Rules Check

Rules Check tests a board against design rules. It checks trace size, clearances, annular rings, drill sizes and slot widths. Each enabled rule runs on the objects you select, and the violations are listed in a table. You can export the table to CSV.

Where to find it

• Menu: Plugins > Rules Check.
• Keyboard: Alt+R.
• The panel opens in a tab next to Project and Properties. The tab shows the plugin name.

Screenshot placeholder: images/Rules-Check-1.png — the Rules Check panel with the Select All, Top, Bottom, Outline and Excellon object rows visible.

Quick start

1. In Top and Bottom, select the Copper, Solder Mask and Silk objects. Check the box of each object that you want to test.
2. In Outline, select the outline object and check it.
3. In Excellon, select the PTH and NPTH objects and check them.
4. Set Preset to a process, for example JLCPCB standard. Or keep Custom and set each rule value.
5. Check the rules to run. Set each value.
6. Click Run Rules Check. The violations appear in the table below.
7. Click Export CSV to save the table.

Screenshot placeholder: images/Rules-Check-2.png — the results table with a few violation rows and the summary line above it.

Parameters

Select All

Each Select All checkbox checks or clears all the boxes of its group. The box stays checked only when all the boxes of the group are checked.

Parameter	Description	Selected by default
Gerber	Checks all Gerber object boxes (Top, Bottom and Outline).	Unchecked
Excellon	Checks both Excellon object boxes (PTH and NPTH).	Unchecked
Copper Rules	Checks the copper rules.	Unchecked
Silk Rules	Checks the silk rules.	Unchecked
Soldermask Rules	Checks the soldermask rule.	Unchecked
Holes Rules	Checks the hole rules.	Unchecked

Top and Bottom

Each row has an object selector and a checkbox. The checkbox enables the object for the run.

Parameter	Description	Selected by default
Copper (Top, Bottom)	The copper Gerber object. Used for the copper rules.	—
Solder Mask (Top, Bottom)	The soldermask Gerber object. Used for the silk to soldermask and the soldermask sliver rules.	—
Silk (Top, Bottom)	The silkscreen Gerber object. Used for the silk rules.	—

Outline

Parameter	Description	Selected by default
Outline	The Gerber outline (cutout) object. Used for the outline rules.	—

Excellon

Parameter	Description	Selected by default
PTH	The Excellon object with plated holes, or a general Excellon file.	—
NPTH	The Excellon object with non-plated holes.	—

Preset

Parameter	Description	Selected by default
Preset = Custom	You set every rule value. Editing a value returns the preset to Custom.	Selected by default
Preset = Home etching, CNC milling (0.2 mm V-bit), JLCPCB standard, PCBWay standard, OSH Park	Fills the rule values with the typical values of that process. These are typical starting values. Confirm them with your manufacturer. See the Advanced section for the values.	—

Copper Rules

Each rule has a checkbox (rule enabled) and a Value field. The unit is mm (or inch in an inch project).

Parameter	Description	Selected by default
Trace Size	Checks the minimum trace width. Flashed pads are not traces.	Enabled, 0.25 mm
Copper to Copper clearance	Checks the minimum gap between two copper features of the same layer.	Enabled, 0.25 mm
Copper to Outline clearance	Checks the minimum distance between copper features and the outline.	Enabled, 1.0 mm
Minimum Annular Ring	Checks the minimum copper ring around a drilled hole in a pad.	Enabled, 0.3 mm
Copper gap vs isolation tool	Checks that the gaps between copper features are wide enough for the isolation tool. The Value is the tool diameter.	Disabled, 0.1 mm

Silk Rules

Parameter	Description	Selected by default
Silk to Silk Clearance	Checks the minimum gap between two silkscreen features of the same layer.	Enabled, 0.25 mm
Silk to Solder Mask Clearance	Checks the minimum distance between silkscreen features and soldermask openings.	Enabled, 0.25 mm
Silk to Outline Clearance	Checks the minimum distance between silkscreen features and the outline.	Enabled, 1.0 mm

Soldermask Rules

Parameter	Description	Selected by default
Minimum Solder Mask Sliver	Checks the minimum width of the soldermask left between two openings.	Enabled, 0.25 mm

Holes Rules

Parameter	Description	Selected by default
Hole to Hole Clearance	Checks the minimum wall between the edges of two holes or slots.	Enabled, 0.3 mm
Hole Size	Checks that the drill diameters are not below this value.	Enabled, 0.3 mm
Minimum Slot Width	Checks the minimum slot width. This is the tool diameter that cuts the slot.	Enabled, 0.5 mm
Hole to Outline clearance	Checks the minimum distance between the edge of a hole and the outline.	Enabled, 0.5 mm
Hole to Copper clearance	Checks the minimum distance between the edge of a hole and foreign copper.	Enabled, 0.2 mm

Run and Results

Parameter	Description	Selected by default
Run Rules Check	Runs the enabled rules on the selected objects. It creates a document with the report.	—
Cancel	Stops the running check and discards its results. Enabled while a check runs.	Disabled
Export CSV	Saves the violations of the last check as a CSV file. Enabled after a check.	Disabled
Summary line	Shows the number of violations and the number of failed rules.	—
Results table	One row per violation: Rule, Layer, X, Y, Value and Limit. A rule that could not run shows the status in the row. Each violation row keeps its X and Y location.	—
Reset Tool	Resets the tool parameters to their default values.	—

Screenshot placeholder: images/Rules-Check-3.png — the Preset combo open, with the list of presets visible.

Advanced

Rule status

• A rule that has no layers selected shows an error. Select the layers for the rule, or disable the rule.
• A rule with nothing to check shows NOTHING TO CHECK.
• A rule that passes adds no row to the table.

CSV columns

The CSV file has these columns: rule, layer, x, y, value, limit, status.

Preset values

The values are in mm. For inch units, the values are converted.

Rule	Home etching	CNC milling (0.2 mm V-bit)	JLCPCB standard	PCBWay standard	OSH Park
Trace Size	0.3	0.2	0.127	0.127	0.152
Copper to Copper	0.3	0.2	0.127	0.127	0.152
Copper to Outline	0.5	0.5	0.3	0.3	0.381
Copper gap vs isolation tool	—	0.2	—	—	—
Minimum Annular Ring	0.3	0.3	0.13	0.15	0.127
Hole Size	0.6	0.6	0.3	0.3	0.254
Hole to Hole	0.5	0.5	0.5	0.5	0.381
Minimum Slot Width	1.0	1.0	0.65	0.8	0.5
Hole to Outline	0.5	0.5	0.5	0.3	0.381
Hole to Copper	0.3	0.3	0.254	0.25	0.254
Silk to Silk	0.2	—	0.15	0.15	—
Silk to Solder Mask	0.2	—	0.15	0.15	—
Silk to Outline	0.5	—	0.3	0.3	—
Minimum Solder Mask Sliver	0.2	—	0.1	0.1	—

A dash means the preset does not set that rule. The rule keeps its value.

The command-line version is check_rules. See Tcl Command Reference.

See also

• Gerber Object
• Excellon Object
• Isolation Routing
• Drilling
• Report
• Tcl Command Reference
• Preferences Plugins