Overview of TinyCAD’s features
Currently
selected tool dialogue
Drawing area,
multiple windows Symbol
selection
The blue lines are
wires. They “snap”
automatically to symbols and other wires - making it possible to draw
without the grid. Junctions can
be placed automatically for you.
Drawing a Design
Designs are created from in-built
objects such as wires, junctions, etc., and from imported component symbols,
such as diodes, transistors, etc.
To place symbols in to your
design:
1.
Use
the Symbol picker on the left of the screen to browse and select the symbols
that you need for your design.
2.
If
you don't know the name of the symbol you want then you can use the search
facility on the dialogue. Enter a word describing the component. As you do so
the list of components will be reduced to include just those that contain the
text in either their name or description.
If the symbol isn’t present, then you will have to create a new one –
this is described in the section on libraries.
3.
Place
the symbols on the design, by selecting them as the current tool. Do this by either double clicking on the
name, selecting the “Get” button on the symbol picker or click on the preview
of the symbol.
4.
You
place the symbol by clicking the location of where you wish to place the
symbol. You can rotate the symbol by
using the tool dialogue that normally sits at the top right of the drawing
area. Select “Up”, “Down”, “Left” or
“Right” to orientate the symbol.
5.
Once
you have finished placing symbols of that type, right click with the mouse to
end.
TIP: You can move a symbol’s text fields
around. First select the symbol for
editing, and then you can drag any of the symbol’s fields with the mouse to a
new position on the drawing.
At any one time a certain
number of symbol libraries are in use. The libraries to be searched are listed
in the libraries option of the Library Menu. Before you can start using symbols
at least one symbol library must be listed here. (See the Library Menu, in the
menu reference for more help on adding a library to this list).
To wire up your design:
1.
Use
the wire tool, which is the blue line on the toolbar.
2.
Move
the mouse over the start point of your wire, a small red circle will highlight
any active points on a symbol or another wire that it is suitable to start
wiring from.
3.
Every
time you click with the left hand mouse button you will place a corner in your
wire.
4.
Continue
drawing the wire. To end, select another
active point (which is shown with the red circle).
5.
Notice
how the wire tool is magnetic towards symbols’ pins and other wires.
6.
When
you place a wire connecting to another wire a junction is placed for you
automatically.
TIP: It is a
common mistake to use polygon lines instead of wires to wire up
components. This should be avoided
because TinyCAD will not be able to use the special features for you. Wires automatically snap to symbols, and
without wires you cannot export your circuit to a PCB design program.
Editing your
drawing
Once a symbol has been
placed you may want to change its properties. The edit tool in the drawing toolbar
is use for editing already placed objects.
Normally you don’t have to select the edit tool as it is the default
tool after you have finished with a different tool. To select it manually click on the white
mouse arrow toolbar button.
Whilst drawing an object
you may wish to move to another area of the design, so that you can move the
object to a part of the design not currently shown. Do this by dragging with
the middle mouse button (normally the scrollwheel) to pan the drawing, or use
the scroll-bars. You can also use the
scrollwheel to zoom in and out on your drawing.
Use the edit tool in the
normal Windows' way – click on objects to select them, or select multiple
objects using the Ctrl-key or dragging out an area. If you have just one item
selected then its options dialogue will be shown to let you change the options
of that object.
You can move objects in the
normal Windows' way, which is to select the objects and then drag them. By
default the connected wires come too, however, if you wish to unhook a symbol
from its wires then drag with the Ctrl-key held down.
To delete selected objects
use the delete option on the drawing toolbar (a red cross) or use the delete
key. The normal cut, copy and paste options are also available to you. You can
access these from the edit menu or use the right-mouse button to bring up the
context menu.
If you prefer you don't
have to use the new Windows' editing features of TinyCAD, still available to
you are the block move, block drag, and duplicate block tools. These can be
found in the block toolbar.
If you wish to rotate part
of a design (by 90 degrees), then you have to use the block rotate object in
the block toolbar. Outline the area you wish to rotate and then use the tool
buttons to rotate the selected area.
There is a full undo/redo
buffer built into TinyCAD. If you make a
mistake you can undo your changes with the “Undo” command in the Edit menu.
Whilst you are editing your
drawing it is saved automatically for you so you don’t lose any work should
TinyCAD crash. The default for Autosave
is to save your drawing every 10 minutes. The backup drawing is saved in the
same directory as the original but with an “.autosave” extension.
Symbol
Attributes
Each symbol has at least
two text attributes associated with it.
The Name attribute
This is the name or type of
the component that the symbol represents. If the component has a value then
insert the value here. For example, if it were a resistor then the name might
be 330R or 4k7. If the symbol represents a phono connector then the name might
be Phono.
This is an identifier that
is unique to the whole design, typical values might be R1 or Q3 etc. There may
be many resistors each with a Name field of 330R, however, each resistor must
have a unique Reference. There should only be one symbol with reference R1 in a
design.
This field can normally be
left as it is, you can use the Special tools to set the references
automatically. Either use the reference painter to “paint” each reference or use
the add symbol references automatically.
This is the attribute is
used for PCB netlist export. The PCB layout program will use this attribute to
determine which pad layout to use. There is no fixed naming convention for this
attribute and it is entirely dependent on the footprint libraries supplied with
your PCB layout program.
Not all symbols have the
package attribute by default. You must add it if you wish to export to a PCB
program. To add it, simply click on the “Add” button, and then rename the new
attribute to Package.
You may add additional
attributes to a symbol from the symbol's tool dialogue. There is no real limit
to the number of attributes you add. You may use these references for almost
any purpose, for example you may wish to add PCB layout instructions here.
All of the the symbols in
the supplied libraries have an “other” attribute already defined for you.
However, you can add more if you wish. Either add them by default by editing
the symbol in the library or add them individually to each symbol at placement
time.
Automatic
Junction placement
Junctions are placed
automatically for you, so normally you don't need to use the junction tool.
Where two wires cross they are
not considered joined unless a junction is used at the crossing point.
Junctions are also required when a pin is connected to the middle of a wire.
If you wish to place
junctions manually, then switch automatic junction placement off, in the
Options->Settings dialogue, and then the junction tool will be available to
you.
Whilst automatic junction
placement is on, you cannot select junctions.