AWR eBooks

RF Electronics Chapter 11: Circuit Manufacture Page 371 2022, C. J. Kikkert, James Cook University, ISBN 978-0-6486803-9-0. Other Substrates Ceramic materials with higher dielectric constants are used to reduce the size and thus weight of resonators used for oscillators and filters. Dielectric resonator oscillators (DRO) [10, 11] are used in LNCs for satellite receivers. The LNC in figure 11.5 has a dielectric resonator oscillator mounted on the other side of the PCB shown in figure 11.5. The diplexer shown in the left of figure 11.3 and the cavity filters in figure 7.98 are examples. Manufacturing RF printed circuit boards can be designed in a similar way to conventional PCBs, so that programs like Altium (formerly known as Protel) [12], Allegro [13] or Autodesk's (formerly CadSoft) Eagle [14] can be used to produce the circuit board layout. For circuits like Stripline filters, and other RF circuits, where the characteristics and lengths of transmission lines are critical, then software like Cadence AWR DE or Keysight is required. AWR DE can produce GDSII, DXF and Gerber plot files. GDSII file format is an industry standard file format for IC layout artwork and DXF is a vector file format developed by Autodesk (AutoCAD), for exchanging files between CAD software. Gerber ASCII vector files were initially developed by Gerber Systems Corp to drive their vector photo plotters. The Extended Gerber files include all the information, like board layer type, drill, solder mask and overlay detail, required to produce a complete PCB. They are the default file type used to produce prototype RF boards, either by commercial PCB manufacturers, or by the milling machines used by many universities for prototypes. The Gerber plot files can also be imported into most PCB layout software and Gerber plot files can be imported into AWR DE, to produce a combined RF and conventional PCB. Such technology is required for the multilayer boards shown in figure 11.6. Importing plot files into AWR DE allows those imported layers to be included in EM simulation. Normal PCBs are protected using a solder-mask. Unless the thickness and the properties of the dielectric of the solder-mask is taken into account in designing the RF circuit, solder-masks should not be used for RF boards. Instead, to prevent corrosion, Gold plating is normally used on the RF circuits as shown in figure 7.67. Layout Hints Many PCB manufacturers can etch to a specified accuracy. Typical values for the thinnest track widths and spacing that can be made on FR4 are 0.1 mm (0.004"). For High frequency laminates like RO4003C, track widths and spacing of 0.051 mm (0.002") are possible. Larger values > 0.15 mm are desirable and will reduce costs. [15, 16]. Ensure the tracks can handle the required current. Note 0.001" is called thou in the UK and other countries, and mil in the USA. In Europe mil is an abbreviation of a millimetre and it is also a measurement of angle. To avoid this confusion mil is not used in this book. Many of the modern ICs have 0.5 mm pitch of the leads on the IC. The 0.5 mm track pitch can easily be achieved using present day PCB manufacture. The smallest drill size that can be used is typically 0.15 mm diameter. Drilling holes smaller than 0.3 mm increases the cost per hole. The smallest pad size for vias or leaded components, which should be used is the drill size plus 0.5 mm, however small pads will lift off easily when components are soldered to them. For through-hole components use a drill size that is approximately 0.1 mm larger than the lead size and use a pad that is approximately 1 mm larger than the drill size. The recommended hole size for a standard RF Electronics: Design and Simulation 371 www.cadence.com/go/awr

• Cover