Cadance OrCAD Capture
Capture is the core schematic entry program in the three program suite by Cadance called OrCAD.
This suite also consists of Pspice (circuit simulation software) and Layout (circuit board layout) packages.
All applications begin with Capture.
Running Capture:
Select Capture CIS
At the window prompt select “PCB Design Studio with Capture CIS”
The package will take a few seconds to load. Then select “File”
“New” and “Project”
At the window prompt enter the project name.
Select Analog or MixedA/D if you are going to do circuit simulation using Pspice or PCBoard wizard if you want to make a board layout.
Select Schematic if you just need to draw your circuit design schematic.
Simple Schematic Design
Example:
Select “Schematic” in the window shown above.
Enter the Drive/network location to store your project files.
Capture will load with a blank screen.
Paper size:
Under the “Options” pull down menu select “Schematic page Properties”
The default is “A” size or 8.5x11 (We will use the “A” size)
The larger you make the paper size the more room you have for circuitry.
When you print the schematic you can always print to an 8.5x11 size paper no matter how large of a schematic you choose.
The output will be scaled to fit. However very large schematics will require a large amount of scaling which can render them illegible.
Placing parts:
Select the “Place” pull down menu to start entering parts on your schematic.
You can also use the tool bar on the right.
The right tool bar functions are:
Place part
Place wire
Place net alias
Place bus
Place junction
Place bus entry
Place power
Place ground
From the right or the pull down menu let’s select place part.
Type the part LM741
When the part is found, click on OK
Note how the search engine looks for the item as the letters are being typed.
If the item is not found you may need to add the library to the project.
Also, be sure all of the libraries are highlighted in blue.
Only highlighted libraries will be searched.
Loading more libraries then you may need is fine, it just slows the component selection the first time they are loaded.
Place the component on the page using the left mouse button. Each click places a new copy of the component.
Press “esc” to exit the place function.
The escape key always
brings you back to the top level in Capture.
. 
Editing parts:
Left click to select the LM741 part placed on the schematic. Next, right click to mirror, rotate, and edit the part.
For now we will mirror the part vertically to put the (–) input pin on top.
Components can be deleted by highlighting (left click) and pressing “Del”.
Component names and location indicators (annotation) can be edited by moving the cursor to the text and double clicking the left mouse button.
Be sure to select only the text and not the entire part.
Wiring:
Using the wiring tool connect an inverting opamp circuit as shown.
Left click on the end of the component and run the wire to its end point and left click again.
Pressing “ESC” will discard the wiring tool. Wires can be deleted by highlighting and pressing “Del”.
When two wires are connected a junction is made. The pink dot indicates a junction.
To manually add a junction select the junction tool and click on the wire cross.
To delete a junction, use the same tool and click on the existing junction.
Next place two resistors by selecting “Place Part” again and type resistor
By double clicking on the word “RESISTOR” when the overall part is NOT selected you can enter the value.
For this example we will pick a 10K input resistor and a 100K feedback.
Place two “Header 4” components and connect as shown.
Edit their names to “OUTPUT” and “INPUT”.
Power:
Place a power “VCC circle” at each of the power pin locations.
Double left click on the VCC name and change the positive supply to +15V and the negative –15V for each supply.
It is not necessary to run individual wires for power.
At each location on your schematic that requires power just insert and wire the appropriate VCC circle.
This will keep the schematic from becoming a confusing mess of wires.
Copy/Paste:
Once a part is edited with the correct name rather then editing each occurrence of the part simply copy and paste the part to add more to the schematic.
This is especially helpful with the VCC power point.
No Connects:
Place a “No connect” at pin 1 and pin 5 of the LM741.
No connects are required by the more advanced Pspice and Layout programs, so it is a good idea to get used to using them anytime a pin is to be left open.
Ground:
The most common grounds are Earth, Power, and Signal.
Earth ground is generally referred to as the “safety” ground.
It’s the third wire in the line cord plug or a physical ground connection such as a water pipe or rod driven in the ground.
It is used to prevent electrical shock or to shield circuitry.
Power ground is a high current ground path separate from the control circuitry.
This separate power ground will reduce noise in certain circuits.
The signal ground is the one used for most circuits.
In our example, place a “signal ground” and connect to pin 3 of the LM741
Title Block:
Edit the title block by double clicking on the text you wish to change.
Saving Schematic/Using tools:
Save the schematic and close the drawing.
Annotation is the component designators such as U1 for the first IC or R1 for the first resistor.
They will help you refer to components in your lab report and are required for Pspice and Layout packages.
Under “tools” select “Annotate” be sure “unconditional reference update” is checked. Then press OK.
The schematic designators for all components will be changed to sequential designators.
Note: Whenever an unconditional update is done all or some of the reference numbers can change.
When a schematic is first created this is not a problem.
However, on an existing design an unconditional update could make a PCB layout and/or a report that refers to the schematic incorrect.
In these cases when adding new parts to the schematic substitute a ”?” for the number in the component designator and only run an incremental update.
Then only the new parts will be changed and added to the designator list.
Be especially careful when copy and pasting components or you could end up with two components with the same designators.
Importing the schematic:
To copy this schematic to word:
Using the mouse hold the left button down and highlight the circuitry on your open Capture schematic.
Copy and paste the circuit into your word document.
More Advanced topics:
Nets:
All wiring connections are internally labeled. These labels are called “Net” and are kept track of in a net list.
For example, in our circuit above the wires from R1 to R2 to U1 pin 2 are all the same connection and would be assigned an internal net name.
If this net name had some significance to the reader it could be assigned a visible name that would be more descriptive.
This is done with the “Place Net Alias” function. A name is entered and inserted on the wire.
These net lists are very important when using Layout to create a PCB.
Bus:
A bus is a collection of wires used for a similar function.
This feature is very popular in digital schematics to make them easier to read and faster to draw.
For example instead of drawing 16 address lines A0 through A15 to every memory chip in a digital design, you could draw one bus (thick line) named address.
You would then use bus entry symbols to show wires entering or leaving the bus.
Each entry symbol would be labeled with the correct wire ID (A4 for example).
Using buses will make the schematic much cleaner and easier to read.
Multiple page schematics:
Schematics can be more then one page. Use OFF-PAGE CONNECTORS to link signals from one page to the other.
A project can also be made up of several schematics.
General Schematic Rules:
In general you want your circuit to flow from left to right. So try and put your inputs on the left and outputs on the right.
For digital designs use buses to simplify the schematic.
Don’t “wire” ground or power pins point to point. Use the signal ground and VCC circle parts instead.
For important signals use the Net Alias feature to “name” the wire. This helps the reader understand the operation of the circuit.