Headings:

9 - Preparation of files for circuit fabrication

9.1 - Final preparations

9.2 - Final DRC test:

9.3 - Generating files for phototracing

9.3.1 - GERBER format:

9.3.2 - HPGL Format:

9.3.3 - POSTSCRIPT Format:

9.4 - Adjusting the clearance for the solder stop mask:

9.5 - Generating the drill file(s)

9.6 - Generating the cabling documentation:

9.7 - Generation of file(s) for automatic component insertion:

9.8 - Advanced tracing options:

Preparation of files for circuit fabrication

Note:

All of the files generated are placed in the working directory, i.e., in the same directory as the file xxxxxx.brd of the printed circuit board.

Final preparations

It is necessary to:

Indicate the layer (e.g., 'component' and 'copper') and project names by placing appropriate text upon each of the layers.

All text on the 'copper' (sometimes called 'solder' or 'bottom') side must be mirrored.

Create any (ground)planes, modifying traces as required to ensure they are contiguous.

Place alignment crosshairs and possibly the dimensions of the board outline (these are usually placed on one of the general purpose layers).

Here is an example showing all of these elements, except the ground planes, which have been omitted for better visibility:

A colour key for the 4 copper layers has also been included:

Final DRC test:

Before generating the output files, a global DRC is very strongly recommended.

Press the button to launch the DRC dialogue:

and then press .

This final check will prevent any unpleasant surprises...

Generating files for phototracing

This is done via the Files/Plot menu option.

Usually, the files are in the GERBER format. Nevertheless, it is possible to produce output in both HPGL and POSTSCRIPT formats.

GERBER format:

For each layer, Pcbnew generates a separate file following the GERBER 274X standard, by default in 3.4 format (each coordinate in the file is represented by 7 digits, of which 3 are before the decimal point and 4 follow it; the units are inches).

The tracing is always drawn to scale (scale = 1).

It is normally necessary to create files for all of the copper layers and, depending on the type of circuit, for the solder stop, solder mask, and silkscreen (component markings) layers. All of these files can be produced in one go, by selecting the appropriate checkboxes.

For example, for a double-sided circuit with solder stop, silkscreen and solder mask (for CMS components), 8 files would be generated ('xxxx' representes the name of the .brd file):

xxxx.copper.pho for the copper side.

xxxx.cmp.pho for the component side.

xxxx.silkscmp.pho for the component-side silkscreen markings.

xxxx.silkscu.pho for the copper-side silkscreen markings.

xxxx.soldpcmp.pho for the component-side solder mask.

xxxx.soldpcu.pho for the copper-side solder mask.

xxxx.maskcmp.pho for the component-side solder stop mask.

xxxx.maskcu.pho for the copper-side solder stop mask.

HPGL Format:

The standard extension for the output files is .plt.

The tracing can be done at user-selected scales and can be mirrored.

The Print Drill Opt list offers the option of pads that are filled, drilled to the correct diameter or drilled with a small hole (to guide hand drilling).

If the Print Sheet Ref option is active, the sheet cartridge is traced.

POSTSCRIPT Format:

The standard extension for the output files is .ps in the case of postscript output.

As for HPGL output, the tracing can be at user-selected scales and can be mirrored.

If the Org = Centre option is active, the origin for the coordinates of the tracing table is assumed to be in the centre of the drawing.

If the Print Sheet Ref option is active, the sheet cartridge is traced.

Adjusting the clearance for the solder stop mask:

The menu option for this is accessed via Dimensions/Tracks and Vias:

and entering the desired setting in the bottom-right option (Mask clearance); the default value is 0.01 inches.

Generating the drill file(s)

The creation of a drill file xxxxxx.drl following the EXCELLON standard is always necessary.

One can also produce an optional drill plan, which will be in HPGL (xxxxxx.plt) or POSTSCRIPT (xxxxxx.ps) format. However, this is only occasionally useful, as an additional check.

The generation of these files is controlled via the Postprocess/Create Drill file menu selection:

The default drill diameter for vias (For vias without a special drill value) should be defined here. For the HPGL tracing of the drill plan, it is possible to define the no. and speed of the pen used.

Coordinate origin:

The dialog box is:

Absolute: absolue coordinates are used

Auxiliary axis: coordinates are relative to the auxiliary axis (use the tool (right toolbar) to put it in good place.

Generating the cabling documentation:

To produce these files, the component and copper silkscreen layers can be traced. Usually, just the component-side silkscreen markings are sufficient for cabling a PCB. If the copper-side silkscreen is used, the text it contains should be mirrored in order to be readable.

Generation of file(s) for automatic component insertion:

This option is accessed via the Postprocess/Create Cmp file menu option. However, no file will be generated unless at lesat one module has the Normal+Insert attribute activated (see Editing Modules). One or two files will be produced, depending upon whether insertable components are present on one or both sides of the PCB. A dialogue box will display the names of the file(s) created.

Advanced tracing options:

The options described below (part of the Files/Plot dialogue) allow for fine-grained control of the tracing process. They are particularly useful when printing the silkscreen markings for cabling documentation.

The options are:

Print Sheet Ref	Trace sheet outline and the cartridge.
Print Pads on Silkscreen	Enables/disables printing of pad outlines on the silkecreen layers (if the pads have already been declared to appear on these layers). In fact useful for preventing any pads from being printed, in the disabled mode.
Always Print Pads	Forces tracing of all pads on ALL layers.
Print Module Value	Enables printing of VALUE text on the silkscreen.
Print Module Reference	Enables printing of the REFERENCE text on the silkscreen.
Print other module texts	Enables the printing of other text fields on the silkscreen.
Force Print Invisible Texts	Forces printing of fields (reference, value) declared as invisible. In combination with Print Module Reference and Print Module Value, this option enables production of documents for guiding cabling and repair. These options have proven necessary for circuits using components that are too small (CMS) to allow readable placement of two separate text fields.

Preparation of files for circuit fabrication	PCBNEW

Page 9 - 6

chap9: Génération des documents de réalisation

IUT

1996-01-27T12:47:00