LABELLING AND MOVING PART REFERENCES
ISIS has a very powerful feature called Real Time Annotation which can be found on the
Tools Menu and is enabled by default. Full information can be found on page 11 but basically,
when enabled, this feature annotates components as you place them on the schematic. If you
zoom in on any resistor you have placed you will see that ISIS has labelled it with both the
default value (RES) and a unique reference. To edit/input part references and values click left
on the Instant Edit icon and then click left on the object you wish to edit. Do the resistors
first, entering R1, 1k and R2, 1k as appropriate. Now do the op-amp and the two terminals.
To move the 'U1' and the '741' labels to correspond with the diagram, press F2 to reduce the
snapping grid to 50th (it starts off at 100th) and then tag the op-amp. Now point at the label
'U1' and with the left button depressed, drag it to its correct position under the op-amp. Then
do the same with the '741' label.
When you have finished positioning the labels, put the snap back to 100th by pressing F3.
Although with the Real Time Snap feature ISIS is able to locate pins and wires not on the
current snap grid, working consistently with the same snap grid will keep drawings looking
neat and tidy.
BLOCK EDITING FUNCTIONS
You may have noticed that the section of circuit you have drawn so far is currently located in
the middle of the sheet, whereas it should be in the top left hand corner. To move it there, first
tag all the objects you have placed by dragging a box round them using the right mouse
button: point at a position above and to the left of all the objects; then press and hold down
the right button and drag the mouse pointer to a position below and to the right of the
objects. The selected area is shown by a cyan tag-box and (as the initial right click
automatically untags any previously tagged objects) all and only those objects wholly within
the tag-box will be tagged after the operation.
Now click left on the Block Move icon. A box will appear round all the tagged objects, and
you can now begin to move this up towards the top left hand corner of the sheet. The sheet
border appears in dark blue so you can now re-position the buffer circuit up at the top left of
the drawing. Click left to effect the move, or else you can abort it by clicking right. You should
also note how, when you moved the pointer off the Editing Window to the top or left, ISIS
automatically panned the Editing Window for you. If you want to pan like this at other times
(i.e. when not placing or dragging an object), you can use the Shift Pan feature.
The group of objects you have moved will remain tagged, so you might as well experiment
with the Copy and Delete icons which similarly operate on the currently tagged objects. The
effect of these icons can be cancelled by immediately following their use by pressing the 'U'
key for Undo.
PRACTICE MAKES PERFECT
You should be getting the hang of things now, so get some more practice in by drawing the
next section of circuitry centred around the op-amp U2:A. You will need to get a capacitor
(CAP). A quick method of picking devices whose names you know is to use the Pick
Device/Symbol command. Press the 'P' key (for Pick Device/Symbol) and then type in the
name - CAP. Use the various editing techniques that have been covered so far to get
everything in the right place. Move the part reference and value fields to the correct
positions, but do not annotate the parts yet - we are going to use the Automatic Annotator
to do this.
When you have done one op-amp filter to you satisfaction, use a tag-box and the Block
Copy icon to make three copies - four filters in all - as there are in the diagram. You may find it
useful to use the zoom commands on the View menu (or their associated short-cut keys) so as
to be able to see the whole sheet whilst doing this. When you have the four filters in position,
wire them together, and place a SW-SPDT device (SW1) on the drawing.
ANNOTATING THE DIAGRAM
ISIS provides you with four possible approaches to annotating (naming) components:
· Manual Annotation - This is the method you have already used to label the first op-amp
and resistors. Any object can be edited either by selecting the Instant Edit icon and
then clicking left on it, or by clicking right then left on it in the normal placement mode.
Whichever way you do it, a dialogue box then appears which you can use to enter the
relevant properties such as Reference, Value and so forth.
· The Property Assignment Tool (PAT) - This tool can generate fixed or incrementing
sequences and assign the resulting text to either all objects, all tagged objects (either on
all sheets or the current sheet) or to the objects you subsequently click left on. Using
the PAT is faster than manual annotation, though slower than using the Automatic
Annotator. However, it does leave you in control of which names are allocated to which
parts.
· The Automatic Annotator - Using the Automatic Annotator leads to the whole design
being annotated in a matter of seconds. The tool is aware of multi-element parts like the
7400 TTL NAND gate package and will allocate gates appropriately. However, the whole
process is non-interactive so you get far less control over the names that are allocated
than with the other two methods.
· Real Time Annotation – This feature, when enabled, will annotate components as you
place them on the design , obviating any need for you to place references and values in
your design. As with the Automatic Annotator, however, it makes the whole process
non-interactive and offers no user control over the annotation process. Real Time
Annotation can be toggled on and off through the Real Time Annotation command on
the Tools Menu or via the CTRL + N shortcut key.
In practice you can use a mix of all four methods, and in any order you choose. The
Automatic Annotator can be set to leave alone any existing annotation so that it is possible
to fix the references of certain parts and then let ISIS annotate the rest by itself. As the Real
Time Annotation is enabled by default, we shall leave it on and use the other three methods
to edit the existing annotation of the design.
The Property Assignment Tool (PAT)
Let us suppose, for the sake of argument, that you wished to pre-annotate all the resistors
using the PAT. Given that you have already manually annotated R1 and R2, you need to
generate the sequence R3, R4, R5 etc. To do this, select the Property Assignment Tool option
on the Tools menu. Enter REF=R# in the String field, then move the cursor to the next field
(the Count field) and key in the value 3. Ensure the On Click button is selected and then click
left on the OK button or press ENTER. The hash-character ('#') in the String field text will be
replaced with the current Count field value each time the PAT assigns a string to an object
and then the Count field value is incremented.
ISIS automatically selects the Instant Edit icon so that you can annotate the required objects
by clicking left on them. Point at resistor R3 and click left. The PAT supplies the R3 text and
the part is redrawn. Now do the same for the resistor below it, R4 and see how the PAT's
Count field value increments each time you use it. You can now annotate the rest of the
resistor references with some panache. When you are done with this, cancel the PAT, by
calling up its dialogue form (use the 'A' keyboard shortcut for speed) and then either clicking
on the CANCEL button or by pressing ESC.
The PAT can also be used to assign the same String to several tagged objects, for example
the part values of resistors or capacitors that all have the same value. Consider the capacitors
C1 to C4 which all have the value 220p. To assign this value, first ensure that only the
capacitors are tagged by first clicking right on a free area of the Edit Window to untag all
objects, then clicking right on each capacitor. Now invoke the PAT and enter VAL=220p in
the String field, select the Local Tagged button and click OK. That's it - you do not need to
cancel the PAT as it is not in its 'On Click' assignment mode.
Try this on your own for the rest of the diagram until you are clear about how the PAT works
- although a little tricky at first, it is an extremely powerful tool and can eliminate a great deal
of tedious editing. Do not forget that, when used in its On Click mode, you need to cancel
the tool when finished.
The Automatic Annotator
ISIS features an automatic annotator which will choose component references for you. It can
be made to annotate all the components, or just the ones that haven't yet been annotated - i.e.
those with a '?' in their reference.
Since you have already annotated some of the parts, we will run the Automatic Annotator in
'Incremental' mode. To do this, invoke the Global Annotator command on the Tools menu,
click on the Incremental button, and then click on OK. After a short time, the diagram will be
re-drawn showing the new annotation. Since the OPAMP device is not a multi-element part
like a true TL074, the annotator annotates them as U2 to U5 which is not what is wanted. To
correct this, edit each one in turn and key in the required reference. We will see how to create
and use a proper TL074 later on.
Even with the automatic annotator, you still have to set the component values manually, but
try this for speed - instead of moving around the drawing to edit each component in turn,
simply key 'E' for Edit Component (on the Edit menu) and key in a component's reference.
This automatically locates the desired part and brings up its Edit... dialogue form. You should
also try out the using the Property Assignment Tool as described in the above section.
CREATING NEW DEVICES
The next section of the circuit employs a 7110 digital attenuator, and this provides an
opportunity to learn how to make new devices in ISIS.
In ISIS new devices are created directly on the drawing - there is no separate device editor
mode, let alone a separate program. The new device is created by placing a collection of 2D
graphics and pins, annotating the pins, and then finally tagging them all and invoking the
Make Device command.
You will find it helpful when creating new devices to sketch
out on paper how you want the device to look, and to
establish roughly how big it needs to be by considering
how may pins there will be down each side and so on. In
this case you can use the diagram opposite as a guide. The
first thing we need to do is to locate a free area of your
design where the new device can be created - click the left
mouse button on the lower-right region of the Overview
Window to position the Editing Window on that area of the
design.
Begin by drawing the device body of the new device. Select the Box icon. You will see that
the Object Selector on the right displays a list of Graphics Styles. A graphics style
determines how the graphic we are about to draw will appear in terms of line colour, line
thickness, fill style, fill colour, etc. Each style listed is a different set of such attributes and
define the way different parts of the schematic appear.
ISIS supports a powerful graphics style system of local and global styles and the ability of
local styles to ‘follow’ or ‘track’ global styles that allows you to easily and flexibly customise
the appearance of your schematic. See the section Graphics And Text Styles on page 41 for a
complete explanation of how styles work and how they are used.
As we are drawing the body of a component, select the COMPONENT graphics style and
then place the mouse pointer over the Editing Window, press and hold down the left mouse
button and drag out a rectangle. Don't worry about getting the size exactly right - you can
always resize the rectangle later. You will see that, as a result of choosing the COMPONENT
graphics style, the rectangle appears in the same colour, fill, etc. as all the other components
on the schematic.
The next thing to do is to place the pins for the new device. To do this, first select the the
Device Pin icon. The Object Selector lists the types of available pins (note that you can also
create your own pin objects in ISIS, though we will not cover that in this tutorial). Select the
Default pin type from the selector; the Overview Window provides a preview of the pin with
the pin's name and number represented by the strings NAME and 99 and its base and end
indicated by an Origin marker and cross respectively - the cross represents the end to which
you will eventual connect a wire. Use the Rotation and Mirror icons to orient the pin preview
ready to place the left-hand pins and then click the left mouse button in the Editing Window
on the left edge of the rectangle where you want each pin's base to appear. Place pins for the
VIN, D0..D5, S1..3 and DGND pins. Note that you can use the DOWN key to move the mouse
pointer down one grid square and the ENTER key as a substitute for the left mouse button - it
is sometimes quicker to use these keys instead of the mouse. Now click left on the Mirror
icon and then place the three right-hand pins: RFB, IOUT and AGND. To finish, place two
pins, one on the top edge and one on the bottom edge of the rectangle, adjusting the
Rotation and Mirror icons before placing them in order that they point outwards from the
device body; these pins will be the VDD and VBB power pins and will eventually be hidden
(this is why they are not shown in the figure).
At this stage, you can reposition the pins or resize the rectangle as required. To move a pin,
tag it with the right mouse button and then drag it with the left button; to re-orient it, use the
Rotation and Mirror icons. To adjust the size of the device body rectangle, tag it with the
right mouse button, click and hold down the left mouse button on one of the eight 'drag
handles' (the small white boxes at the corners and mid-points of the rectangle's edges) and
drag the handle to the new position. If you adjust its width, you will also need to draw a tagbox
(with the right mouse button) around the pins and then use the Move icon to re-position
them.
So, having arranged the device body rectangle and pins as required, we now need to annotate
the pins with names and numbers, and to assign them an electrical type. The electrical type
(input, power, pull-up, etc.) is used by the Electrical Rules Check to ensure that only pins
with the correct electrical type are inter-connected.
We will first assign names, electrical types and visibility. To do this, we have to tag each pin
by clicking right on it and then edit it by clicking left on the tagged pin; the pin displays its
Edit Pin dialogue form.
Edit each pin in turn, as follows:
· Enter the pin's name in the Name field. Leave the Number field empty as we will assign
the pin numbers with the Property Assignment Tool.
· Select the appropriate electrical type for the pin - Output for the IOUT pin, Power for the
VDD, VBB, AGND and DGND pins, and Input for the remainder.,
· Select whether the pin is to be hidden by unchecking its Draw body checkbox - the
VDD and VBB pins are both standard power pins and can be hidden. The AGND and
DGND pins are non-standard and so need to remain visible in order that they can be
wired up as appropriate to the design the device is being used in.
· Select the OK button when finished.
To assign the pin numbers, we will use the Property Assignment Tool. To initialise the PAT,
select the Property Assignment Tool command from the Tools Menu, and enter NUM=# in the
String field and the value 1 in the Count field. Select the On Click button, and then close the
dialogue form with the OK button. Now carefully click on each pin in order of its number
(IOUT, AGND, etc.). As you click on each pin, it is assigned a pin number by the PAT. When
done, don't forget to cancel the PAT by bringing up its dialogue form and selecting the
CANCEL button.
All we do now is actually make the device. To do this, tag all the pins and the body rectangle
- the easiest way is to drag out a tag-box with the right mouse button around the whole area
being careful not to miss out the two hidden power pins. Finally, select the Make Device
command from the Library menu to display the Make Device dialogue form. Key in the name
7110 in the Name field and the letter U in the Prefix field. Then press the Next button until
the list of writable device libraries is displayed, select an appropriate library and then click the
OK button to save the new device.
FINISHING TOUCHES
Now that you have defined a 7110 you can place, wire up and annotate the remainder of the
diagram - use the Automatic Annotator in Incremental mode to annotate the new parts
without disturbing the existing annotation.
The labelling and bracket around the six input terminals DA0-DA5 is done with 2D graphics.
ISIS provides facilities for placing lines, boxes, circles, arcs and text on your drawings; all of
which offered as icons on the Mode Selector toolbar.
The bracket is made from three lines - place these by selecting the Line icon and then clicking
at the start and end of each line. Then place the text FROM PIO-1A as shown by selecting
the Text icon, setting the Rotation icon to 90° and then clicking left at the point where to want
the bottom of the 'F' character to appear. You can of course tag and drag 2D graphics objects
around to get things just how you want.
Finally, you need to place a sheet border and a header block. To do the former, select the Box
icon, zoom out till you can see the whole sheet outline (dark blue) and then place a graphics
box over it. It is important to realise that the dark blue sheet outline does not appear on hard
copy - if you want a bounding box you must place one as a graphics object.
The header block is worthy of more discussion. It is, in fact, no different from other symbols
such as you might use for your company logo (see section [Symbols And The Symbol
Library] for more on symbols). A default header block called HEADER is provided but you
can re-define this to suit your own requirements - see The Header Block on page 38.
To actually place the header, select the Symbol icon and then click left on the P button of the
Object Selector to display the Symbol Library Selector dialogue form. Picking symbols from
symbol libraries is similar to picking devices from device libraries except that there is no Prefix
selector. Select the HEADER object from the SYSTEM symbol library and close down the
dialogue form. With HEADER now the current symbol, point somewhere towards the bottom
left of the drawing, press the left mouse button, and drag the header into position.
Some of the fields in the header block will fill in automatically; others such as the Design Title,
Sheet Title, Author and Revision need to be entered using the Edit Design Properties and
Edit Sheet Properties commands on the Design menu. Note that the Sheet Name field on the
Edit Sheet Properties dialogue form is different from the Sheet Title - the Sheet Name is a
short label for the sheet that is used in hierarchical design. The Sheet Title is a full description
of the circuitry on that sheet and it is this that will appear in the header block.
You will need to zoom in on the header to see the full effects of your editing.
SAVING, PRINTING AND PLOTTING
You can save your work at any time by means of the Save command on the File menu, and
now is as good a time as any! The Save As option allows you to save it with a different
filename from the one you loaded it with.
To print the schematic, first select the correct device to print to using the Printer Setup
command on the File menu. This activates the Windows common dialogue for printer device
selection and configuration. The details are thus dependent on your particular version of
Windows and your printer driver - consult Windows and printer driver documentation for
details. When you have selected the correct printer, close the dialogue form and select the
Print option on the File menu to print your design. Printing can be aborted by pressing ESC,
although it may be a short time before everything stops as both ISIS and possibly your
printer/plotter have to empty their buffers.
Further details regarding printer and graphics output are given under Hard Copy Generation.
If you have the demo version, please note that you can only print un-modified sample
designs. To try this now, use the Load command on the File menu to load a sample design.
MORE ABOUT CREATING DEVICES
Making a Multi-Element Device
We shall now define a proper library part for the TL074 quad op-amp. As there are four
separate op-amps to a single TL074 package our tutorial will be showing you how to create
multi-element devices using the Visual Packaging Tool.
The illustration on the left shows the new op-amp device before it is
made. The op-amp is made from some 2D graphics, five pins and an origin
marker. We will look at two ways to construct the op-amp graphics. The
easiest approach uses the pre-defined OPAMP symbol. Proceed as
follows:
· Click on the Symbol icon and then click the P button at the top left of the Symbols
Object Selector. This will launch the Symbol Library Selector dialogue form.
· Double-click on OPAMP in the System Library and close the dialogue form using the
Windows Minimise button on the right of the title bar.
· Position the mouse pointer in an empty area of the Editing Window and use the left
mouse button to place the op-amp. The op-amp automatically appears in the
COMPONENT graphics style as this style was used to create the symbol.
Now place the pins around the component body. This is the same process as for creating the
7110 attenuator earlier:
· Select the Device Pin icon to obtain a list of available pin types and select the Default
type.
· Use the Rotate and Mirror icons to orient the pins before placing them on the design.
· Once all the pins are in the correct positions, edit each pin in turn by tagging it with the
right mouse button and then clicking left on it. Use the resulting Edit Pin dialogue form
to annotate the pin with the correct electrical type and pin name. We have to give the
pins names so that we can reference them in the Packaging Tool however, we don't
want the name to be displayed (as the op-amp pins' uses are implicit from the graphics)
so ensure that the Draw Name check-box is not checked. Note, there is no need to
specify pin numbers as these will entered using the Packaging Tool.
The power pins have the names V+ and V- and have the electrical type of Power; if you place
them just in from the left edge of the op-amp, you will find they just touch the sloping sides of
the OPAMP graphic whilst keeping their pin ends (marked by an 'X') on a grid-square. If in a
similar situation, they didn't touch, you could 'extend' the base of the pin by placing short
lines in 2D Graphic Mode and with the mouse snap off. The input pins have the names +IP
and -IP and the electrical type Input. The output pin has the name OP and the electrical type
Output.The final stage is to place an Origin marker. Select the Marker icon to display a list of system
marker symbols in the Object Selector. Select the Origin marker in the System Library and
then place the marker symbol at the centre of the op-amp graphics. The Origin marker is
displayed as a rectangle with cross-hairs and it indicates to ISIS how the new device should
appear around the mouse pointer when the device is dragged or placed in a design.
We have now completed making the device. Tag the constituent parts - the op-amp symbol,
pins and the Origin marker - by dragging out a tag-box around them using the right mouse
button, and then invoke the Make Device command on the Library menu. Then proceed as
follows:
· Enter the Device Name as TL074 and the Prefix as 'U'
· Click Next button display the Packaging page and click Add/Edit to launch the
packaging tool itself.
The Visual Packaging Tool
The visual packaging tool provides a graphical environment in which to assign one or more
PCB footprints to a schematic part. For each packaging, a table of pin numbers to pin names is
created such that different packagings can have different pin numbers for the same schematic
pin.
Having launched the packaging tool, the first thing to do is to create a packaging:
· Click the Add button. This will launch the ARES library browser.
· Select the PACKAGE library, and double click the DIL14 part.
Then, you need to make the following changes to the default settings for the packaging:
· Change the number of elements from 1 to 4. This corresponds with the fact that there are
four op-amps within the one physical DIL14 package.
· Mark the V+ and V- pins as common pins. This means that they will have the same pin
number on each element, and that you can wire to any or all of the pins on the elements
on the schematic. All such wiring will be deemed interconnected.
· Click the Gates can be Swapped checkbox. This specifies that the elements are identical
and the ARES can perform gateswap operations on this part.
No comments:
Post a Comment