VALUE | VARIANT | VIA | VPPROBE | VPROBE
Function
Displays and changes values.
Syntax
VALUE ..
VALUE value ..
VALUE name value ..
VALUE ON;
VALUE OFF;
See also NAME, REPOSITION, VARIANT.
Elements can be assigned a value, for example '1k' for a resistor or '10uF' for a capacitor. This is done with the VALUE command. The command selects an element and opens a popup menu that allows you to enter or to change a value. If you type in a value before you select an element, then all of the subsequently selected elements receive this value. This is very useful if you want, for instance, a number of resistors to have the same value.
If the parameters name and value are specified, the element name gets the specified value.
The VALUE command can only be used in the default assembly variant. If you want to change the value of another assembly variant, you need to use the VARIANT command.
VALUE R1 10k R2 100k
In this case more than one element has been assigned a value. This possibility can be used in script files:
VALUE R1 10k \
R2 100k \
R3 5.6k \
C1 10uF \
C2 22nF \
...
The '\' prevents the following line from being mistaken for an EAGLE key word.
If the VALUE command is used in the device edit mode, the parameters ON and OFF may be used:On: Permits the actual value to be changed in the schematic.
Off: Automatically enters the actual device name into the schematic (for example 74LS00N). The user can only modify this value after a confirmation.
Function
Manages assembly variants.
Syntax
VARIANT
VARIANT name part_name [NO]POPULATE [ value [ technology ] ];
VARIANT [ + | - ] name;
See also VALUE, TECHNOLOGY.
By default all parts of the schematic are populated on the board (provided they have a package). However, sometimes different variants of a design may require that some parts are not populated, or that they have different values or technologies than the default. The VARIANT command allows you to define which parts are actually populated in a given assembly variant, and to give them particular values and technologies.
name is the name of the variant. It is treated not case-sensitive and must be enclosed in single quotes if it contains blanks or '+' or '-'.
If part_name followed by the keyword POPULATE or NOPOPULATE is given, a variant of the given name is created for that part, in which it will be marked as either "populated" or "not populated".
Parts that are not populated in the current assembly variant are indicated with an X drawn over their entire bounding rectangle in the schematic. In the board anything that is related to actually placing the part on the board (like placeplan, names, values etc.) is not drawn in such a case.
The optional value and technology (which is only applicable in a schematic) can be used to further refine the variant. A value may only be given if the part's device set has its "user value" parameter enabled. If only the technology shall be specified without using a different value, an empty string ('') can be entered for the value.
A new variant can be created by preceding name with a '+'. If a variant with that name already exists, nothing happens.
If the variant name is preceded with a '-', the given variant will be deleted. If name is '*', all variants will be deleted. Unless this command is used in a script, a confirmation prompt will ask the user whether this action should really be taken.
Giving only a variant name will switch the whole project to that variant. This means that all "populate" flags, values, and technologies will appear as specified in that variant for each part. Using an empty string ('') here switches to the default assembly variant, which is the same as if there were no variants at all. Note that when loading a drawing it is always in its default state, with no assembly variant selected.
If used without any parameters, a dialog will open that allows you to manage all assembly variants.
The name of the current assembly variant can be displayed by using the text variable >ASSEMBLY_VARIANT.
The commands ADD, CHANGE PACKAGE | TECHNOLOGY, REPLACE, UPDATE, and VALUE can only be used if no assembly variant is active.
The COPY command doesn't copy assembly variants.
In the board the VARIANT command is not supported, everything is controlled from schematic if f/b annotation is active (the variant combobox in the board editor is only for informational reasons). However, for standalone boards it's possible to set the populate option of elements with the CHANGE command or in the properties dialog.
Assembly variants can also be created for a module. A specific assembly variant of the module can be selected in each module instance that refers to it. The assembly variants of the schematic and assembly variants of modules are completely independent. The VARIANT command is not intended to switch assembly variants of a module.
Therefore for more clarity we distinguish between Module Assembly Variants and Main Assembly Variants. Within a module the VARIANT command refers to its module assembly variants, on the schematic's main sheets it refers to the main assembly variants.
Function
Adds vias to a board.
Syntax
VIA ['signal_name'] [diameter] [shape] [layers] [flags] ..
See also SMD, CHANGE, DISPLAY, SET, PAD, Design Rules.
When the VIA command is active, a via symbol is attached to the cursor. Pressing the left mouse button places a via at the current position. The via is added to a signal if it is placed on an existing signal wire. If you try to connect different signals, Electronics will ask you if you really want to connect them.
The signal_name parameter is intended mainly to be used in script files that read in generated data. If a signal_name is given, all subsequent vias will be added to that signal, and no automatic checks will be performed.
This feature should be used with great care because it could result in short circuits, if a via is placed in a way that it would connect wires belonging to different signals. It is recommended to run a Design Rule Check after using the VIA command with the signal_name parameter!
Entering a number changes the diameter of the via (in the actual unit) and the value remains in use for further vias. Via diameters can be up to 200 mm (7.7840 inch). The drill diameter of the via is the same as the diameter set for pads. It can be changed with
CHANGE DRILL diameter
A via can have one of the following shapes:Square
Round
Octagon
These shapes only apply to the outer layers (Top and Bottom). In inner layers the shape is always "round".
Vias generate drill symbols in the Drills layer and the solder stop mask in the SolderMaskTop/SolderMaskBottom layers.
Like the diameter, the via shape can be entered while the VIA command is active, or it can be changed with the CHANGE command. The shape then remains valid for the next vias and pads.
Note that the actual shape and diameter of a via will be determined by the Design Rules of the board the via is used in.
The layers parameter defines the layers this via shall cover. The syntax is from-to, where 'from' and 'to' are the layer numbers that shall be covered. For instance 2-7 would create a via that goes from layer 2 to layer 7 (7-2 would have the same meaning). If that exact via is not available in the layer setup of the Design Rules, the next longer via will be used (or an error message will be issued in case no such via can be set). With SET Option.ViaLength 1, the via length is textually displayed.
The following flags can be used to control the appearance of a via:
| STOP | always generate solder stop mask |
By default, a via with a drill diameter that is less than or equal to the value of the Design Rules parameter "Masks/Limit" will not have a solder stop mask. The above STOP flag can be used to force a solder stop mask for a via.
Function
Attaches voltage phase probe to buses and nets.
Syntax
VPPROBE
Voltage phase probes allow the user to view the phase of node voltages in AC simulation results. Command available as context menu item on nets in schematic, as well as through command line and with a toolbar command button.
Function
Attaches voltage probe to buses and nets.
Syntax
VPROBE ..
Voltage probes allow the user to view node voltages in simulation results. Command available as context menu item on nets in schematic, as well as via command-line and via a toolbar command button.