The Layout Editor window opens when you open an existing board file or create a new board.
Descriptions of commands that cannot be reached through the command toolbar are also to be found in the section concerning the Schematic Editor window. All of the commands can also be reached through the pull-down menus in the menu bar. This also applies, of course, to the Schematic and Layout Editor windows.
Shows the properties of the selected object. Typing INFO IC1 in the command line results in the properties dialog of the object named IC1. Depending on the selected object some of the properties can be altered here.
Highlights the object to be selected with the mouse.
It's also possible to enter the object's name (even several names at once) in the command line. * and ? are allowed to be used as wildcards, as well.Ctrl + SHOW toggles the show state of the selected object.
Select and deselect the layers to be displayed. Components on the top side of the board can only be selected if the layer 23, OriginsTop, is displayed. The same applies to components on the bottom side of the board and layer 24, OriginsBottom.
See Appendix for the meaning of the layers.
The DISPLAY command supports so-called Layer Presets (Aliases). This allows you to name certain combinations of layers and use it as a parameter with the LAYER command. A quick change from one view to another layer combination is possible with this command.
Double-click one of the layer entries for changing its color or fill style.
DISPLAY LAST switches to the last displayed layer combination.
The DISPLAY menu shows only those layers defined in the Layer Setup of the Design Rules!
Further information about DISPLAY can be found in the help function.
The following mouse click defines the new origin for the coordinate display. Relative coordinates (R x-value y-value) and polar values (P radius angle) are shown in addition to absolute coordinates in the coordinate display box.
If you first click the MARK icon and then the traffic-light icon, only the absolute coordinate values will be displayed again.
Define a group which can then be moved, rotated, or copied with COPY and PASTE to another drawing or whose properties should be changed.
By default the GROUP command is always active. If you click into empty space of a drawing and hold the mouse button you can drag a rectangle or draw a polygon around the objects in the group. After defining the group you can immediately move it without having to select a command icon by clicking and holding the mouse button onto a groups’ object.
If the option GROUP command default on is not active or you want to execute another command with the group, define the group, select for example a command icon (for rotate, copy…..) and execute it on the group with Ctrl + right mouse-click.
GROUP ALL in the command line selects all objects.
To be sure that all objects are selected DISPLAY ALL layers before. On the other hand, deselecting specific layers can exclude certain objects from the selection.
Further information about GROUP can be found in the section about the Schematic Editor and in the help function.
Move any visible object. The right mouse button rotates the object.
The MOVE command cannot connect signals even if a wire (trace) is moved over another wire or a pad. Use ROUTE to route signals.
Keeping the Ctrl key pressed while selecting an object selects it in a particular manner. Please consult the help function for details (CRICLE, ARC, LINE, MOVE, ROUTE etc.).
For moving groups, please see MOVE in the Schematic Editor section.
Mirror objects. Components can be placed on the opposite side of the board by using the MIRROR command.
Rotate objects (also possible with MOVE). Keep the left mouse button pressed to rotate the selected object by moving the mouse. The parameter toolbar shows the current angle. This can be done with groups (GROUP and right mouse button) as well. ROTATE can be used with groups, as well. Activate ROTATE, press the Ctrl key and click with the right mouse button into the drawing to set the center of rotation. The group will be rotated counterclockwise by the given angle.Alternatively type in the angle in the Angle box or in the command line. Details about the syntax can be found in the help function.
The ALIGN command can be used to align selected objects in relation to each other or to move their origin location to the nearest grid point.
The following modes are supported:
Copy parts and other objects.
When copying objects, a new name will be assigned, but the value will be retained. When copying a single wire, the copy will have the same name.
Keep the Ctrl key pressed while clicking onto an object and the object will be grabbed at its origin. So it will be placed in the currently chosen grid.
COPY can be used with groups. The group will be put into the clipboard of the operating system. It is possible to copy it into another Electronics program, for example.
Insert objects from the paste buffer.
Use the menu Edit/Paste from... in order to paste a whole layout (and schematic, if available) into your current drawing. See help for further information.
Delete visible objects.
If a group has been defined, it can be deleted with the right mouse button while the Ctrl key is pressed.
DELETE SIGNALS in the command line erases all tracks and signals in the layout, provided there is no consistent schematic loaded. The DELETE command deletes an entire polygon when clicking on a polygon wire with the Shift key pressed. Keeping the Ctrl key pressed while clicking with the left mouse button on a wire bend will delete the bend. A new direct connection between the next bends will be drawn now.
If objects cannot be deleted, the reason can lie with error polygons related to the DRC command. They can be deleted with the ERRORS command (ERRORS CLEAR). If layer 23, OriginsTop, or 24, OriginsBottom, is not displayed, components cannot be deleted. CHANGE Change the properties of an object, for example the width of a wire or the size of a text. If the Esc key is pressed after changing a property, the previously used value menu will appear again. In this way a new value can be conveniently chosen. See also the help function.
Alternatively, object properties can be viewed and some of them even changed with the context menu's Properties entry. The context menu opens after a right mouse click onto the object.
Add a Design Block into the drawing. If the Design Block consists of board and schematic the Layout part can be placed with the mouse cursor. The Schematic part will be added automatically to the Schematic on new sheets accordingly.
Add library elements to the drawing. It offers a convenient search function for Packages here. USE specifies which libraries are available.
A right-click onto the ADD icon opens a popup menu that contains a list of recently placed Devices.
Swap two signals connected to equivalent pads of a component, provided the pins have been defined with the same Swaplevel. A pin that is connected to several pads can't be swapped.
Replace a component (or a Package, if there is no schematic) by another one from any library.
If you want to change the Package variant only and not the whole Device, use CHANGE PACKAGE or the PACKAGE command.
A right-click onto the REPLACE icon opens a popup menu that shows a list of recently replaced components.
Locks the position and orientation of a component on the board. If a component is locked, you can't move it or duplicate it with CUT and PASTE. Shift + LOCK unlocks the component. This is also possible with the unLock entry of the context menu.To be able to distinguish locked from unlocked components, the origin cross of a locked component is displayed like x instead of +.
The position of a locked component can be changed, however, by typing in new coordinate values in the properties dialog.
Give names to components, signals, vias, and polygon pours. With NAME it's possible to move a polygon pour from one signal to another.
Provide values for components. A resistor, for example, gets 100k as its value. A right-click onto this icon opens a list of already used values. Select an entry and apply it to one or more components by clicking onto them successively.
Separate name, value, and attribute (if any) texts from a Device, so that they can be placed individually. The size of detached (smashed) texts can also be individually changed. Also in combination with GROUP. If a group is defined, you can smash it with a right mouse click while the Ctrl key is pressed.
Use the DELETE command to hide smashed texts.
To unsmash texts, keep the Shift key pressed while using the SMASH command. The texts are not editable any more and appear at their original positions after a window refresh (also possible with unSmash in the context menu).
Alternatively you can switch on or off the option Smashed in the context menu's Properties entry.
Round off or bevel wire joints (also possible for polygon contours). The grade of mitering is determined by the miter radius. Positive sign results in a rounded joint, negative sign in a bevel.The miter radius influences some wire bend modes, too (see help function: SET, Wire_Bend).
Insert a bend into a wire.
If you want to change, for example, the layer for a section of an already routed track, you can insert two wire bends with the SPLIT command and change the layer of the newly created segment with the CHANGE LAYER. Electronics will set vias automatically at the position of the wire bends.
You can use the SPLIT command for a quick re-routing of an already existing track. Click onto the track to insert a wire bend. Now move the mouse and route it anew. To remove the previous track use the RIPUP command or DELETE in combination with the Ctrl key.
Joins wire segments in a signal layer which lie in one straight line.
Draw meanders to balance the length of signals, especially of differential pairs. Can be used for measuring the length of a signal, when pressing the Ctrl key.
The SLICE command cut lines in two parts. If it is a routed trace the gap contains an airwire that connects the two parts of the signal. So a signal is actually not cut into two different parts, but it rips up the trace according to the given width of the gap. Simply click left to start the cutting wire, a second click ends it. All objects crossing the cutting wire will be slices. Exception is a
polygon’s contour. SLICE can be used in the command line. The cutting line is defined by start and end coordinates, like SLICE (0.2 3) (0.5 4);
Route signals manually. Airwires are converted to wires.
By default the ROUTE command works in “Obstacle Avoidance” mode. So it automatically takes care on Design Rules and avoids obstacles that are along the path of a trace. If the routing mode is set to “Ignore Obstacle” mode by clicking on the icon in the parameter toolbar, the user takes responsibility for all the Design Rules.
ROUTE offers several options with the different mouse buttons, also in combination with the Ctrl and Shift key.
Ctrl + Left |
starts routing at any given point along a wire or via |
Shift + Left |
if the airwire begins at an already existing wire and this wire has a different width, the new wire adopts this width |
Center |
selects the layer |
Right |
changes the wire bend style |
Shift + Right |
reverses the direction of switching bend styles |
Ctrl + Right |
toggles between corresponding bend styles |
Shift + Left |
places a via at the end point of the wire |
Ctrl + Left |
defines arc radius when placing a wire's end point |
More information can be found in the help function of the ROUTE command. See also Group Default On.
Convert routed wires (tracks) into unrouted signals (airwires), and hide the fill polygon pours. Using signal names in the command line allows you to ripup only certain signals, to exclude particular signals, or to execute the command exclusively for polygon pours. More details can be found in the help function. Wires not connected to components must be erased with DELETE.
Draw lines and arcs. If used in the layers 1 through 16, the LINE command creates electrical connections.The Style parameter (CHANGE) determines the line type. The DRC and the Autorouter always treat a LINE as a continuous line, regardless of what Style is used. Clicking the right mouse button changes the wire bend (SET WIRE_BEND).
Please note the particularities in combination with the Ctrl and Shift key in the help function:If you press, for example, the Ctrl key while starting to draw a wire, the wire begins exactly at the end of an already existing wire nearby. Even if this wire is not in the currently set grid. Wire width, style and layer will be adopted from the already existing wire.
Placing text. Use CHANGE SIZE to alter the height of the text. If the text is using a vector font, CHANGE RATIO will alter the thickness. CHANGE TEXT is used to alter the text itself. CHANGE FONT alters the typeface. CHANGE ALIGN defines the alignment (the location of the origin) of the text.The option Always vector font (Options/User Interface) shows and prints all texts in vector font, regardless of which font is actually set for a particular text.
If you want to have inverted text in a copper layer, you have to enter the text in the layers 41, RestrictTop, or 42, RestrictBottom, and draw a copper plane in Top or Bottom layer around the text with the PPOUR command. The polygon pour keeps the restricted areas (which is the text) free from copper.
Use Shift+Enter in order to insert a line break for multi-line texts. The line distance can be set via the Properties window or in the parameter toolbar, as long as the text is not yet placed and still attached to the mouse cursor.
It is strongly recommended to write texts in copper layers as vector font! So you can be sure that the CAM Processor's output is identical with the text shown in the Layout Editor. See also help function.
Draw a circle. This command creates restricted areas for the Autorouter, if used in the layers 41, RestrictTop, 42, RestrictBottom, or 43, RestrictVias. Circles with wire width = 0 are drawn as filled.
Draw an arc (also possible with LINE).
CHANGE CAP FLAT | ROUND defines straight or rounded ends for arcs. If the arc is a part of a trace and both ends are connected to a wire, caps will be round.
Arcs with flat caps are emulated when generating manufacturing data in Gerber format with the CAM Processor. That means they will be drawn with small short straight lines. Arcs with round caps won't be emulated.
Draw a rectangle. This command creates restricted areas for the Autorouter, if used in the layers 41, RestrictTop, 42, RestrictBottom, or 43, RestrictVias.
Draw a solid or hatched polygon pour.
A polygon pour is a signal member polygon on a routing layer. It automatically fills its copper area by islolating from non-same-signal objects, and connecting to same-signal objects, according to DRC rules.
A polygon pour's definition contour is always displayed as a dotted line. In the case of a hatched polygon pour, its width and spacing define a mesh of lines, and implicitly control areas that can be filled using the specified line width. In the case of a solid polygon pour, its width is likewise used by the solid fill process as a minimum web width.
Draw a polygon cutout void that prevents polygon pours from filling an area with copper.
A polygon cutout is placed on a routing layer to define a fill void for all same-layer polygon pour objects that overlap it.
Draw a simple solid polygon shape.
A polygon shape is a non-signal solid shape. Its most common uses are to prevent the Autorouter from utilizing an area (RestrictTop, RestrictBottom, or RestrictVias layers), and to define annex pad/smd shapes for devices in the Footprint Editor.
Draw an appropriate polygon pour, polygon shape, or polygon cutout, according to the current editor context, parameter settings, and layer.
Place a plated-through hole. Vias are placed automatically if the layer is changed during the ROUTE command. You can assign a via to a signal with the NAME command by changing it's name to the name of the signal. Vias can have different shapes in the outer layers (round, square, octagon) , but are always round in inner layers.
Definition of a signal. This is not possible if the Forward&Back Annotation is active. In that case you have to define the connection with the NET command in the Schematic Editor.
Define a mounting hole (not plated-through).
Defines an attribute for a component. Through the menu Edit/Global attributes, you can define attributes that are valid for the whole layout.
Can be used to add dimensioning to the board. It can either be applied to an object or you can draw arbitrary dimensions. When you select an object Electronics selects a suitable dimensioning type (Dtype). If it is not the one needed, click the right mouse button to change it. If you want to start at any location in the drawing use Ctrl key + left mouse click. There are different dimensioning types: Parallel, Horizontal, Vertical, Radius, Diameter, Angle, and Leader.
Configuration of dimensioning lines, text size units and so on can be done in the objects' properties dialog or with the CHANGE command, which can be executed for groups of objects, as well:
| CHANGE Dtype | changes the dimensioning type |
| CHANGE Dunit | decides about the measurement unit, the precision, and about showing or hiding the unit. |
| CHANGE Dline | determines the width of the measurement line, the width of the extension line, the Extension length after the dimension arrow head, the distance from the object measured (Extension, offset). |
Calculate the shortest airwires possible and recalculate and show the fill of polygon pours.
Use the RATSNEST command with a signal name in order to calculate and display or hide a certain airwire. A preceding exclamation mark hides the airwires of the given signal name. More information can be found in the help function.
The polygon pour calculation can be deactivated with the SET command. Either through the menu Options/Set/Misc or by typing in the command line: SET POLYGON_RATSNEST ON | OFF or in short: SET POLY ON | OFF.
RATSNEST will be executed automatically for the selected signal while drawing a wire with ROUTE.
While RATSNEST is active the status bar of the Layout Editor displays the name of the currently calculated signal.
Start the Autorouter.
If you type AUTO FOLLOWME in the command line, the Autorouter Setup window opens in the follow-me mode, which allows to set the parameters for the follow-me router only.
Start the BGA Autorouter.
If you type AUTO BGA or click this icon, EAGLEs start a special Autorouter in order to route signals connected to BGA components out of the BGA area. In a first step you select the BGA component(s) in the layout. Second, you select the signals that shall be routed. You can also decide about the layer assignment for the signals. Micro Vias are supported, if this option is enabled. Please verify Design Rules before starting the BGA router!
Perform a consistency check for schematic and board.
Define Design Rules and perform Design Rule Check.
Typing DRC * into the command line opens the Design Rules window where you can check and adjust your settings and close the dialog window again without starting the Design Rule Check.
Show errors found by the DRC. If you haven't already processed a Design Rule Check for the board, it will be done automatically before showing the error list, if there are any errors found.
More commands are available for the Layout Editor, as they are in the Schematic, that are not available in the Command Menu. Most of them are valid in both Schematic and Layout.