DELETE | DESCRIPTION | DIMENSION | DISPLAY | DRC | DSOURCESETUP
Function
Deletes objects.
Syntax
DELETE ..
DELETE name ..
DELETE SIGNALS
Mouse keys
Shift+Left deletes higher-level object.
Ctrl+Left deletes a wire joint or a port.
Ctrl+Right deletes the group.
Use DELETE to delete a selected object.
Parts, pads, smds, pins and gates can also be selected by their name, which is especially useful if the object is outside the currently shown window area. Note that when selecting a multi-gate part in a schematic by name, you will need to enter the full instance name, consisting of part and gate name.
Attributes of parts can be selected by entering the concatenation of part name and attribute name, as in R5>VALUE.
Right-click the mouse to delete a previously defined GROUP.
After deleting a group it is possible that airwires which have been newly created due to the removal of a component may be "left over", because they have not been part of the original group. In such a case you should recalculate the airwires with the RATSNEST command.
With active Forward&Back Annotation, no wires or vias can be deleted from a signal that is connected to components in a board. Also, no components can be deleted that have signals connected to them. Modifications like these have to be done in the schematic. In this scenario, the DELETE command behaves like the normal mode of the RIPUP command, converting wires and vias back to airwires.
Use the RIPUP command to convert an already routed connection back into an airwire.
The DELETE command has no effect on layers that are not visible (refer to DISPLAY).
The DRC might generate error polygons which can only be deleted with DRC CLEAR.
If Ctrl-DELETE is applied to the joining point of two wires, these wires are combined to form one straight wire. For this to work the two wires must be in the same layer and have the same width and line style, and must both have round endings (in case of arcs).
The DELETE command deletes one corner at a time from a polygon. The whole polygon is deleted if there are only three corners left.
Components can be deleted only if the OriginsTop layer (or OriginsBottom with mirrored components) is visible and if (with active Forward&Back Annotation) no signals are connected to the component (see also REPLACE). Note that an element can appear to be not connected (no airwires or wires leading to any of it's pads), while in fact it is connected to a supply voltage through an implicit power pin. In such a case, you can only delete the corresponding part in the schematic.
The following rules apply:
If the last supply symbol of a given type is deleted from a net segment that has the same name as the deleted supply pin, that segment is given a newly generated name (if there are no other supply symbols still attached to that segment) or the name of one of the remaining supply symbols.
If you select wires (tracks) or vias belonging to a signal with the DELETE command, three cases have to be considered:
After wires or vias have been deleted from a signal which contains polygons, all polygons belong to the signal keeping the original name (usually the bigger part).
DELETE SIGNALS can be used to delete all signals on a board. This is useful if you want to read in a new or changed netlist (see EXPORT). Only those signals are deleted which are connected to pads.
If you want to delete a part that has the name SIGNALS, you need to write the name in single quotes.
If the Shift key is pressed when clicking on an object, the object that is hierarchically above the selected one will be deleted. This applies to the following objects:
| Gate | Deletes the entire part containing this gate (even if the gates are spread over several sheets). If f/b annotation is active, the wires connected to the element in the board will not be ripped up (as opposed to deleting a single gate), except for those cases where a pin of the deleted part is only connected directly to one single other pin and no net wire | |
| Polygon Wire | Deletes the entire polygon | |
| Net/Bus Wire | Deletes the entire net or bus segment |
Don't forget: Deleting can be reversed by the UNDO command!
You can delete objects selected in the current group by pressing the delete key with the Group Default On options enabled.
Function
Defines the description of a drawing or a library object.
Syntax
DESCRIPTION [ * ] [ description_string; ]
DESCRIPTION ** [ description_string; ]
See also CONNECT, PACKAGE, VALUE.
DESCRIPTION is used to define or edit the description of a drawing or a library object.
The description_string may contain HTML tags.
The first non-blank line of description_string will be used as a short descriptive text (headline) in the Control Panel.
The DESCRIPTION command without a parameter opens a dialog in which the text can be edited. The upper pane of this dialog shows the formatted text, in case it contains HTML tags, while the lower pane is used to edit the raw text. At the very top of the dialog the headline is displayed as it would result from the first non-blank line of the description. The headline is stripped of any HTML tags.
By default the DESCRIPTION command works on the description of the object that is currently edited, like a device set, footprint, symbol, board, or sheet. If, in a library, there is no currently edited object (as can be the case after it has been newly loaded) the description of the library will be changed.
To explicitly access the description of a library, even if a device, footprint, or symbol is already being edited, enter the asterisk character ('*') as the first parameter to the DESCRIPTION command. This is also the way to access the description of a schematic, as opposed to the description of an individual sheet.
To access the description of the current MODULE, enter a pair of asterisk characters ('**') as the first parameter to the DESCRIPTION command.
DESCRIPTION 'Quad NAND\nFour NAND gates with 2 inputs each.';
This would result inQuad NAND
Four NAND gates with 2 inputs each.
Function
Adds dimensioning to a drawing.
Syntax
DIMENSION [dtype] ..
Mouse keys
Center selects the layer.
Right changes the dtype.
Shift+Right reverses the direction of changing the dtype.
Ctrl+Left when starting/ending a dimension does not select an object.
See also LINE, CHANGE, CIRCLE, HOLE.
DIMENSION adds dimensioning to a drawing. It can either be applied to an object, or it can draw arbitrary dimensions.
If the first point selects an object, a suitable dimension object is generated as follows:
| straight wire | linear dimension displaying the distance between the end points of the wire | |
| curved wire | radius dimension displaying the radius of the arc | |
| circle | diameter dimension displaying the diameter of the circle | |
| hole | diameter dimension displaying the diameter of the hole |
If no object is selected, or a wire is selected at one of its end points, a dimension object is generated according to the current dimension type. If this dimension type is not the one that is needed, the right mouse button can be clicked to loop through the various types.
To draw an arbitrary dimension even at close proximity to an object that would trigger a specific kind of dimension, press the Ctrl key with the first click. This may also be useful when using the DIMENSION command in a script (by adding the 'C' modifier to the first coordinate), to make sure the dimension appears exactly as intended.
The way in which a dimension object is drawn (line, unit, precision) can be configured with "CHANGE DLINE/DUNIT" or with its properties dialog. Note that the "Unit" parameter in this dialog refers to the unit in which the actual numbers of the dimension object will be displayed.
Every dimension object has three coordinates that define its reference points and an alignment point. How these coordinates are actually interpreted to display a dimension object depends on the dtype property.
Parallel
A parallel dimension displays the distance between its first and second reference point. The dimension line is parallel to the line going through its reference points, and it runs through the given alignment point. The actual position of the alignment point doesn't matter, only its distance from the the line through its reference points is taken into account. When a parallel dimension object is newly created or modified, the alignment point is normalized, so that it lies in the middle of the dimension line.
Horizontal
Same as parallel, but the dimension line extends only in X direction, and it displays only the X distance between the reference points.
Vertical
Like horizontal, but for Y.
Radius
A radius dimension displays the distance between its first and second reference point. The first reference point is at the center of the arc this dimension is drawn for, while the second point is somewhere on the arc itself. If the alignment point is between the two reference points, the dimension line is drawn between the reference points, which is "inside" the arc. Otherwise the dimension line is drawn "outside" of the arc. If the measurement text is too long to fit on an inside radius dimension, the dimension line is drawn on the outside. A radius dimension automatically displays a cross at its first reference point (which is the center of the arc). When a radius dimension object is newly created or modified, the alignment point is normalized, so that it lies in the middle of the dimension line for an "inside" dimension, or just beyond the arrow for an "outside" dimension.
Diameter
A diameter dimension displays the distance between its first and second reference point. The two reference points are on opposite sides of the circle's circumference, so their distance measures the circle's diameter. If the alignment point is between the two reference points, the dimension line is drawn between the reference points, which is "inside" the circle. Otherwise the dimension line is drawn "outside" of the circle, much like a parallel dimension. If the measurement text is too long to fit on an inside diameter dimension, the dimension line is drawn on the outside. A diameter dimension automatically displays a cross in the middle between its two reference points (which is the center of the circle). When a diameter dimension object is newly created or modified, the alignment point is normalized, so that it lies at the same coordinates as its second reference point for an "inside" dimension, or in the middle of the dimension line for an "outside" dimension.
Angle
An angle dimension displays the angle between the second and third reference point, measured counterclockwise around the first reference point (which is the center of the arc). When an angle dimension object is newly created or modified, the second reference point is normalized, so that it has the same distance from the first point as the third one does.
Leader
A leader dimension can be used to point at something in a drawing. There is an arrow at the first point, and the second and third point define a (bent) line. The leader doesn't display any measurement. You can use the TEXT command to place any text you need.
A dimension object can be selected at any of its three points.
Function
Selects the visible layers.
Syntax
DISPLAY
DISPLAY [option] layer_number..
DISPLAY [option] layer_name..
Valid options are: ALL, NONE, LAST, ? and ??
DISPLAY is used to choose the visible layers. As parameters, the layer number and the layer name are allowed (even mixed). If the parameter ALL is chosen, all layers become visible. If the parameter NONE is used, all layers are switched off. For example:
DISPLAY NONE BOTTOM;
Following this command only the Bottom layer is displayed. If the parameter LAST is given, the previously visible layers will be displayed.
Note that only those signal layers (1 through 16) are available that have been entered into the layer setup in the Design Rules.
If the layer name or the layer number includes a negative sign, it will be filtered out. For example:
DISPLAY TOP -BOTTOM -3;
In this case, the Top layer is displayed while the Bottom layer and the layer with the number 3 are not shown on the screen. Avoid layer names ALL and NONE as well as names starting with a "-", as well as the names of layer presets and aliases.
Some commands (PAD, SMD, SIGNAL, ROUTE) automatically activate certain layers.
If the DISPLAY command is invoked without parameters, a dialog is presented which allows you to adjust all layer settings.
The options '?' and '??' can be used to control what happens if an undefined layer is given in a DISPLAY command. Any undefined layers following a '?' will cause a warning and the user can either accept it or cancel the entire DISPLAY command. Undefined layers following a '??' will be silently ignored. This is most useful for writing script files that shall be able to handle any drawing, even if a particular drawing doesn't contain some of the listed layers.
DISPLAY TOP BOTTOM ? MYLAYER1 MYLAYER2 ?? OTHER WHATEVER
In the above example, the two layers TOP and BOTTOM are required and will cause an error if either of them is missing. MYLAYER1 and MYLAYER2 will just be reported if missing, allowing the user to cancel the operation, and OTHER and WHATEVER will be displayed if they are there, otherwise they will be ignored. The '?' and '??' options may appear any number of times and in any sequence.
If pads or vias have different shapes on different layers, the shapes of the currently visible (activated with DISPLAY) signal layers are displayed on top of each other. If the color selected for layer 17 (Pads) or 18 (Vias) is 0 (which represents the current background color), the pads and vias are displayed in the color and fill style of the respective signal layers. If no signal layer is visible, pads and vias are not displayed.
If the color selected for layer 17 (Pads) or 18 (Vias) is not the background color and no signal layers are visible, pads and vias are displayed in the shape of the uppermost and undermost layer.
This also applies to printouts made with PRINT.
If you want to select certain objects or elements (for example with MOVE or DELETE) the corresponding layer must be visible. Elements can only be selected if the OriginsTop (or OriginsBottom with mirrored elements) layer is visible!
Parameter aliases can be used to define certain parameter settings to the DISPLAY command, which can later be referenced by a given name. The aliases can also be accessed by clicking the DISPLAY button and holding the mouse button pressed until the list pops up. A right click on the button also pops up the list. The syntax to handle these aliases is:
DISPLAY = name parameters
Defines the alias with the given name to expand to the given parameters. The name may consist of any number of letters, digits and underlines, and is treated not case-sensitive. It must begin with a letter or underline and may not be one of the option keywords.
DISPLAY = name @
Defines the alias with the given name to expand to the current parameter settings of the command.
DISPLAY = ?
Asks the user to enter a name for defining an alias for the current parameter settings of the command.
DISPLAY = name
Opens the DISPLAY dialog and allows the user to select a set of layers that will be defined as an alias under the given name.
DISPLAY = name;
Deletes the alias with the given name.
DISPLAY name
Expands the alias with the given name and executes the DISPLAY command with the resulting set of parameters. The name may be abbreviated and there may be other parameters before and after the alias (even other aliases). Note that in case name is an abbreviation, aliases have precedence over other parameter names of the command.
Example:DISPLAY = MyLayers None Top Bottom Pads Vias Unrouted
Defines the alias "MyLayers" which, when used as in
DISPLAY myl
will display just the layers Top, Bottom, Pads, Vias, and Unrouted (without the "None" parameter the given layers would be displayed in addition to the currently visible layers). Note the abbreviated use of the alias and the case insensitivity.
Function
Checks design rules.
Syntax
DRC
DRC ;
DRC LOAD|MERGE|SAVE filename;
DRC *
See also CLASS, SET, ERC, ERRORS.
The command DRC checks a board against the current set of Design Rules.
Note that electrically irrelevant objects (wires in footprints, rectangles, circles and texts) are not checked against each other for clearance errors.
The errors found are displayed as error polygons in the respective layers, and can be browsed through with the ERRORS command.
If no parameters have been entered, the DRC command opens a Design Rules dialog in which the board's Design Rules can be defined, and from which the actual check can be started.
If two coordinates are given in the DRC command (or if the Select button is clicked in the Design Rules dialog) all checks will be performed solely in the defined rectangle. Only errors that occur (at least partly) in this area will be reported.
If you get DRC errors that don't go away, even after modifying the Design Rules, make sure you check the Net class of the reported object to see whether the error is caused by a specific parameter of that class.
To delete all error polygons use the command
ERRORS CLEAR
The LOAD and SAVE options can be used to load the Design Rules from or save them to the given file. If filename doesn't have the extension ".dru" it will be appended automatically. The MERGE option can be used to merge some additional Design Rules parameters (the others remain unchanged).
If the DRC command is given an asterisk character ('*') as the first parameter, the Design Rules dialog will be opened and allow editing the Design Rules, without triggering an actual check when the dialog is confirmed.
With Live DRC enabled, the design rules are checked while editing.
The SET command can be used to change the behavior of the DRC command:
SET DRC_FILL fill_name;
Defines the fill style used for the DRC error polygons. Default is LtSlash.
SET LIVE_DRC ON | OFF;
Enables/Disables design rule checking of the design while editing.
Function
Used to setup a digital stimulation source for a simulation-compatible digital source part.
Syntax
DSOURCESETUP name
See also SIM, ADDMODEL, SOURCESETUP
Used to set up a "digital source" part to provide input signal stimuli for digital circuit simulations. Data can be entered in a table manually, or loaded from a .csv file. EAGLE provides 1, 4, and 8-output digital source parts ready to use in the ngspice-digital library for your convenience and the DSOURCESETUP command is used to configure it.
After you place a digital source part, connect all the part pins to nets, then run DSOURCESETUP and click the part (or alternatively, right-click on the part and choose Digital Source Setup), to configure it. You will be presented with a table-based interface, with one column for time, and one column for each output of the device. Data is entered into the table so that each row has a time value (that is, 0.010s, or 10m, or 10ms, or 10e-3), then a series of digital values (0 or 1) for each output of the device. The table below gives an example of the data that could be entered for a 4-output digital source.
TIME OUT1 OUT2 OUT3 OUT4 0 0 0 0 0 10ms 1 0 1 0 15ms 0 1 1 1
The digital values can be entered simply as 0 or 1 or U (for unknown state), or also optionally ending with a signal strength/type indicator suffix character which is one of s, r, z, or u (these stand for strong, resistive, hi-impedance, and undetermined). The full list of possible values is:
0s, 1s, Us, 0r, 1r, Ur, 0z, 1z, Uz, 0u, 1u, Uu
If you want to convert an arbitrary device to work as a digital source, you need to map it to a subcircuit SPICE model that contains the d_source digital model inside it. The DRIVERD1, DRIVERD4, and DRIVERD8 models are provided in the example models directory for you and provide a template for how to use the d_source ngspice model. The model can be adjusted to include any number of outputs. Consult the ngspice manual for more detail on the d_source model.
Consult the ngspice manual included in the EAGLE install directory for more details on digital source parts.