Transcript PCB design with Design Entry CIS and Layout Plus

ECE-121
TA: Ritu Bajpai
Drawing the schematic
 We have a new version of cadence in the lab now. You
will find it listed under ALL PROGRAMS as cadence
16.1 (I am not sure if 16.1 but 16 something)
 We will use design entry CIS to make the schematic
 If given an option you will choose PCB design allegro
in the beginning
 Start a new project as we used to do in the older
version
Drawing the schematic
Click this icon to
bring up the place
part window
Click this icon
to add libraries
Libraries
 You can pick up your components from the following
libraries
 Diode from Pspice-diodes
 TIP 31A and TIP32A from Pspice-pwrbjt
 Voltage regulator and LM741 form Pspice-Opamp
 Resistors and capacitors from Pspice-analog
Note: You will not find your diode number in the diode
library. You can use any other diode because we only
need to select the right foot print. More on this later in
the slide show.
PCB design
 The PCB board that we will build is the simplest type
with insulating layer in between two conducting layers
of Cu on top and bottom
 Since our aim is to export the design to layout plus and
create a layout for our PCB board, we are not
concerned with the values of the components. You can
leave them as default values.
 Do not connect a AC source as an input to the voltage
rectifier.
 In place of the AC source we want two vias where we
should be able to provide transformer connections.
 A via is a through hole in the PCB
 We could connect a resistor across the two points
where the AC power supply to the rectifier is
connected
 This will generate 2 vias where we will be able to
connect power supply from the transformer
Matching the pins
 Once you have connected all the components, recheck
your circuit because once the PCB is made you cannot
change your connections.
 Match the pin numbers on the schematic with the pin
numbers of the parts in your kit.
 For example, TIP BJTs have pins 1,2 and 3 as the base,
collector and emitter for the component in your kit.
The numbers should correspond to the same in the
schematic.
Matching the pins
 Can you find any component for which the pin
numbers don’t match?
 LM7805 has pins 1 input, 2 gnd and 3 output on the
part in your kit but in the schematic it has 1 input, 2
output and 3 gnd
 This will swap pins 2 and 3 for us when we put the
component on the board
 So we will create our own symbol for LM 7805 and give
it the pin numbering that we want
Creating a library
You will see a new library
appear in the library
folder
New library
You can save
your library
with a new
name if you
like
Creating a part
Select library name
and right click to
get the menu and
then click New Part
Creating a part
You can
name your
part
LM7805C
and PCB
Footprint as
TO220.
Click OK
Creating a part
Use “draw
line” from
the tool bar
on the right
to draw a
box along
the dotted
line.
Next use pin icon from the toolbar to draw
pins. Name them IN, GND and OUT and
number them 1,2 and 3 respectively. Type will
be input, power and output respectively.
Creating a part
 Having created the part, you can remove the LM7805
symbol that you had used from opamp library and
replace it by the symbol that you just created.
 Now you are ready to create a Netlist for your design.
 Before that you will have to modify the footprint name
for some of the components as this software will not
accept / and . in the footprint name. This is just a
software compatibility problem.
 We will modify the footprint name for the resistors,
capacitor and LM 741
Modifying footprint name
 Select a resistor
 Right click and choose edit properties
 Scroll to the right to find part footprint
 Note the value of the footprint as you will need it later
 Now modify the footprint name to remove any . or / in
the name
 Do this for all the resistors, capacitors and LM741
Creating the netlist
Click on schematic,
then go to Tools and
click on create netlist.
Create netlist window
pops up, hit OK.
This should create a
.MNL file in your
project folder.
Sometimes it doesn’t
show the .MNL file
immediately in which
case try creating the
netlist again.
Starting Layout Plus
 Now we will start the layout plus software again from
cadence 16
 Go to file->New
 For input Layout TCH
browse the file default.tch
(not _default.tch)
 For input MNL file read
your netlist file from your
project folder
 Hit apply ECO.
Select footprint
 You will now need to link your components to the
footprints.
 The software will automatically read some footprints
but not all so you will
have to enter the ones
that it does not take
on its own.
 We will use 1st option
of linking existing footprint to component
Footprints
 Footprints basically contain the information about physical
dimensions and distances between pins of the device so
that vias for placing the component on the PCB can be
made accordingly.
 For your design look for the footprints
LM 741 will be in DIP100
LM7805 will be in TO, look for TO 220 showing pins 1,2 and 3
Capacitor, Resistor and Diode footprints are in the libraries
TM_CAP_P, TM_AXIAL and TM_DIODE respectively. Use
the footprint names that you earlier made a note of. For
diode use DO35
 After choosing all the footprints you will get a view of
all your components
•Place the footprint within the rectangular outline.
•Place the design components so that they are evenly spread
out. This will make routing and tracking easier later on.
Settings
 Select View Spreadsheet in the toolbar (A grid like
icon). A pop-up menu will appear.
 Select Nets. The Nets spreadsheet will appear.
 Select the "Width" cell. All the cells in that column
should be highlighted.
 Right click the mouse and select Properties from the
pop-up menu. The Edit Net dialog box will appear.
 Change Min Width to track width 30 (mils). Change
Conn Width to 50 (mils). Change Max Width to 65
(mils). Click O.K.
Settings
 Next ensure the pad widths are 80mils.
 Select View Spreadsheet in the toolbar. A pop-up
menu will appear.
 Select Padstacks. The Padstacks spreadsheet will
appear.
 Select the Pad Width and Pad Height cells. Right-click
and select Properties.
 Enter 80 (mils) for both Pad Width and Pad Height.
Click O.K.
Settings
 Next disable all layers for routing except the BOTTOM.
Select View Spreadsheet in the toolbar. Select Layers.
 In the Layers spreadsheet, click on the Layer Type cell
to highlight the entire column. Press the Ctrl (on the
keyboard) and click the BOTTOM.
 Right-click and select Properties. In the Edit Layer
dialog box, select the Unused Routing option.
 Now all tracks will be routed on the bottom layer. This
will simplify component soldering once the board is
fabricated.
Drawing the board outline
 Click on the Obstacle Tool in the toolbar.
 Place the crosshair of cursor on the black field of the
design window and double click.
 The Edit Obstacle window should appear.
 Select Board Outline for the Obstacle Type.
 Change the Width to 62 mils.
 Select Global Layer for the Obstacle Layer. Click
OK.
 Begin drawing enclosed border of the design.
 Select Auto-> Autoroute -> Board. The software will




route the board.
When it is done, a pop-up window will announce that
the task has been completed. Click O.K.
Any thin yellow connections still present in the layout
show that those tracks have not been routed.
Select Auto->Unroute->Board. Move the components
around and try routing it again.
Its more of a hit and trial thing but if you are not able
to route it, you can enable both top and bottom layer
for routing.
Creating Gerber files
 Once done with routing proceed to creating Gerber
files
 Step by step instructions are on the lab website