Table of Contents
Altium Designer is a professional PCB design tool.
Design Rule Setup
Kind customers have provided loadable DRC rule and Stackup files for our 2 and 4 layer services.
Note, these files are not exhaustively validated or guaranteed by OSHPark, and may contain errors. Use your judgment and always verify your designs meet our service specs to prevent design defects that could affect your boards. If you have corrections or find errors, please email support.
known issues: Current minimum 2 layer specs are 10 mil drill hits, with 5 mil annular rings. The RUL file currently shows the older 13mil drill and 6mil ring
Generating Manufacturing Files
For accessing the various menus and output screens, see Altium’s Gerber Setup
Disabling “ Mechanical Layers to Add to All Gerber Plots”
Altium has an option
Mechanical Layers to Add to All Gerber Plots, which must have all layers unchecked. May footprints contain mechanical “courtyard” or “pick and place” data. If this is added to copper layers, it can create gerbers that will be fabricated with shorts. See Altium’s Gerber Setup for information on how to access this setting.
Internal Plane Polarity
We recommend submitting planes with a Positive polarity. See our Positive vs Negative Gerbers page for additional information.
For best results, place the outline by itself on the
Keep Out, or on a
Mechanical Layer (normally 1 or 2). This will generate the outline on
.GKO or a
We need the drills exported in the 2:4 inches format or a 3:3 metric format. Check out our Drill File CAM configuration page for settings that we know will work correctly.
We do not currently support slots from Altium’s standard callout. Currently, these must be added to the board outline as indicated on our cutouts and slots guide.
Missing Drill File
Altium keeps the drill data in the
project-name.TXT file. Make sure any uploaded zip files include this file.
Drill file not being read correctly
Try exporting the drill file with the
INCH units. Some format issues in
METRIC are more difficult to reliably correct.
Internal Layer names
If you’re using a 4 layer stackup with both “power” and “signal” internal layers, Altium will generate the internal layers as
G1. Unfortunately, this makes it impossible for us to determine the correct layer order, since multiple layers identify themselves as “Internal Layer 1”.
To correct this, simply rename the layers using the
G3L extensions. The
G2L will be near the Top Copper Layer, and
G3L will be near the bottom layer.