The following sections of this topic discuss additional layout practices, many of which involve using commands on the command line.

Without the schematic (not recommended)

INSPECTOR shows detailed information about the selected object. Depending on the object you clicked on, some of its properties can be altered in the dialog.

Exchanging footprints

If, as the layout is developed, you want to replace the selected footprint variant with a different one, then you can use either the PACKAGE or the REPLACE command, depending on the situation.

PACKAGE command

It is assumed that the layout and the schematic diagram are consistent and the device has been defined with more than one footprint variant.

Type in the command line PACKAGE and click onto the footprint to be replaced or alternatively click onto the footprint with the right mouse button and select the footprint entry from the context menu. A third variant would be to click onto the CHANGE icon and select the footprint option. Now you select the desired footprint, and confirm it with OK, in the dialog that then appears.

If the Show all Attribute Sets option is active, the footprint versions for all the attribute sets available for this device are displayed. If this option is not active you will only see footprints that are defined in the selected attribute set.

The footprint can also be exchanged from within the schematic diagram.

Devices that don't have alternative footprint variants defined, can be modified in the Library Editor. Add further footprint variants as needed and update your drawing with the new library definition.

If you change the footprint variant of a device which you gave a new value with the help of the VALUE command, although it has been defined with VALUE Off, the value will remain unchanged. See also page 103.

If you would like to change the footprint variant for several identical parts, you can do this in the command line. Define a GROUP with all parts that shall get a new footprint variant, first. Now type in the command line

CHANGE PACKAGE 'new-device-name'

and click with Ctrl + right mouse button into the drawing. The name of the new footprint variant has to be enclosed in inverted commas.

REPLACE command

Consistent schematic/layout pair

The REPLACE command allows you to substitute one component with another. The well-known ADD dialog window opens where you can select the new part. Now click onto the part you want to have replaced in the schematic or layout. The old and new device must be compatible, which means that their used gates and connected pins/pads must match, either by their names or their coordinates. Otherwise the substitution is not possible.

Layout without schematic

If you have a layout without an associated schematic diagram, you exchange the footprint with the aid of the REPLACE command. REPLACE opens the window that is familiar from the ADD dialog, in which it is possible to search for devices. When the footprint has been chosen you click on the part that is to be replaced in the layout.

The REPLACE command operates in the Layout Editor in two ways: chosen in the Parameter toolbar or with the SET command: The first mode permits footprints whose pad or SMD names are identical to be exchanged. The connecting areas can have any position. The second mode (replace_same coords) requires that pads or SMDs in the new footprint are located at the same coordinates (relative to the origin). The names may differ.

The text for the name and value of a device is only exchanged if they have not been separated from the device with SMASH.

The new footprint can come from a different library, and can contain additional pads and SMDs. Connections on the old footprint that were connected to signals must exist correspondingly in the new footprint. The new footprint can even have fewer connections, provided that this condition is satisfied.

Changing the attribute set

It is possible to change the attribute set of a device in the layout at any time, provided there are various attribute sets defined in the component. Use the CHANGE command with the Attribute Set option or the Attribute command of the context menu (available by clicking onto the footprint with the right mouse button). This procedure is identical to the one described before in which footprint forms are exchanged using PACKAGE.

Define forbidden areas

Areas in the form of rectangles, polygons or circles in layers 41, tRestrict, and 42, RestrictBottom, are forbidden for the Autorouter. No copper objects may be drawn in the top or bottom layers inside these areas. These regions are tested by the Design Rule Check and taken into consideration by the Autorouter.

Layer 43, RestrictVias, is for drawing restricted areas where the Autorouter may not set vias. Manually placed vias in such a RestrictVias region are not examined by the DRC and therefore not reported as an error.

Routing – placing tracks manually

The ROUTE command allows the airwires to be converted into tracks.

ROUTE offers two different modes: Walkaround obstacles (default)

Width

Line thickness with which the polygon is drawn. Select the largest possible width. This avoids unnecessary quantities of data when the board is sent for manufacture. If the wire width is lower than the resolution of the output driver in the CAM Processor, a warning is issued. A finer line width permits the polygon to have a more complex shape.

Pour

Specifies the filling type: the whole area (Solid) or a grid (Hatch). The special type Cutout can be used to define polygons that get subtracted from all other signal polygons within the same layer. Suitable for cut-outs (restricted areas) in polygons in inner signal layers.

Rank

Overlapping polygons must not create any short-circuits. Rank can therefore be used to determine which polygons are to be subtracted from others. A polygon with rank = 1 has the highest priority in the Layout Editor; no other polygon drawn in the layout is ever subtracted from it, while one with rank = 6 has the lowest priority. As soon as there is an overlap with a higher rank, the appropriate area is cut out from the polygon with rank = 6. Polygons with the same rank are compared by the DRC. The rank property works only for polygons with different signals. For overlapping polygons with the same signal name it is without effect. They will be drawn one over the other. Polygons that are created in the Package Editor and not assigned to a signal, will be subtracted from all other polygons. There is no rank parameter available.

Spacing

If the option Hatch is chosen for Pour, this value determines the spacing of the grid lines.

Isolate

Defines the value that the polygon must maintain with respect to all other copper objects not part of its signal and objects in BoardOutline, tRestrict or RestrictBottom layer. If higher values are defined for special signals in the Design Rules or net classes, the higher values apply.

In the case of polygons with different Ranks, Isolate always refers to the drawn contour which is shown in the outline mode of the polygon, even if the calculated polygon has got another contour, for example, due to a wire that supersedes the polygon. The actual clearance can become greater than the given Isolate value.

Thermals

Determines whether pads in the polygon are connected via Thermal symbols, or are completely connected to the copper plane. This also applies to vias, assuming that the option has been activated in the Design Rules.

The width of the thermal connectors is calculated as the half of the pad's drill diameter. The width has to be in the limits of a minimum of the wire width and a maximum of twice the wire width of the polygon.

The length of the thermal connectors is defined by the Thermal isolation value in the Design Rules' Supply tab.

Orphans

Determines if a polygon may contain areas (islands) that are not electrically connected to the polygon's signal. If Orphans is set Off such disconnected areas won't be drawn.