EAGLE Help

Design Rules


Design Rules define all the parameters that the board layout has to follow.

The Design Rule Check checks the board against these rules and reports any violations.

The Design Rules of a board can be modified through the Design Rules dialog, which appears if the DRC command is selected without a terminating ';'.

Newly created boards take their design rules from the file 'default.dru', which is searched for in the first directory listed in the "Options/Directories/Design rules" path. If no such file is present, the program's builtin default values apply.

Note regarding the values for Clearance and Distance: since the internal resolution of the coordinates is 1/10000mm, the DRC can only reliably report errors that are larger than 1/10000mm.

File

The File tab shows a description of the current set of Design Rules and allows you to change that description (this is strongly recommended if you define your own Design Rules). There are also buttons to load a different set of Design Rules from a disk file and to save the current Design Rules to disk.
Note that the Design Rules are stored within the board file, so they will be in effect of the board file is sent to a board house for production. The "Load..." and "Save as..." buttons are merely for copying a board's Design Rules to and from disk.

Clearance

The Clearance tab defines the various minimum clearance values between objects in signal layers. These are usually absolute minimum values that are defined by the production process used and should be obtained from your board manufacturer.
The actual minimum clearance between objects that belong to different signals will also be influenced by the Net Classes the two signals belong to.

Note that a polygon in the special signal named _OUTLINES_ will be used to generate outlines data and as such will not adhere to these clearance values.

Distance

The Distance tab defines the minimum distance between objects in signal layers and the board dimensions, as well as that between any two drill holes. Note that only signals that are actually connected to at least one pad or smd are checked against the board dimensions. This allows edge markers to be drawn in the signal layer without generating DRC errors.

For compatibility with version 3.5x the following applies: If the minimum distance between copper and dimension is set to 0 objects in the Dimension layer will not be taken into account when calculating polygons (except for Holes, which are always taken into account). This also disables the distance check between copper and dimension objects.

Sizes

The Sizes tab defines the minimum width of any objects in signal layers and the minimum drill diameter. These are usually absolute minimum values that are defined by the production process used and should be obtained from your board manufacturer.
The actual minimum width of signal wires and drill diameter of vias will also be influenced by the Net Class the signal belongs to.

Restring

The Restring tab defines the width of the copper ring that has to remain after the pad or via has been drilled. Values are defined in percent of the drill diameter and there can be an absolute minimum and maximum limit. Restrings for pads can be different for the top, bottom and inner layers, while for vias they can be different for the outer and inner layers.
If the actual diameter of a pad (as defined in the library) or a via would result in a larger restring, that value will be used in the outer layers. Pads in library packages usually have their diameter set to 0, so that the restring will be derived entirely from the drill diameter.

Shapes

The Shapes tab defines the actual shapes for smds and pads.
Smds are normally defined as rectangles in the library (with a "roundness" of 0), but if your design requires rounded smds you can specify the roundness factor here.
Pads are normally defined as octagons in the library (long octagons where this makes sense), and you can use the three combo boxes to specify whether you want to have pads with the same shapes as defined in the library, or always square, round or octagonal. This can be set independently for the top and bottom layer.

Supply

The Supply tab defines the dimensions of Thermal and Annulus symbols used in supply layers.
Please note that the actual shape of supply symbols may be different when generating output for photoplotters that use specific thermal/annulus apertures!

Masks

The Masks tab defines the dimensions of solder stop and cream masks. They are given in percent of the smaller dimension of smds, pads and vias and can have an absolute minimum and maximum value.
Solder stop masks are generated for smds, pads and those vias that have a drill diameter that exceeds the given Limit parameter.
Cream masks are generated for smds only.

Misc

The Misc tab allows you to turn on a grid and angle check, and to limit the maximum number of errors that will be reported.


Index Copyright © 2002 CadSoft Computer GmbH