SCHEMATIC AND SYMBOL DESIGN WITH DESIGN ARCHITECT

Invoking Design Architect

Schematic design steps

  1. Open a drawing "sheet".
  2. Instantiate components (select them from a library and place them on the sheet).
  3. Draw wires (pin-to-pin wiring connections) to interconnect the components.
  4. Create/modify component and wire "properties"
  5. Add "comments" in text or graphical form.
  6. Check the sheet for errors.
  7. Save and register the schematic sheet.

Opening a schematic sheet

A schematic drawing represents a component and may comprise one or more drawing sheets. All sheets and information for one component are contained in a single directory called a component container.

  1. Click on the OPEN SHEET icon in the Design Architect session palette
  2. In the dialog box that appears,

NOTE: If the component does not exist, a new one will automatically be created.

The Schematic Palette and Function Menus

The palette of function buttons that appears is one of four that can be displayed. Each contains functions pertaining to a specific type of activity. Most schematic drawing operations use the ADD/ROUTE or TEXT palettes.

All commands can also be activated via popup menus and/or pull-down menus from the menu bar. In addition, many of them can be activated via function keys, as indicated on the bottom of the display.

Common Schematic Drawing Operations

Undoing and redoing operations:

Changing the on-screen view of a Schematic Sheet

Select/Unselect Objects on the Schematic Sheet

NOTE: The pulldown menu allows you to specify the type of objects affected by Select/Unselect All or Area.

Alter or reorient one or more objects on a schematic sheet

Instantiating components on the sheet

Select components from supplied libraries

Generic Library (gen_lib) - Mentor Graphics-supplied library of standard digital gates, latches, and flip flops.


Board Process Library (BPL) - Mentor Graphics-supplied library of digital and analog components for different technologies.


ASIC Design Kit - Mentor Graphics-supplied library of standard cell functions for creating integrated circuits in AMI 0.5 or 1.2 micron n-well technologies.


XILINX FPGA and ALTERA PLD Libraries - are available via the Libraries pull-down menu when Design Architect is invoked via pld_da or max2_da, respectively.
  1. Select a component by clicking on its name in the library list.
  2. Place (instantiate) the component by moving the mouse pointer to the schematic sheet, dragging the "ghost" of the component symbol to the desired location on the sheet, and then click to fix the symbol at that location.
  3. Use palette buttons to flip, rotate, move, or copy symbols as needed to create a "neat" schematic.

NOTES:

User-designed components

To select a user-created component, click on the CHOOSE SYMBOL button in the schematic-palette (or select Instance > Choose Symbol) to pull up a navigator window.

Switching between library and schematic palettes

Within the schematic palette and library/parts list area, a pop-up menu is available which allows you to:
NOTE: By making a component list your default palette, you have a convenient method for toggling between the schematic-palette and the component list.

Interconnect Components with Wires

A wire is a single electrical net used to connect device pins or other wires. Each wire is assigned a unique name by Design Architect, which can be changed to something more meaningful to aid in identifying the net during simulation.
  1. Click on the ADD WIRE button in the schematic palette to enter "Add Wire" mode.
    (You may also press function key F3 or select Wire: from the popup menu.)
  2. Create the starting point of a wire by clicking on a component pin or on some point on another wire.
  3. Draw the wire by moving the cursor, clicking at each intermediate point (vertex).
  4. End the wire by double-clicking on a component pin or at a point on another wire.
  5. Repeat steps 2-4 for each additional wire.
  6. Click on OK in the ADDWI form at the bottom of the screen to exit "Add Wire" mode.
NOTES:

Assign a unique name to each wire

A wire name is an example of a "property", having a name and a value. Net names are needed for simulation and other tools. Each wire is given the default name NET when it is created. These must be changed to unique names.
    1. Click on the CHANGE VALUE button in the Text Palette.
    2. Click on a name or drag a rectangle around multiple names to select them.
    3. A "Property" form appears, showing the current name in the "property value" space. Enter the desired name and hit RETURN (or click on OK).
    4. If multiple names were selected, repeat step 3 for each selected object.
      (Each Property form is automatically displayed.)
    1. Click on the NAME NET button in the Text Palette.
    2. Click on a wire or drag a rectangle around multiple wires to select them.
    3. A "Property" form appears. Enter the desired name in the "property value" space and hit RETURN (or click on OK).
    4. Move the mouse to drag the "ghost" name to the desired location and click to place the name at that location.
    5. If multiple wires were selected, repeat steps 3 and 4 for each
      (a new Property form is displayed for each).
    1. Click on the SEQUENCE TEXT button in the Text Palette.
    2. In the form, enter

Ex. To name signals: Data0,Data1,...,Data15

Prefix = Data
Beginning index number = 0
Step by = 1
    1. Drag a rectangle around the group of wires to be named to select them.
    2. The wires are automatically named, in top-to-bottom or left-to-right order.

Creating and Naming Buses

A bus is a bundle of wires represented by a single "fat" wire to reduce the complexity of a schematic drawing. A bus is assigned an indexed net name of the form B(3:0), where "B" is the name of the bundle, and "3:0" are the indexes of the most and least significant bits of the bus, respectively, i.e. B(3:0) represents nets B(3), B(2), B(1), and B(0). Indexes may also be given in ascending order, i.e. B(0:3), where B(0) and B(3) are the most and least significant bits, respectively. Buses are created using the procedures described above for creating and naming wires, with the following differences.

Bus Rippers

A bus ripper separates (rips) a bus into individual wires or smaller bundles for connection to component pins or other wires. A menu of ripper components is available in the generic parts library. Bus rippers are connected as follows. 
	      
    Example:    B(3:0)_________________________
		           R \   R \   R \   R \
                              \     \     \     \

    Change to:  B(3:0)_________________________
		           3 \   2 \   1 \   0 \
                      ________\_____\_____\_____\____
		      |       W     X     Y     Z   |
                      |                             |
 
        B(3:0)_________________________
		             \   
                          2:1 \________ A(1:0)
This ripper connects A(1) to B(2) and A(0) to B(1), associating indexes from left to right, i.e. most to least significant.

Check the sheet for errors:

From the pull-down menu, select: Check > Sheet
or press function key CTRL-F5

Save the sheet:

From the pull-down menu, select: File > Save Sheet.

To plot a hard-copy of a schematic sheet:

  1. From the pull-down menu, select: File > Print Sheet
  2. When prompted, enter printer name mentor_ps
  3. You will receive an email message with instructions on sending the sheet to a designated printer.

Exit Design Architect:

Select CLOSE from window menu.IV.

CREATING SYMBOLS WITH DESIGN ARCHITECT

A. A SYMBOL is a graphical element representing a schematic or other circuit model comprising:

B. A symbol can be created automatically to represent a schematic drawing.

  1. While the schematic drawing is open, select (pull-down menu):
    Miscellaneous > Create Symbol
  2. The created symbol will appear on the screen, consisting of a simple block with pins, named according to the input/output ports on the schematic.
  3. The symbol must be "checked" for errors by selecting: Check > With Defaults
  4. Save the symbol by selecting: File > Save
The symbol can be subsequently altered with the Symbol Editor.

C. Creating a symbol manually with the Symbol Editor:

  1. Open a Symbol Editor Window by clicking on the OPEN SYMBOL icon in the session-palette.
  1. Draw the desired shape, using rectangles, circles, lines, arcs, polylines, polygons, and dots.
  1. Define pins, i.e. specific points to which electrical connections will be made.

NOTES:
  1. Note the cross which represents the origin point. You may move the symbol shape as desired to change this origin point.
  2. Check the symbol via Check > With Defaults
  3. Save the symbol via File > Save

D. The new symbol can now be intantiated in any schematic drawing.