Beginning a Board Layout

This lesson will demonstrate how to initialize a board layout and configure the required settings for PCB layout in OrCAD X Presto.

To follow along, continue with the previously downloaded files or download the starting materials from the Materials tab of this lesson.

Creating a New Design

Step 1: Select File > New > Board from the menu or the New button in the Start page.

Step 2: Select File > Save As from the menu.

Step 3: Enter presto_tutorial.brd for the file name. In the materials provided, browse to the folder Presto Walkthrough\Allegro and click Save.

Configuring Design and Board Parameters

Step 4: In the Properties Panel under Parameters, select mm for Units to change the design units to millimeters.

Note: If the Properties panel is not visible, select View > Panels > Properties from the menu.

Step 5: Ensure the accuracy is set to 4. The accuracy is automatically set to four digits. The accuracy setting determines the number of significant digits allowed after a decimal point.

Step 6: In the PCB canvas, select the green board outline.

Step 7: Back in the Properties panel, set the Length X to 100 and the Height Y to 50.

Step 8: Enter 0.3 for the Conductor Keep-in.

Step 9: Enter 0.3 for the Component Keep-in.

Step 10: In the Properties Panel under Parameters, select A3 for Sheet to change the sheet size to A3. The extents of the PCB canvas are adjusted automatically.

Step 11: Select the minus (-) key on the keyboard to zoom out to view the full extents of the PCB canvas.

Note: Another option to zoom out on the PCB canvas is to scroll down with the mouse wheel.

Moving the Board

Step 12: Click to select the Move mode from the toolbar on the side of the canvas.

Step 13: Click to select the board outline. The board is attached to your cursor.

Step 14: Move the outline so the board is more centered in the canvas. Click to place the board when finished.

Note: The board can also be moved by entering coordinates in the X and Y locations in the Properties Panel.

Step 15: Click anywhere to deselect the board. Press Escape to return to the selection mode.

Defining the Board Origin

Step 16: Right-click the Zoom Icon on the toolbar and select Zoom Points.

Step 17: Click and drag to draw a small selection around the lower-left corner of the board.

Step 18: Under General in the Properties panel, select Pick Origin Location.

Step 19: Select the lower-left corner of the board. The origin is snapped to the corner vertex automatically.

Note: Snapping can be configured by selecting the Snapping menu at the top of the PCB canvas.

Step 20: Right-click the Zoom Icon on the toolbar and select Zoom Fit.

Step 21: In the Properties Panel, select the lock icon to lock the board outline.

Configuring the Board Stackup

Step 22: Select Tools > Cross Section from the menu.

Step 23: The Cross-Section Editor window opens. Right-click on Top and select Add Layers.

Step 24: Select Below Conductor Top to create the plane below the top layer.

Step 25: Enter PowerPlane for the name prefix.

Step 26: Select Plane for the layer type. The layer function and layer material are selected automatically.

Step 27: Click Add and Exit to add the layer and its associated dielectrics.

Note: The layer is added to the tabular and graphical stackups. Additional information can be added in the stackup including:

• Thickness
• Tolerance
• Material
• Fill-in Material

Step 28: Click OK to save the settings and close the window.

Syncing the Schematic

Step 29: Select ECO > Update PCB from the menu.

Step 30: The Update Layout window opens. Select the ellipsis for Schematic to select the netlist.

Step 31: Change the Files of Type selection filter to Capture Projects (opj). Select Capture_Tutorial.opj in the working directory. Click Open.

Step 32: Select Sync. The list of unplaced components, unrouted nets, and unrouted connections is updated.

Placing Mounting Holes

Step 33: Select Tools > Mechanical from the menu.

Step 34: The Place Mechanical window opens. Select MOUNTING_HOLE1, included with the design files.

Step 35: With the window open, click to place a hole at each corner of the board. Close the window when finished.

Step 36: Select the top-left mounting hole.

Step 37: In the Properties panel under Location, enter 4 for X and 46 for Y.

Step 38: Click the button with the lock icon to lock the symbol.

Note: When a mechanical symbol, board, or any object in the PCB canvas is locked, it cannot be moved or modified.

Step 39: Repeat steps 36-38 for the remaining three holes, with the following coordinates:

• Top Right: X = 96, Y = 46
• Bottom Left: X = 4, Y = 4
• Bottom Right: X = 96, Y = 4

Measuring the Mounting Holes

Step 40: Hold Alt on the keyboard and select the top left mounting hole. The rest of the board is shaded.

Step 41: Hover your mouse over the center of the bottom left mounting hole. The distance between the two is shown.

Edge-to-edge distance is shown in red, while center-to-center distance is shown in white. Hover your mouse over another object to measure the distance between the top left mounting hole and that object.