[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Pcb
works and how to develop your layouts to make the best use of Pcb
's
features. All event translations (i.e. the buttons and keys you
press) refer to the default application resource file shipped with Pcb
.
There is probably no need to change this unless your window
manager uses some of the button events itself; however, if you want
to customize the behavior of Pcb
then changing the resource file
is usually the best way to do it.
Get yourself a printout of this chapter and User Commands, if you haven't already done so, and follow the examples.
Start Pcb
(the actual command will use all lower-case letters)
without any additional options.
If you get the error message:
can't find default font-symbol-file 'default_font' |
m4
program supports searchpaths.
If not, get GNU m4
.
For other messages, see A.2 Troubleshooting.
Another quick-start is provided by pcbtest.sh
in the `src'
directory. If some features don't seem to work, try running pcbtest.sh
,
if that works, then Pcb
hasn't been installed properly.
2.1 The Application Window | The elements of the main window. | |
2.2 Log Window | The optional logging window | |
2.3 Library Window | The circuit selection window | |
2.4 Netlist Window | The desired connections window | |
2.5 Drawing and Removing Basic Objects | ||
2.6 Moving and Copying | ||
2.7 Loading and Saving | ||
2.8 Printing | Creating Gerber files or postscript files | |
2.10 Arrow Tool | Selecting/Moving objects. | |
2.11 Rats Nest | Helps you place and route tracks against a netlist. | |
2.12 Design Rule Checking | Check for manufactureability | |
2.9 Connection Lists | How to get a list of all or some connections. |
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
2.1.1 Menus | ||
2.1.2 The Status-line and Input-field | What is the program configuration. | |
2.1.3 The Panner Control | Used to pan the layout view when zoomed in. | |
2.1.4 The Layer Controls | Switch layers on/off; change current one. | |
2.1.5 The Tool Selectors | Select a layout tool. | |
2.1.6 Layout Area | Where the layout is drawn. |
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
move pointer to the appropriate screen position and press a button |
Pressing Btn3 in the Layout area also pops up a menu with many of the most common operations (except when you're in the midst of drawing a line or arc). When a choice in the Btn3 popup menu needs a cross hair position, it uses the position where the cross hair was when Btn3 was pressed. For example, to get detailed information on an object, place the cross hair over the object, press Btn3, then choose `object report'. If you pop up the Btn3 menu but don't want to take any of the actions, click on one of the headers in the menu.
The Screen menu also allows you to turn on and off the visiblity of the solder-mask layer. When the solder-mask layer is made visible it obscures most of the layout, so only turn this on when you really want to know what the solder-mask will look like. The solder-mask that you see belongs to the side of the board you are viewing, which can be changed with the `view solder side' option, also found in the Screen menu. When the solder-mask is displayed, the pin and pad clearance adjustments (see section 1.5 Lines) alter the size of mask cut-outs.
Pcb
always knows which tracks
were routed by the auto-router, and you can selectively remove them
without fear of changing tracks that you have manually routed
with the `rip-up all auto-routed tracks' entry in the Connects
menu. The `design rule checker' entry runs a check for copper
areas that are too close together, or connections that touch too
tenously for reliable production. The DRC stops when the first
problem is encountered so after fixing a problem be sure to
run it again until no problems are found.
Warning: COPPER TEXT IS IGNORED BY THE DRC CHECKER. |
Pcb's
windows to the front. The Library window is used to
bring elements from the library into the paste-buffer. The
Message Log window holds the various messages that
Pcb
sends to the user. The Netlist window shows
the list of connections desired.
Now that you're familiar with the various menus, it's time to try some things out. From the File menu choose `load layout', navigate to the tutorial folder, then load the file `tut1.pcb'.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
The status-line shows, from left to right, the side of the board that you are viewing (Tab key changes this), the current grid values, if new lines are restricted to 45 degrees, which type of 45 degree line mode is active, whether rubberband move and rotate mode is on (R), and the zoom factor. This information is followed by the active line-width, via-size and drilling hole, keepaway spacing, and text scaling. Last is the active buffer number and the name of the layout. An asterisk appearing at the far left indicates that the layout has been modified since the last save. Note that the name of the layout is not the same thing as the filename of the layout. Change the grid factor to 1.0 mm from the Screen menu. Observe how the status line shows the new grid setting. Except for the case of the metric grid, all dimensions in the status line are in units of 0.001 inch (1 mil).
The input-field pops up (temporarily replacing the status-line) whenever user input is required. Two keys are bound to the input field: the Escape key aborts the input, Return accepts it. Let's change the name of a component on the board to see how the input-field works. Position the cross hair over R5, and press the N key. The input field pops-up showing the name for you to edit. Go ahead and change the name, then hit return. Notice the name of the element changed. Now undo the change by pressing the U key. You can position the cross hair over the name, or the element before pressing the N key.
Now select `realign grid' from the Screen menu. Notice that the status line has been replaced with an instruction to position the cursor where you want a grid point to fall. In this case, since the cross hair can only fall on a grid point, you must move the tip of the finger cursor to the place where you want a grid point to appear. Do not worry that the cross hair is not coincident with the cursor. Click Btn1 at your chosen location. See how the grid has shifted, and the status line has returned.
The present cross hair position is displayed in the upper right corner of the window. Normally this position is an absolute coordinate, but you can anchor a marker at the cross hair location by pressing Ctrl-M (try it now) and then the display will read both the absolute cross hair position as well as the difference between it and the marker. The numbers enclosed in < > are the X and Y distances between the cross hair and the mark, while the numbers enclosed in parenthesis are the distance and angle from the mark to the cross hair. The values displayed are always in units of 0.001 inch (1 mil). Pressing Ctrl-M again turns the marker off.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Move the pointer back into the Layout area.
Increase the zoom by hitting the Z key. See how the inner part of
the panner becomes smaller to reflect that you are viewing a smaller
part of the layout. Now zoom out by hitting Shift-Z. If you
hit the arrow key with the pointer in the Layout area, it moves
the pointer rather than scrolling the window. In general the keyboard
shortcuts depend on which region of Pcb's
window the pointer
is over. For the most part, the key strokes in this manual refer to
the case when the pointer is in the Layout area. You can do fine
scrolling in the Layout area by dragging it directly with the
Panner tool. Press the Escape key to select the panner tool.
Now drag in the layout area with Btn1 down. You can scroll the drawing
window while the pointer is inside it with Mod-Arrow
keys.
If you are moving or drawing an object and go beyond the drawing window borders, the window will auto-scroll. If you want to stop the auto-scrolling while the pointer is outside the Layout area, simply pass the pointer briefly over the panner control area, or a menu button.
Another way to navigate around a layout is with Shift-Btn3. When pressed down, the layout will zoom so the whole extent of objects is visible, and will return to the previous zoom when you release the button, but will be centered at the cross hair position where the button is released. You can do this while in the middle of drawing an object. Try it now to center near U7.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
The upper buttons are used to switch layers on and off. Click <Btn1> on one or more of them. Each click toggles the setting. If you turn off the currently active layer, another one that is visible will become active. If there are no others visible, you will not be able to turn off the active layer. When the layers are grouped, clicking on these buttons will toggle the visibility of all layers in the same group. This is a good idea because layers in the same group reside on the same physical layer of the actual board. Notice that this example has 2 groups each having 3 layers, plus two other layers named `unused'. Use the `Edit layer groups' option in the `Settings' menu to change the layer groupings. Note that changing the groupings can radically alter the connectivity on the board. Grouping layers is only useful for helping you to color-code signals in your layout. Note that grouping layers actually reduces the number of different physical layers available for your board, so to make an eight layer board, you cannot group any layers.
The far side button turns on and off the visibility of elements (including SMD pads) on the opposite (to the side you're viewing) board side, as well as silk screening on that side. It does not hide the x-ray view of the other copper layers, these must be turned off separately if desired. Use the tab key to view the entire board from the other side. To see a view of what the back side of the board will actually look like, make the solder layer the active layer then press tab until the status line says "solder" on the right, then turn off the visibility of all layers except solder, pins/pads, vias, and silk. Now turn them all back on.
The lowest button, named active, is used to change the active drawing layer. Pressing <Btn1> on it pops up a menu to select which layer should be active. Each entry is labeled with the layer's name and drawn in its color. The active layer is automatically made visible. The active layer is always drawn on top of the other layers, so the ordering of layers on the screen does not generally reflect the ordering of the manufactured board. Only the solder, component, silkscreen, and solder-mask layers are always drawn in their physical order. Bringing the active layer to the top makes it easier to select and change objects on the active layer. Try changing the active layer's name to ABC by selecting `edit name of active layer' from the `Edit' menu. Changing the active layer can also be done by pressing keys 1..8.
Turn off the visibility of the component layer. Now make the component layer the active layer. Notice that it automatically became visible. Try setting a few other layers as the active layer. You should also experiment with turning on and off each of the layers to see what happens.
The netlist layer is a special layer for adding connections to the netlist by drawing rat lines. This is not the recommended way to add to the netlist, but occasionally may be convenient. To learn how to use the netlist layer see 1.9 Nets.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Escape key Panner tool F1 key Via tool F2 key Line tool F3 key Arc tool F4 key Text tool F5 key Rectangle tool F6 key Polygon tool F7 key Buffer tool F8 key Delete tool F9 key Rotate tool Insert key Insert-point tool F10 key Thermal tool F11 key Arrow tool F12 key Lock tool |
Some of the tools are very simple, such as the Via tool. Clicking Btn1 with the Via tool creates a via at the cross hair position. The via will have the diameter and drill sizes that are active, as shown in the status line. The Buffer tool is similar. With it, <Btn1> copies the contents of the active buffer to the layout, but only those parts that reside on visible layers are copied. The Rotate tool allows you to rotate elements, arcs, and text objects 90 degrees counter-clockwise with each click. Holding the Shift key down changes the Rotate tool to clockwise operation. Anything including groups of objects can be rotated inside a buffer using the rotate buffer menu option.
The Line tool is explained in detail in 1.5 Lines. Go read
that section if you haven't already.
Activate the Line tool. Set the active layer to the solder layer.
Try drawing some lines. Use the U key to undo some of the
lines you just created. Zoom in a bit closer with the Z key.
Draw some more lines. Be sure to draw some separate lines by starting
a new anchor point with Ctrl-Btn1. Change the `crosshair snaps to pin/pads'
behavior in the Settings menu. Now draw a line. Notice that
the new line points must now always be on a grid point. It might not
be able to reach some pins or pads with this setting. Increase the active line thickness
by pressing the L key. Note that the status line updates
to reflect the new active line thickness. Now draw another line. Before completing the
next line, make the component layer active by pressing the 4 key.
Now finish the line. Notice that a via was automatically placed where
you switched layers. Pcb
does not do any checks to make sure that
the via could safely be placed there. Neither does it interfere with
your desire to place lines haphazardly. It is up to you to place
things properly when doing manual routing with the Line tool.
The Arc tool is explained in detail in 1.6 Arcs. Its use is very similar to the Line tool.
The Rectangle tool, Polygon tool and Thermal tool are explained in detail in 1.7 Polygons. Go read that section. Remember that the Thermal tool will only create and destroy thermals to polygons on the active layer. Use the Rectangle tool to make a small copper plane on the component layer. Now place a via in the middle of the plane. Notice that it does not touch the plane, and they are not electrically connected. Use the Thermal tool to make the via connect to the plane. Thermals allow the via or pin to be heated by a soldering iron without having to heat the entire plane. If solid connections were made to the plane, it could be nearly impossible to solder. Click on the via again with the Thermal tool to remove the connection to the plane.
The Insert-point tool is an editing tool that allows you to add points into lines and polygons. The Insert-point tool enforces the 45 degree line rule. You can force only the shorter line segment to 45 degrees by holding the Shift key down while inserting the point. Try adding a point into one of the lines you created. Since line clipping is turned on, you may need to move the cross hair quite far from the point where you first clicked on the line. Turn off the line clipping by selecting `all-direction lines' from the Settings menu (or hit the Period key). Now you can place an inserted point anywhere. Try adding a point to the rectangle you made earlier. Start by clicking somewhere along an edge of the rectangle, then move the pointer to a new location and click again.
The delete-mode deletes the object beneath the cursor with each Btn1 click. If you click at an end-point that two lines have in common, it will replace the two lines with a single line spanning the two remaining points. This can be used to delete an "inserted" point in a line, restoring the previous line. Now delete one of the original corner points of the polygon you were just playing with. To do this, place the cross hair over the corner and click on it with the Delete tool. You could also use the Backspace key if some other tool is active. Try deleting some of the lines and intermediate points that you created earlier. Use undo repeatedly to undo all the changes that you've made. Use redo a few times to see what happens. Now add a new line. Notice that you can no longer use redo since the layout has changed since the last undo happened. The undo/redo tree is always pruned in this way (i.e. it has a root, but no branches).
The Arrow tool is so important, it has its own section: 2.10 Arrow Tool. Go read it now.
The Lock tool allows you to lock objects on the layout. When an object is locked, it can't be selected, moved, rotated, or resized. This is useful for very large objects like ground planes, or board-outlines that are definied as an element. With such large objects, nearly anywhere you click with the Arrow tool will be on the large object, so it could be hard to draw box selections. If you lock an object, the Arrow tool will behave as if it didn't exist. You cannot unlock an object with undo. You must click on it again with the Lock tool. If an object is locked, previous changes to it cannot be undone either. When you lock an object, a report message about it is popped up and will always tell you what object it is, and that it is locked if you just locked it. Other than noticing your inability to manipulate something, the only way to tell an object is locked is with a report from the Info menu. Use the Lock tool sparingly.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Pcb
s
stderr which normally is the parent shell. I suggest you iconify
the log window after startup for example by setting *log.iconic to
true in the resource file. If raiseLogWindow is set true,
the window will deiconify and raise itself whenever new messages are to be
displayed.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
m4
.
For details on the old libraries,
check-out 6.7 Library File Format and 6.6 Library Contents File Format. For
details on the format of an element file used for the new libraries,
see 6.3 Element File Format.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
The button labeled `Sel Net On Layout' can be used to select (on the layout) everything that is connected (or is supposed to be connected) to the net. If you click on a connection in the connection list, it will select/deselect the corresponding pin or pad in the layout and also center the layout window where it is located. If you "Find" (`lookup connection to object' in the Connects menu [also F key]), a pin or pad it will also choose the net and connection in the netlist window if it exists in the netlist.
If no netlist exists for the layout, then the netlist window does not appear. You can load a netlist from a file from the File menu. The format for netlist files is described in 6.5 Netlist File Format.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
hace begging gutting here, and do a real-world tutorial example.
There are several ways of creating new objects: you can draw them yourself, you can copy an existing object (or selection), or you can load an element from a file or from the Library window. Each type of object has a particular tool for creating it.
The active tool can be selected from the tool selectors in the bottom left corner or by one of the function keys listed earlier in this chapter. Each <Btn1> press with the tool tells the application to create or change the appropriate object or at least take the first step to do so. Each tools causes the cursor to take on a unique shape and also causes the cooresponding tool selector button to be highlighted. You can use either cue to see which tool is active.
Insert mode provides the capability of inserting new points into existing polygons or lines. The 45 degree line clipping is now enforced when selected. Press and hold the shift key while positioning the new point to only clip the line segment to the nearer of the two existing points to 45 degrees. You can also toggle the 45-degree clipping in the middle of a point insertion by pressing the <Key>. If the shift key is not depressed and the 45 degree line clipping mode is on, both new line segments must be on 45 degree angles - greatly restricting where the new point may be placed. In some cases this can cause confusion as to whether an insertion has been started since the two new lines may be forced to lie parallel on top of the original line until the pointer is moved far from the end points.
Removing objects, changing their size or moving them only applies to objects that are visible when the command is executed.
2.5.1 Lines | ||
2.5.2 Arcs | ||
2.5.3 Polygons and Rectangles | Drawing polygons and rectangles. | |
2.5.4 Text | ||
2.5.5 Vias | ||
2.5.6 Elements | ||
2.5.7 Pastebuffer | A multi-purpose buffer. |
There are several keystrokes and button events refering to an object without identifying its type. Here's a list of them:
<Btn1> creates (or deletes) an object depending on the current mode.
<Key>BackSpace or <Key>Delete removes the visible object at the cursor location. When more than one object exists at the location, the order of removal is: via, line, text, polygon and element. The drawn layer order also affects the search - whatever is top - most (except elements) is affected before lower items. Basically all this means that what is removed is probably just what you expect. If for some reason it isn't, undo and try again. Only one object is removed for each keystroke. If two or more of the same type match, the newest one is removed.
Use <Key>s and Shift<Key>s to change the size (width) of lines, arcs, text objects, pins, pads and vias, or to toggle the style of polygons (whether pins and vias automatically have clearances).
<Key>n changes the name of pins, pads, vias, the string of a text object, or the currently displayed label of an element.
<Key>m moves the line, arc, or polygon under the cross hair to the active layer if it wasn't on that layer already.
<Key>u (undo) recovers from an unlimited number of operations such as creating, removing, moving, copying, selecting etc. It works like you'd expect even if you're in the midst of creating something.
Shift<Key>r restores the last undone operation provided no other changes have been made since the undo was performed.
<Key>tab changes the board side you are viewing.
For a complete list of keystrokes and button events see 5.3 Default Translations.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
<Key>l, Shift<Key>l and the entries in the Sizes menu change the initial width of new lines. This width is also displayed in the status line.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Now switch to rotate-mode and press <Btn1> at the text-objects location. Text objects on the solder side of the layout are automatically mirrored and flipped so that they are seen correctly when viewing the solder-side.
Use <Key>n to edit the string.
TEXT OBJECTS ON COPPER LAYERS CREATE COPPER LINES BUT THEY ARE NOT SCANNED FOR CONNECTIONS. If they are moved to the silkscreen layer, they no longer create copper.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Now that you're familiar with many of the basic commands, it is time to put the first element on the layout. First of all, you have to load data into the paste buffer. There are four ways to do this:
1) load the data from a library 2) load the data from a file 3) copy data from an already existing element 4) convert objects in the buffer into an element |
Select lsi from the menu in the library window press <Btn1> twice at the appropriate text-line to get the MC68030 CPU. The data is loaded and the mode is switched to pastebuffer-mode. Each notify event now creates one of these beasts. Leave the mode by selecting a different one or by <Key>Escape which resets all modes.. The cross hair is located at the mark position as defined by the data file. Rotating the buffer contents is done by selecting the rotate entry of the Buffer menu or by pressing Shift<Key>F3. The contents of the buffer are valid until new data is loaded into it either by a cut-to-buffer operation, copy-to-buffer operation or by loading a new data file. There are 5 buffers available. Switching between them is done by selecting a menu entry or by Shift<Key>1..5. Each of the two board sides has its own buffers.
The release includes all data files for the circuits that are used by the demo layout. The elements in the LED example are not found in the library, but you can lift them from the example itself if you want. If you have problems with the color of the cross hair, change the resource cross hairColor setting to a different one.
Now load a second circuit, the MC68882 FPU for example. Create the circuit as explained above. You now have two different unnamed elements. Unnamed means that the layout-name of the element hasn't been set yet. Selecting description from the Display menu displays the description string of the two circuits which are CPU and FPU. The values of the circuits are set to MC68030 and MC68882. Each of the names of an element may be changed by <Key>n at the elements location and editing the old name in the bottom input line. Naming pins and vias is similar to elements. You can hide the element name so that it won't appear on the board silkscreen by pressing <key>h with the cursor over the element. Doing so again un-hides the element name.
Entering :le and selecting an element data file is the second way to load circuits.
The third way to create a new element is to copy an existing one. Please refer to 2.6 Moving and Copying.
The fourth way to create a new element is to convert a buffer's contents into an element. Here's how it's done: Select the Via-tool from the Tool pallette. Set the grid spacing to something appropriate for the element pin spacing. Now create a series of vias where the pins go. Create them in pin number order. It is often handy to place a reference point (!Ctrl<Key>m) in the center of the first pin in order to measure the location of the other pins. Next make a solder-side layer the active layer from the active-layer popup menu. Now draw the outline of the element using lines and arcs. When you're done, select everything that makes up the element with a box selection (<Btn3Down> drag, <Btn3Up>). Now select "cut selection to buffer" from the Buffer menu. Position the cursor over the center of pin 1 and press the left button to load the data into the buffer. Finally select "convert buffer to element" from the Buffer menu. You'll only want to create elements this way if they aren't already in the library. It's also probably a good idea to do this before starting any of the other aspects of a layout, but it isn't necessary.
To display the pinout of a circuit move to it and press Shift<Key>d or select show pinout from the Objects menu. A new window pops up and displays the complete pinout of the element. This display can be difficult to read if the component has been rotated 90 degrees :-( therefore, the new window will show an un-rotated view so the pin names are readable. <Key>d displays the name of one or all pins/pads inside the Layout area, this is only for display on-screen, it has no effect on any printing of the layout.
You also may want to change a pin's or pad's current size by pressing <Key>s to increase or Shift<Key>s to decrease it. While this is possible, it is not recommended since care was probably taken to define the element structure in the first place. You can also change the thickness of the element's silkscreen outline with the same keys. You can change whether a pin or SMD pad is rounded or square with the <Key>q. SMD pads should usually have squared ends. Finally, you can change whether the non-square pins are round or octagonal with the !Ctrl<Key>o.
SMD elements and silkscreen objects are drawn in the "invisible object" color if they are located on the opposite side of the board.
For information on element connections refer to 2.9 Connection Lists.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Pcb
you will probably want to save
your work. :s name passes the data to an external program which
is responsible for saving it. For details see saveCommand in
5.1 Non-Standard X11 Application Resources.
Saving also is available from the File menu, either with or
without supplying a filename. Pcb
reuses the last
filename if you do not pass a new one to the save routine.
To load an existing layout either select load layout data from the File menu or use :l filename. A file select box pops up if you don't specify a filename. Merging existing layouts into the new one is supported either by the File menu or by :m filename.
Pcb
saves a backup of the current layout depending on the resource
backup. The file is named `/tmp/PCB.%i.backup'. During critical
sections of the program or when data would be lost it is saved as
`/tmp/PCB.%i.save'.
%i is replaced by the process ID.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Pcb
now has support for device drivers,
PostScript
, encapsulated PostScript,
and Gerber X drivers are
available so far. The Gerber X
driver generates a NC drill file for automated drilling.
I recommend the use of GhostScript
if you
don't have a PostScript
printer for handling the PostScript
output. Printing always generates
a complete set of files for a specified driver.
See the page about
the Print() action for addtional information about the filenames.
The control panel offers a number of options. Most of them are not avilable
for Gerber output because it wouldn't make sense, for example, to scale the gerber output
(you'd get an incorrectly made board!) The options are:
X11
geometry specification.
This entry is only available if you use X11R5
or later.
For earlier releases the user defined size or, if not available, A4
is used.
Well known size are:
A3 A4 A5 letter tabloid ledger legal executive |
X11R5
or later. A zero
offset is used for earlier releases.
The created file includes some labels which are guaranteed to stay unchanged
awk
script to produce several printouts on one piece of paper by
duplicating the code and putting some translate
commands in front.
Note, the normal PostScript
units are 1/72 inch.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
1) create at least two elements and name them 2) create some connections between their pins 3) optionally add some vias and connections to them |
Now select lookup connection from the Connections menu,
move the cursor to a pin or via and press any mouse button. Pcb
will look for all other pins and/or vias connected to the one you have
selected and display the objects in a different color.
Now try some of the reset options available from the same menu.
There also is a way to scan all connections of one element. Select a single element from the menu and press any button at the element's location. All connections of this element will be saved to the specified file. Either the layout name of the element or its canonical name is used to identify pins depending on the one which is displayed on the screen (may be changed by Display menu).
An automatic scan of all elements is initiated by choosing all elements. It behaves in a similar fashion to scanning a single element except the resource resetAfterElement is used to determine if connections should be reset before a new element is scanned. Doing so will produce very long lists because the power lines are rescanned for every element. By default the resource is set to false for this reason.
To scan for unconnected pins select unused pins from the same menu.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Moving a single un-selected object is different from moving a selection. First of all, you can move the end of line, or a point in a polygon this way which is impossible by moving selections. Secondly, if rubber banding is turned on, moving a single object will rubber-band the attached lines. Finally, it is faster to move a single object this way since there is no need to select it first.
You can select any visible object unless it is locked. If you select an object, then turn off its visibility with the Layer controls, it won't be moved if you move the remaining visible selection.
If you have not configured to use strokes in the Pcb
user interface, then
the middle mouse button is automatically bound to the arrow tool, regardless
of the active tool (which is bound to the first mouse button). So using
the middle button any time is just like using the first mouse button
with the Arrow tool active.
The entries of the Selection menu are hopefully self-explanatory. Many of the Action Commands can take various key words that make them function on all or some of the selected items.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
Rat-lines are lines having the special property that they only connect to pins and pads at their end points. Rat-lines are drawn on the screen with a stippled pattern to make them easier to identify since they have special behavior and cannot remain in a completed layout. Rat-lines are added in the minimum length straight-line tree pattern (always ending on pins or pads) that satisfies the missing connectivity in the circuit. Used in connection with moves and rotates of the elements, they are extremely useful for deciding where to place elements on the board. The rat-lines will always automatically rubberband to the elements whether or not the rubberband mode is on. The only way for you to move them is by moving the parts they connect to. This is because it is never desireable to have the rat-lines disconnected from their element pins. Rat-lines will normally criss-cross all over which gives rise to the name "rats nest" describing a layout connected with them. If a SMD pad is unreachable on the active layer, a warning will be issued about it and the rat-line to that pad will not be generated.
A common way to use rats nests is to place some elements on the board, add the rat-lines, and then use a series of moves/rotates of the elements until the rats nest appears to have minimum tangling. You may want to iterate this step several times. Don't worry if the layout looks messy - as long as you can get a sense for whether the criss-crossing is better or worse as you move things, you're fine. After moving some elements arround, you may want to optimize the rats nest <Key>o so that the lines are drawn between the closest points (this can change once you've moved components). Adding rat-lines only to selected pads/pins (Shift<Key>w) is often useful to layout a circuit a little bit at a time. Sometimes you'll want to delete all the rat-lines (<Key>e) or selected rat-lines (Shift<Key>e) in order to reduce confusion. With a little practice you'll be able to achieve a near optimal component placement with the use of a rats nest.
Rat-lines are not only used for assisting your element placement, they can also help you to route traces on the board. Use the <Key>m to convert a rat-line under the cursor into a normal line on the active layer. Inserting a point into a rat-line will also cause the two new lines to be normal lines on the board. Another way that you can use rat-lines is to use the <Key>f with the cursor over a pad or pin. All of the pins and pads and rat-lines belonging to that net will be highlighted. This is a helpful way to distinguish one net from the rest of the rats nest. You can then route those tracks, turn off the highlighting (Shift<Key>f) and repeat the process. This will work even if the layer that the rat-lines reside on is made invisible - so only the pins and pads are highlighted. Be sure to erase the rat-lines (<Key>e erases them all) once you've duplicated their connectivity by adding your own lines. When in doubt, the <Key>o will delete only those rat-lines that are no longer needed.
If connections exist on the board that are not listed in the netlist when <Key>w is pressed, warning messages are issued and the affected pins and pads are drawn in a special warnColor until the next Notify() event. If the entire layout agrees completely with the netlist, a message informs you that the layout is complete and no rat-lines will be added (since none are needed). If the layout is complete, but still has rat-lines then you will be warned that rat-lines remain. If you get no message at all it's probably because some elements listed in the net list can't be found and where reported in an earlier message. There shouldn't be any rat-lines left in a completed layout, only normal lines.
The Shift<Key>w is used to add rat-lines to only those missing connections among the selected pins and pads. This can be used to add rat-lines in an incremental manner, or to force a rat-line to route between two points that are not the closest points within the net. Often it is best to add the rats nest in an incremental fashion, laying out a sub-section of the board before going further. This is easy to accomplish since new rat-lines are never added where routed connectivity already makes the necessary connections.
[ < ] | [ > ] | [ << ] | [ Up ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |
After a DRC error is found and corrected you must run the DRC again because the search for errors is halted as soon as the first problem is found. Unless you've been extremely careless there should be no more than a few design rule errors in your layout. The DRC checker does not check for minimum spacing rules to copper text, so always be very careful when adding copper text to a layout. The rules for the DRC are specified in the application resource file. The minimum spacing value (in mils) is given by the Settings.Bloat value. The default is 7 mils. The minimum touching overlap (in mils) is given by the Settings.Shrink value. This value defaults to 5 mils. Check with your fabrication process people to determine the values that are right for you.
If you want to turn off the highlighting produced by the DRC, perform an undo (assuming no other changes have been made). To restore the highlighting, use redo. The redo will restore the highlighting quickly without re-running the DRC checker.
[ << ] | [ >> ] | [Top] | [Contents] | [Index] | [ ? ] |