Schematic Entry and PCB layout

In this lab you will be using a program to enter a schematic and lay out a printed circuit board (PCB) that will then be manufactured.  At this point of the semester you don't know enough to design your own circuit, so I am giving you one that we will use again later in the semester.  The program that we will be using to do the schematic entry is called Multisim and the program for the PCB layout is called Ultiboard   This lab will serve as an introduction to schematic entry and PCB layout.


The Lab

Schematic Entry

Starting out

Step 1.  The software for this lab should be on any of the PC's in room 310 or 212 of Hicks.  Log on to one of the computers and start the program called "MultiSim" (it is in the "National Instruments/Circuit Design Suite" program group).  The schematic defines all the interconnections between various circuit elements.

First, we'll add a title block to identify the schematic as your own.  Now download the file SwatTitleBlock.tb7 and then from the MultiSim menu choose Place→Title Block and choose that file.  Place the title block onto your schematic.  After placing it, you can right-click on the title block to move it exactly into place (e.g., the lower right corner).  Now double click on the title block and change the data in the block to reflect your circuit.

Save your circuit -- You should save your circuit someplace you can access it later (i.e., swatfiles, or Google drive...).   Files stored on the local PC may be deleted.  Also, having the files stored remotely allows you to work on your design from any of the PC's running Multisim.  Make sure that the filename is unique -- some permutation of the names of the people in the group is good.  You will be emailing me your design later on, and a unique name will help me keep your design from being confused with another.

Picking Components for the Schematic

Step 2.  At this point we want to pick the components that will be in your design (a circuit that flashes LED's) and put them on the schematic diagram.  Go to Place→Component and select the "Corporate" database, then select the "Basic" group, the "LED" family and finally select the "LED-R" as the component by hitting the "OK" button..  If you can't find one of the parts, hit the "Search..." button on the right side of the dialog box; this should make the missing parts appear.

Place the component anywhere on the diagram.   This component is an LED (Light Emitting Diode).

The rest of the components are listed in the table below.  They are all in the Corporate database.  Note that some components are used more than once, so you need to place multiple copies.

Quantity Group Family Component Description.
1 Basic LED LED-R This LED is controlled by a PMOS transistor.
4 Basic LED S-WhiteLED_LCW6SG 4 LED's controlled by an NMOS transistor.
3 Basic Resistor 680Ohm Used to limit the current through the LED's and set frequency of oscillation.
1 Basic Resistor 2kOhm Sets frequency of oscillation.
2 Basic Resistor 120Ohm Limits current in white LED's
1 Basic Resistor Potentiometer

Adjusts frequency of oscillation.

2 Basic Capacitor 0.01uF

Used by timer IC (555) that makes LED's blink.

1 Basic Capacitor 100uF
1 Analog FUN S-555_SOIC The Integrated circuit that blinks the lights.
3 Misc Connector S-HDR1x2 Allows dis/connection between two points
5 Misc Connector S-TestPnt A test point that will be useful for debugging.
1 Sources Battery Battery_9V A 9 volt battery.
1 Transistors NMOS S-IRFD024 NMOS Transistor (note arrow points inward, towards transistor)

Next you need to place some components from the MultiSim database.  Go to Place→Component and choose "Database:  Multisim Master → Group: Sources → Family: POWER_SOURCES → Component: Vcc

Place two or three Vcc symbols on your schematic.  Also place two or three GROUND symbols symbols from the same Database, Group and Family.  As you are doing your design use as many or as few of these power symbols as you need to make a neat drawing.

Your schematic should now look something like the circuit shown below but with.  Your part numbers may be different, and I have renamed some of the components (Select component, Right-Click, then Properties→Label→RefDes); you should do the same.  I also changed the default voltage of Vcc to 9 V (Properties→Value→Voltage (V)). You can also choose which information is displayed (Properties→Display)

 

Step 3.  Now you need to make all the connections.  Lets start with some simple ones.

First we will connect the battery.  The jumper labeled "JPwr" is used as on/off switch (if jumper is across pins, the battery is connect to Vcc, else it is not).  We also connect the test point and the mounting hole to ground.

 

Complete the rest of the connections as shown in the diagram below.  Your diagram may look substantially different than mine, depending on the placement of your parts.  Neatness counts -- make your diagram as neat as possible.  Note, wires that cross but don't have an intersection symbol (a dot, as shown above) are not touching.  If you need to add a junction to make a connection you can go to Place→Junction. (pdf version of circuit)

 

Important:  Double check all your connections.  Have one member of your group read off connections from my diagram while another checks it against your own diagram.  This sound tedious, but takes little time.  Any connections that get fabricated incorrectly are much more difficult to change later on. 

Select a trace that is connected to Vcc, right click on it and choose Properties→PCBSettings→Trace widths→Default and set it to 20 mils.  Repeat for ground and the the wire between JPwr and the 9 volt battery.  This will set the trace widths for the power lines on the printed circuit board to be somewhat broader than the signal lines.

Save your schematic.

PCB Layout

Step 4.  From Multisim, save your schematic.  Now go to Transfer→Transfer to Ultiboard.  Save the files that are created in the same directory you saved your schematic.  Hit "OK" on the "Import Netlist" window.  Your window should look something like the one below:

Step 5. The objects at the top of the board are the components that form your circuit, the large yellow rectangle is the circuit board.   The circuit board is large than we want.  To make it smaller, select the "Layers" tab in the lower left corner and select "Board Outline".  Now use the cursor to select the yellow rectangle, then right-click and choose "Properties".  Change the width to 2360 mils (thousandths of an inch) and the height to 2150 mils to define a board that is 2.36x2.15 inches.  (Note: you must use exactly 2.36x2.15 because all boards must be the same size because they are fabricated in a rectangular array.)

Step 6.  Move the components onto the board.  Exact location is not important except for the following:
Note: if you have trouble when you try to have parts overlap you may have to disable "Part Shoving" (this is one of the options under the "Design" tab on the menu).

  1. The battery should be at the far right of the board.
  2. Select the 555 (U1 in my design) and the 4 white LED's (L1 through L4) and right-click, Orientation→Swap Layer to put them on the other side of the board (their color should change to a pinkish/salmon).
  3. The 4 white LED's should be near the middle of the board, and all four should have the same orientation (i.e., the triangle should be in the same direction for all four diodes - don't rotate them).
  4. All the test points should be near the edge of the board - we will be connecting scope leads to them later in the semester.

A general rule to follow is to place components that are associate with each other on the schematic near to each other on the PCB layout, to minimize trace lengths and to make routing the wires on the board easier. 

Neatness counts in your board layout as well as in the schematics.  You may want to move component labels to make the diagram clearer.  Also, rotating components often makes connections more direct.  Circuit connections are shown by the yellow lines called, appropriately, the ratsnest.  Note that judicious placement of parts can significantly simplify the ratsnest (and resulting PCB); as an example see how C1, JSlow and C2 are laid out, as well as R1, R4 and R7.  Note, also, the pink components on the back of the board.

Now, add some text.  The light blue text on the diagrams is the silk screen layer, it will show up as white text on the manufactured board.  Hit the "Layers" tab (as you did to select the board outline).  Now select the layer labeled "Silkscreen Top" and add some text to the board.   Go to Place→Graphics→Text.  You should add some text that will uniquely identify your board (like your name).  My completed layout is shown later.

Most of the connections on our PCB will be 10 mils (1 mil=1/1000 inch), but the power connections (with somewhat higher currents) will be 20 mils; you set these trace widths in the schematic editor.

Step 7.  Now lets set the rules for the boards.  Go to Edit→Properties

  1. Go to the "Copper Layers" tab and set "Layer Pairs" to 1.  We will have two copper layers, one on top of the board, and one below.  More elaborate boards can be made with several layers embedded within the PC board itself.  Hit "Apply".
  2. Go to the "Design Rules" tab and set the "Vias -- Drill Diameter to 28 mil".  Also set the "Vias -- Pad Diameter to 40".  A via is a connection that is made to get a copper trace from one side of the board to another via a hole drilled in the board.  Hit "Apply".

Save your design.

Step 8.  All that is left is to make connections.  To do that go to Autoroute→Start/Resume Autorouter.  I This may take a few seconds (a complicated layout takes longer, and may ultimately fail).  Go to the "results" tab and make sure that all connections were made.  If not, see if you can determine where the problem is.  To lay down a trace of your own select the layer ("Top" or "Bottom") from the "Layers" pane.  Go to Place→Follow Me and draw the traces as needed.  If you have difficulty getting all connections made, come see me. 

To make sure all connections are made go to Design→Connectivity Check, and check all nets.  The text in the "Results" tab should say "Connectivity check completed; 0 error(s), 0 warning(s);..."

A completed board is shown below. 

To make sure everything was properly connected go to Design→Netlist and DRC Check.  (DRC stands for "Design Rule Check" - this ensures that all the nets are connected properly, and that all design rules are obeyed - e.g., there is sufficient spacing between traces...).    If you get any errors and can't fix them yourself, please contact me so we can figure out what went wrong.  (Occasionally two traces are routed too closely together, if you grab one with the cursor you can usually "nudge" it to make the violation go away).

Also make sure all the connections are made with Design→Connectivity Check and check all nets.

Any mistakes (Netlist, DRC or Connectivity) will come back to haunt you.  Double check (or have me check) to make sure there are no problems.

Finishing up

To finish up (due date is on moodle page)

  1. Send me an email with a list of the people in your lab group.
  2. Save three files on moodle:
    1. Print a color pdf of your schematic from Multisim.  Save a copy to the moodle page.
    2. Print a color pdf of your layout from Ultiboard.  Make sure you choose the option Zoom Options→Fit to Page in the print dialog box.  Choose the layers
      • Copper Top
      • Copper Bottom
      • Silkscreen Top
    3. Save a copy of the file to moodle.
    4. Also on the moodle page, upload a copy of your Ultiboard file.  It is the one with the filename extension ".ewprj". Make sure that you save this file after the routing, and not before. 
  3. Double check to make sure that you have saved the ".ewprj". I need this file to get the board manufactured.
  4. Save copies of the schematic and layout files, as well as the printout, for yourself.

Congratulations, you have finished the first lab!  Be sure to turn everything in by Thursday afternoon.  I will send the circuits out to be fabricated over the weekend.