I imported the schematic into eagle, replaced the components with their SMD equivalents, and routed the board manually in board mode. .brd is the board format for eagle. I don't really recommend newcomers to power electronics to design PCBs. Aside from thermal considerations, the high current from the power-carrying traces must be isolated from the traces which carry the high frequency signals from the switching regulator. Otherwise, EMI will be induced into the power lines, not very good for the load.
I discovered rather recently my board design is rather flawed. For one, it could have encompassed more copper on it, like ground plains, to aid in heat dissipation. Non-power and signalling traces can also be made with a smaller width, to aid in reducing EMI. The signalling traces must also be supplied with their own dedicated ground paths, the ground paths must not carry power current. Lastly, I designed the HF signals too close to the power traces. A killer for any device without noise filtering that connects to it. A good design will be something like this:
Basically, empty spaces are just blank copper and are left alone or connected to VCC or GND. All commercial PCBs manufactured, especially products involving HF signals, have similar designs. Some even has tiny holes drilled into them grid style, and vias connecting them to the other layers, which effectively turns the copper plains into a heatsink!
I've built the board over my free time last year as a second year electrical engineering student. I never even looked at the datasheet for the LT1302 and was totally clueless with what I was doing. However, I've learnt much over the year - my PCB designs of the previous were very flawed, with no thermal and EMI considerations.
Compare my board design to the reference design from the LT1302 datasheet:
Clearly, it shows just how clueless I was when I was routing the PCB. An obvious mistake is with the long and thick traces coming from the battery. Not only is there an added impedance, I believe the traces will also either emit EMI or act as an antenna to external EMI.
To quote a very important section on layout and thermal considerations from the datasheet:
The high speed, high current switching associated with the LT1302 mandates careful attention to layout.
...High current functions are separated by the package from sensitive control functions. Feedback resistors R1 and R2 should be close to the feedback pin (pin4). Noise can easily be coupled into this pin if care is not taken. A small capacitor (100pF to 200pF) from FB to ground provides a high frequency bypass.
...The 0.1µF ceramic bypass capacitor C3 (use X7R, not Z5U) should be mounted as close as possible to the package.
...Grounding should be segregated as illustrated. C3’s ground trace should not carry switch current. Run a separate ground trace up under the package as shown. The battery and load return should go to the power side of the ground copper.
...For surface mount devices heat sinking is accomplished by using the heat spreading capabilities of the PC board and its copper traces. Experiments have shown that the heat spreading copper layer does not need to be electrically connected to the tab of the device. The PCB material can be very effective at transmitting heat between the pad area attached to pins 1 and 8 of the device, and a ground or power plane layer either inside or on the opposite side of the board. Although the actual thermal resistance of the PCB material is high, the length/area ratio of the thermal resistance between the layer is small. Copper board stiffeners and plated through holes can also be used to spread the heat generated by the device.