Reference manual

This document is Copyright © 2010-2015 by it’s contributors as listed below. You may distribute it and/or modify it under the terms of either the GNU General Public License (http://www.gnu.org/licenses/gpl.html), version 3 or later, or the Creative Commons Attribution License (http://creativecommons.org/licenses/by/3.0/), version 3.0 or later.

All trademarks within this guide belong to their legitimate owners.

Contributors

The KiCad Team.

Feedback

Please direct any bug reports, suggestions or new versions to here:

Publication date and software version

Published on February 14, 2015.

Introduction to GerbView

GerbView is a Gerber file viewer (RS 274 X format), and is also able to display drill files from Pcbnew (in Excellon format).

It accepts up to 32 files (Gerber and/or Drill files)

Files can be displayed using a transparency mode or stacked mode.

For more information about the Gerber file format please have a read at the specification in The Gerber File Format Specification - Ucamco.

Main Screen

gerbview_main_screen_png

Top toolbar

gerbview_top_toolbar_png

gerbview_clear_layers_png

Clear all layers

gerber_file_png

Load Gerber files

gerbview_drill_file_png

Load drill files (Excellon format from Pcbnew)

sheetset_png

Set page size for printing and show/hide page limits

print_button_png

Open print dialog

zoom_in_png zoom_out_png

Zoom in and out

zoom_redraw_png

Refresh screen

zoom_fit_in_page_png

Zoom fit in page

gerbview_top_layer_png

Layer selection

gerbview_top_dcode_png

D Code selection (hight light items that use this dcode)

gerbview_top_info_png

Info about Gerber file options loaded in the current layer

Left toolbar

gerbview_left_toolbar_png

grid_png

Grid on / off

polar_coord_png

Display polar coordinates on / off

unit_inch_png unit_mm_png

Units selection to display coordinates

cursor_shape_png

On grid cursor shape selection

pad_sketch_png

Display mode selection (solid or outlines) for flashed items

track_sketch_png

Display mode selection (solid or outlines) for lines

opt_show_polygon_png

Display mode selection (solid or outlines) for polygons

gerbview_show_negative_objects_png

Show negative objects in ghost color

show_dcodenumber_png

Show / hide D Codes values (for items using a dcode)

gbr_select_mode0_png gbr_select_mode1_png gbr_select_mode2_png

Mode used by Gerbview to show layers.

Commands in menu bar

File menu

gerbview_file_menu_png

It is possible to load gerber and drill files into Gerbview. There is also an auxiliary option to export gerbers to pcbnew. Previously (a long time ago) it was also possible to load so called Dcodes, but those are now obsolete and is therefore not possible anymore.

Export to Pcbnew

GerbView has a limited capability to export Gerber files to Pcbnew.

The final result depends on what features of RS 274 X format are used in Gerber Files.

RS 274 X format has raster oriented features that cannot be converted (mainly all features relative to negative objects).

Flashed items are converted to vias.

Lines items are converted to track segments (or graphic lines for non copper layers)

So the usability of the converted file is very dependent upon the way each Gerber file was built by the original Pcb tool.

Preferences menu

gerbview_preferences_menu_png

Gives access to the hot keys editor, and some options to display items.

Miscellaneous menu

gerbview_misc_menu_png

  • List Dcodes shows the Dcodes in use and some of Dcode parameters.

  • Show Source displays the Gerber file contents of the active layer in a text editor.

  • Clear Layer erases the contents of the active layer.

Layer Manager

The layer manager has 2 purposes:

  • Select the active layer

  • Show/hide layers

gerbview_layer_manager_png

The active layer is drawn after the other layers.

When loading a new file, the active layer is used (the new data replace the previous data)

Note:

  • Mouse left click on a line: select the active layer

  • Mouse right click on the layer manager: show/hide all layers

  • Mouse middle click on a icon: select the layer color.

Modes to show Gerber layers

  • Raw mode gbr_select_mode0_png

Each gerber file and each item in files are drawn in the order files are loaded.

However the active layer is draw last.

When Gerber files have negative items (drawn in black) artefacts are visible on already drawn layers

gerbview_mode_raw_stack_png

  • Stacked mode gbr_select_mode1_png

Each gerber file is drawn in the order files are loaded.

The active layer is draw last.

When Gerber files have negative items (drawn in black) there are no artefacts on already drawn layers, because this mode draws each file in a local buffer before it is shown on screen. Negative items do not create artefacts.

gerbview_mode_raw_stack_png

  • Transparency mode gbr_select_mode2_png

gerbview_mode_transparency_png

Effect of layer selection for drawings

This effect is visible only in raw or stacked mode.

The layer 1 (green layer) is drawn after the layer 2

gerbview_layer_select_1_png

The layer 2 (blue layer) is drawn after the layer 1

gerbview_layer_select_2_png

To print layers, use the print_button_png tool, or the main menu (files)

But be sure items are inside the printable area (select by sheetset_png a suitable page format).

Do not forget photoplotters can use a large plottable area, much bigger than the page sizes used by printers)

Moving (by block move command) the entire layers is often needed.

Move block command

You can move items by selecting them (drag the mouse with left button down) and then moving the selected area on screen.

Click the left button to finally place the area you are moving.