness listed in the stackup builder. This is due to the fact that epoxy in the prepreg layer will flow into the spaces where metal has been removed (etched) from the inner layers. The actual thickness reduction is a function of the metal layer thickness and the metal coverage of the layer. See Prepreg Thickness Chart or Multilayer Dielectric Thickness Calculation for a more detailed description.

Aluminium

Aluminium is sometimes used (especially in LED lighting applications) to improve the heat dissipation of a board. An aluminium carrier or core may be added to a free build with the check box (near the Help button). An aluminium carrier is added to the bottom of the build. An aluminium core replaces the dielectric of a 2-layer board.