Heading:

8 - Routing PCBs

8.1 - Choosing routing parameters and routing a PCB

8.2 - Typical dimensions for different PCB classes

8.2.1 - Track width

8.2.2 - Insulation (clearance)

8.3 - Some typical combinations

8.3.1 - 'Rustic'

8.3.2 - 'Standard'

8.4 - Manual routing

8.5 - Creating the copper zones

8.5.1 - Net selection:

8.5.2 - Creating a zone:

8.5.2.1 - Creating the zone limits:

8.5.2.2 - Filling the zone:

8.5.3 - Fill Options:

8.5.3.1 - Working grid for filling.

8.5.3.2 - Clearance

8.5.3.3 - Pad options

Routing PCBs

Choosing routing parameters and routing a PCB

The choice is made in the menu: Dimensions ->Tracks and Vias.

The dimensions are given in inches or mm, depending upon the active units.

Reminder: 2.54 cm = 1 inch (or " ) = 1000 mils = 10000 tenths of mils.

Typical dimensions for different PCB classes

Track width

Use the largest possible value and conform to the minimum sizes given here:

Units	CLASS 1	CLASS 2	CLASS 3	CLASS 4	CLASS 5
mm	0,8	0,5	0,4	0,25	0,15
1/10mils	310	200	160	100	60

Insulation (clearance)

Unité	CLASS 1	CLASS 2	CLASSE3	CLASS 4	CLASS 5
mm	0,70	0,5	0,35	0,23	0,20
1/10mils	270	200	140	90	80

Usually, the minimum clearance is very similar to the minimum track width.

Some typical combinations

'Rustic'

Clearance: 0.35mm (0.0138 inches).

Track width: 0.8mm (0.0315 inches).

Pad diameter for ICs and vias: 1.91mm (0.0750 inches ).

Pad diameter for discrete components: 2.54mm (0.1 inches).

Ground track width: 2.54mm (0.1 inches).

'Standard'

Clearance: 0.35mm (0.0138 inches).

Track width: 0.5mm (0.0127 inches).

Pad diameter for ICs: make them elongated in order to allow tracks to pass between IC pads and yet have the pads offer a sufficient adhesive surface (1.27 x 2.54 mm -->0.05x 0.1 inches).

Vias : 1.27mm (0.0500 inches).

Manual routing

Manual routing is recommended, because it is the only method offering control of routing priorities. For example, is is preferable to start by routing power tracks, making them wide and short and keeping analog and digital supplies well separated. Then sensitive signal tracks should be routed. Amongst other problems, automatic routing often requires many vias. However, automatic routing can offer useful insight into the positioning of modules. With experience, you will probably find that the automatic router is useful for quickly routing the 'obvious' tracks, but the remaining tracks will best be routed by hand.

Creating the copper zones

Copper zones must be created when all the routing is finished.

After a route modification, zones must be deleted and recreated.

Pads of the net must be already connected by standard tracks. Do not expect connecting pads through the zone.

This is because:

All board caracteristics (pads, board edges) must be known.

D.R.C. does not test zones (because of time computation problems).

Copper zones (Usually ground and power planes) are usually attached to a net.

In order to create a copper zone one must:

Sélect the net (Hightlight this net), to attach the zone to this net.

Create the zone limit (If no, All the board will be filled.)

Fill the zone from a starting point.

A zone is always created allof a piece, to insure there is not any unconnected copper block.

Net selection:

Use the tool , and click on a pad connected to the net, which must be highligted.

Creating a zone:

Creating the zone limits:

Use the tool .

Choose the layer for the zone.

Draw the zone limit, on this layer.

This zone limit is a polygon, created by a click (left button) for each corner.

A double click ends the polygon.

The polygon will be automaticaly closed. If the starting point and the ending point are not at the same coordinate, pcbnew will add a segment from the end point to the start point.

Here is a zone limit created (polygon in thin line):

Filling the zone:

Tje filling zone is initiated from a starting point (Mouse cursor).

In order to do it, when the edge zone is finished, put the mouse cursor on a starting point for the filling. This point can be inside or outside the polygon, and on a free spot.

Click the right mouse button. This menu will be showed:

Activate the "Fill" button

Here is the filling result for a starting point inside the polygon:

Here is the filling result for a starting point outside the polygon:

The polygon is a frontier for filling.

Note:

you can use many polygons to create a complex limit. Here is an example:

Here is the filling result for a starting point inside the large polygon and outside the small polygon:

Fill Options:

One must choose:

The working grid for filling.

The clearance.

How the pads are drawn inside the zone (or connected to this zone).

Working grid for filling.

The smaller the filling grid is, the better the filling is.

However, the filling is made with horizontal and vertical track segments, if the grid is small, board files can be very larges (several Mo.).

A 0.01 inch grid is a good compromise.

Clearance

A good choice is a grid a bit bigger than the routing grid.

Pad options

Pads of the net can either be included or excluded from the zone, or connected by thermal reliefs.

If included, soldering and unsoldering can be very difficult.

If excluded, the connection to the zone is not very good.

A thermal relief is a good compromise.

Here is the result for the 3 options:

	Include Pads
	Exclude Pads
	Thermal relief. Pad is connected by 4 track segments. The segment width is the current value used for the track width.

PCBNEW: Routing PCBs

Page 8 - 8

IUT

1996-01-27T12:47:00

jean-pierre Charras

jean-pierre Charras