I. ORCAD/SDT

OrCAD's SDT directory is where you create your schematic diagrams and the files needed to do circuit simulations.

At the SDT prompt C:ORCAD/SDT> the following utilities are available.

1. DRAFT - an interactive, schematic capture program that uses pop-up command

menus and prompts.
The worksheet
Creating a new worksheet or loading an existing worksheet. At the DOS prompt type:

DRAFT a:file.sch

DO NOT USE ANY OTHER EXTENDERS. (i.e. only use .SCH )
DO NOT LEAVE THE EXTENDER OFF.

If this file exists it is loaded, if not, a new worksheet is created. Once you have a worksheet, you are ready to create a schematic with TTL &/or CMOS parts. The short OrCAD manual discusses some of the commands needed to create a schematic diagram. If you want to know more then go to the big ORCAD manual.


The Main Command Menu (MM)

This is invoked from your worksheet by pressing Enter or the left mouse button.


Invoking commands from the MM ( 3 ways )
Some MM commands result in subcommand menus &/or prompts for input.

Saving Worksheets

QUIT from MM
WRITE from sub menu
This allows you to save to a different file from the one you used when invoking DRAFT.
UPDATE from sub menu
This saves the schematic to the file you used when invoking DRAFT.

Printing your schematic
HARDCOPY from MM
MAKE HARDCOPY from sub menu
Exiting DRAFT
QUIT from MM
ABANDON from sub menu ***** NOT SUSPEND TO DOS *****

2. ANNOTATE - Scans an input file and automatically updates reference designators. This includes updating the corresponding pin numbers that are associated with a device with multiple parts per package. Annotate modifies your work file: but it creates a backup file that contains the original copy of the work file.

After leaving DRAFT, with what you hope is a good schematic saved in a file with the .SCH, you will type the following command at the ORCAD\SDT\ prompt.

ANNOTATE source [destination] [switches]

source: The file name that you used to save your schematic

destination: A file & path where the output from this utility is placed. If the /M switch is used we don't need this.

switches: These indicate how you want OrCAD to handle the files. These will be given to you in the tutorials. In 301 you will learn more about these.

For our schematics the following command will be your best choice

ANNOTATE file.sch /O/M/U

3. CLEANUP - Scans a work file and checks for overlapping parts. It removes duplicate or overlapping wires, buses and junctions. It displays warnings on duplicate parts. It DOES NOT remove duplicate parts. This is a very common error. So, be alert to these warnings.

This is the next command after ANNOTATE.

CLEANUP source [destination] [switches]

source: The same as in annotate or the destination file in annotate.

destination: The same as in annotate.

switches: use the switches shown below. Explanations are provided in the big ORCAD manual.

CLEANUP a:file.sch /O

4. ERC - Performs a classical electrical rules check. WOW! That sounds really important. It flags unused inputs on parts, unlabeled wires connected to a bus, and invalid connections, such as two outputs wired together.

ERC source [destination] [switches]

source: the same as cleanup.

destination: a file into which the messages are placed. If not specified it displays messages on the screen.

switches: As usual use what is shown and see the big ORCAD manual for explanations.

ERC a:file.sch a:file.err
This command has created an error file called file.err. You must check this file to see if you have errors. If you do have errors then you must go back to DRAFT to fix them.

To read the .ERR file type

type a:file.err | more

This will show the error file one page at a time.

5. NETLIST - Generates a net and wire list in a number of possible formats. The default format is EDIF. This is used for simulations in OrCAD's VST. This is the final step before we will finally get to the simulation and see how the circuit works.

NETLIST source [destination] [format] [switches]

source & destination are the same as in ERC.

format: If you do not specify, it is an EDIF format. This is what we will use for VST.

switches: Same as usual.

NETLIST a:file.sch a:file.net /O/P

If you get error messages then you will have to go back to DRAFT and fix your drawing.

The OrCAD functions

I. Blocks

This function allows you to move or drag or copy a block

Move - allows moving a block to another location on your sheet

Place the cursor at one corner of the drawing and press B for Begin. Move the cursor to opposing corner and a rectangle will encase your drawing. Press E for End. Now move the block and press P for Place.

Drag - this allows moving a block while extending wires.

Save - this allows copies of a block to be made.

Make these selections from MM onward
  • Block
  • Save
  • Begin to enclose
  • End it
  • Block
  • Get
  • Place
    • II. Labels
    You can use these for connecting wires and see what states are occurring during the simulation at other than the inputs and outputs.

    From the MM choose
    Place
    Labels

    You will see:

    Label ?

    Type the label in UPPERCASE (no spaces and 8 characters max.) then press Enter key. You will see:

    Place Orientation Value Larger Smaller Find Jump Zoom Esc

    Use the mouse or arrow keys to move labels.

    - Orientation
    Horizontal
    Vertical
    Horizontal labels must be above the wire. When the color of the label changes the label is in the correct position. (Do not let the label hang off the edge of a wire) Press P to place the label.

    Vertical labels must be on the right side of the wire. When the color changes press P to place it.

    III. Delete

    Select Delete from the MM and you will get a submenu
    Object
    Block


    Object - Press O and place the cursor on the object and press D for Delete
    Block - Press B and outline the block as usual then press D for delete.


    IV. Large drawings

    From the MM select
    Set
    Worksheet Size
    A (11 x 8.5) usual size
    B (17 x 11)
    C (22 x 17)
    D (34 x 22)
    E (44 x 34)
    When making a hardcopy of large drawings you can make them fit on a single sheet with :

    c:\ORCAD\SDT> PLOTALL file.sch /o/p/g/s 0.474


    V. Zoom

    If you are working on a large drawing and you want to see all of it at once, this function will help you.

    From the MM select Zoom
    Select
    1
    2
    5
    10
    20
    Usually 2 will do OK.

    VI. Macro

    This function allows you to repeat something (such as drawing or a series of keystrokes)

    From the MM select
    Macro
    Capture

    You will get the prompt "Capture Macro?"

    Press the CTRL key and any other key (A-Z) simultaneously. Press Enter.

    Now draw the circuit you wish to repeat or press the keys (Place, Wire, Begin) and finally press the CTRL-END keys. Move the cursor to any position and press CTRL and the key you chose before. You should see a copy of your drawing or be ready to draw a wire etc.