Express PCB With Free Software. Express PCB tutorial leads you through the design of a PCB using layout software from ExpressPCB, which is freeware available. Before beginning you should make sure your computer has both Express PCB and ExpressSCH, if not than you should download the software. PCB software and PDF given below.
Open ExpressSCH to create schematic Diagram.
The first time you start ExpressSCH you will get a dialog box with a link to a quick start guide for ExpressSCH. This can be useful if you want to get a general overview for the tool. Once you are ready to start, close the dialog box to view the empty schematic.
- Click on Op-Amp-like symbol to place components.
- We get Component Library.
- Select Your component.
- To place the resistors, select in the text box in the upper right corner.
- Right click on a resistor and choose “Set component properties.”
- In the Component Properties box, under “Component ID,” select “Auto assign Part ID.”
- The program should assign this resistor to be R1.
- Rotate R1 by right clicking on it, selecting “Rotate component” and then “Body left 90º”
Now add the capacitor, potentiometer, comparator, and transistor to the circuit by first clicking back on the component placement tool (the red op-amp symbol) and using the component names “Capacitor polarized,” “Potentiometer,” “IC DIP-8,” and “Semiconductor – Transistor NPN.” Use “set component properties” to assign all of these parts Part IDs, label them and position them.
- Connect all components as per your diagram by clicking Track key.
- Use zoom to check all connections.
- Save your diagram.
Create Layout with ExpressPCB
Open ExpressPCB, When you first open the program, a dialog box appears with links to the Quick Start Guide and aPCB Design Tips file. If you have time, both of these links can be instructive. Once you’re ready to continue, hit OK to go to a new file.
The yellow line on the screen shows the boundary for the PCB. The default boundary is 3.8 x 2.5 inches, which matches the express PCB. This demo will use the entire board—however for our class project you should only use half the board (1.9” x 2.5”) so that we can double up designs.
Also, be aware that no copper (pads or traces) can be placed closer than 0.025″ to the perimeter of the board.
Let’s start with the resistors. Select the component placing tool, which looks like a little IC, and from the pull-down menu on the upper right.
- choose “Resistor-0.25 watt (lead spacing 0.4 inch).”
- (This description matches the small resistors in Ri-024).
- Put resistors on the schematic.
- A capacitor with the description “Cap – radial electrolytic – Lead spacing 0.2 inch” and give it part ID, “C1” (notice how the square pad denotes the positive lead)
- A transistor with the description “Semiconductor – TO-39” and give it part ID, “Q1”
- A potentiometer with the description “Potentiometer – Bourns series 3386H” and give it partID, “R1”
The holes have a diameter of 0.035”, which corresponds to 0.89 mm.
This could be a little tight for our buzzer, where the pin diameter is specified as 0.8 +/- 0.1 mm. Pull down on the “pad type” menu and select ‘0.100” square pad with 0.046” hole’ which gives us a little clearance.
(You need to make the pad and hole large enough that it the part will fit considering tolerances on pin dimension and placement, but if you make the holes too big it will be harder to solder the part in place a beginner should err on the side of making the hole too large).
One thing that you must consider when drawing connector lines is the current capacity of the lines on the board. Here are some general rules of thumb on line widths from the ExpressPCB.
Track size with current Ratings.
- 0.010″ 0.3 Amps
- 0.015″ 0.4 Amps
- 0.020″ 0.7 Amps
- 0.025″ 1.0 Amps
- 0.050″ 2.0 Amps
- 0.100″ 4.0 Amps
- 0.150″ 6.0 Amps
Most of our circuits will not draw more than 100 mA, so any line width should be acceptable. However, if your circuit uses a component that draws a significant current, such as a motor, than you should err towards larger line widths.
Let’s begin with the +9V lines. Use the net tool to highlight the +9V net on your board. Then click on the wire tool and select the upper metal (red) layer, and a 0.1” trace width (this is overkill, but it’s a good habit to make the power lines fat). Connect the + terminal of the battery to the top of the buzzer.
Use the network tool to highlight the ground connections. Right-click on the ground pad for the battery. Select “Bottom layer pad shape” and then “Thermal pad to filled plane.” This will link that pad to the ground plane. The thermal pad has some thermal isolation between it and the rest of the plane, which will make it easier to solder later.
- For your own circuit, you should also add your initials in an unused corner of the chip.
- Do these initials in the top metal (red) layer rather than in the silkscreen (yellow) layer, because if we use mini-boards, the silkscreen layer is not included.
- To add text, select the text tool, select the layer where you want the text to appear, and enter the text in the box on the upper right.
- Then click on the layout to place the text.
- Carefully inspect your circuit board.
- Use the layer visibility tools in the bottom left corner to turn off and on layers.
- Zoom in to check for connections.
- Highlight all of the pads with the network tool on to verify that they are correctly connected.
- Print out your circuit and confirm that every connection specified in the schematic is present.
- With circuit boards, you definitely want to measure twice and cut once.
- At this point, you would be ready to submit the circuit.
- DOWNLOAD SOFTWARE: Click here
- Thanks to: www.expresspcb.com