To assist in resolving common Design for Manufacture (DFM) issues faced by having silkscreen overlapping exposed copper, holes and board shape, the PCB editor includes a dedicated feature for preparing the silkscreen for your boards. These issues can be effectively addressed by:
automated clipping of silkscreen lines and arcs;
automated clipping or movement of fills and regions;
automated movement of silkscreen text and component designators.
The silkscreen preparation tool can also be accessed when creating a PCB footprint: learn more.
To access the silkscreen preparation tool in the PCB editor, use the Tools » Silkscreen Preparation command from the main menus. After launching the command, the Silkscreen Preparation dialog will open.
Use the dialog to configure the settings of the silkscreen object clipping/movement. The available options are:
All / Selected – choose to which objects the silkscreen preparation will be applied: all objects on the PCB or only those selected in the design space.
Overlay layers – choose to which overlay layers the silkscreen preparation will be applied: Top, Bottom or both Top & Bottom. The option is only available when All is selected above.
Use Design Rules – enable to use constraint values of the applicable Silk to Solder Mask Clearance and Board Outline Clearance design rules as the Silkscreen Clearance Distance. When the option is disabled, define the value of the Silkscreen Clearance Distance using the field below in the dialog.
Lines Minimum Remaining Length – if the line/arc length is less than the defined value after clipping, these objects will be removed from the PCB (including existing objects that were not clipped). Note that this length is the vertex-to-vertex length, not the edge to edge length (show image).
Silkscreen Clearance Distance – define the minimum acceptable value between silkscreen objects and exposed copper, holes and board edge. When the Use Design Rules option is enabled, the field is not available for editing, and relevant values are taken from the applicable Silk to Solder Mask Clearance and Board Outline Clearance design rules.
Auto-Action Text and Designators – enable to move silkscreen text strings and component designators away from exposed copper, holes and board edges if the distance between them is less than the Silkscreen Clearance Distance. The movement is limited by the Auto-Action Max Distance value.
Auto-Action Fill & Region – select an action to be performed for fills and regions when the distance between them and exposed copper, holes and board edges is less than the Silkscreen Clearance Distance:
None – fills and regions remain untouched.
Clip – fills and regions will be clipped to maintain the Silkscreen Clearance Distance. Fills are converted to regions if applicable.
Move – fills and regions will be moved away from exposed copper, holes and board edges. The movement is limited by the Auto-Action Max Distance value.
Auto-Action Max Distance – define a maximum distance to which text strings, component designators, fills and regions can be moved to maintain the Silkscreen Clearance Distance.
Delete Silkscreen Outside Board Shape – enable to remove silkscreen objects that are outside of the board shape.
Clip Locked Components and Primitives – enable to clip primitives that are locked or which parent components are locked.
Click OK to perform clipping and/or movement of silkscreen objects according to the settings in the dialog.
If an action cannot be performed for an object (e.g., a text string cannot be moved due to the limitation of Auto-Action Max Distance), a message for this object will appear in the Messages panel.
Use the Edit » Undo command to revert the last set of changes performed by the Silkscreen Preparation feature.
Below is shown an example of the silkscreen preparation tool performance.