Configuring PCB Sawtooth Object Properties in Altium Designer

Parent page: Sawtooth

PCB Editor object properties are definable options that specify the visual style, content, and behavior of the placed object. The property settings for each type of object are defined in the following way:

• Post-placement settings – all Sawtooth object properties are available for editing in the Properties panel when a Sawtooth is selected in the design space.

   

Net Information

• Net Name – the name of the selected net.
• Net Class – the name of the selected net class.
• Total
  • Length – the total Signal Length. The Signal Length is the accurate calculation of the total node-to-node distance. Placed objects are analyzed to resolve stacked or overlapping objects and wandering paths within pads; and via lengths are included. If the net is not completely routed, the Manhattan (X + Y) length of the connection line is also included. For more information regarding Signal Length and its applications, see the PCB – Nets page.
  • Delay – the delay of the routed segments of the Total Length.
• Selected
  • Length – the total length sum of the selected segments.
  • Delay – the total delay of the selected segments, including those unrouted.

Target

• Source
  • Manual – enter the length in the Target field. The Recently Used Lengths region keeps track of the values you have entered so that you can use them again.
    • Recently Used Lengths – lists the recently used manual target lengths that you can use to define the Target length value. The currently selected length value is shown in the Target Length field.
  • From Net – choose a net from the displayed nets. The length of the chosen net will become the target, however, it will be overridden if there are more restrictive design rules defined.
    • List Nets – lists the net names and their lengths on the current PCB according to their class. The currently selected net length value is shown in the Target Length field.
  • From Rules – you need to have one or both of the Length and Matched Length design rules defined to use this mode. Altium Designer will then obey the most stringent combination of these rules.
    • List of Rules – lists the length rules for the current PCB document. The currently selected rule maximum length value is shown in the Target Length field.
• Target – displays the target length being defined by the rules. Note that the most stringent combination of the rules is used.
  • Clip to Target – enable to ensure that the final length does not exceed the target length.

Pattern

• Angle – displays the slope of the leading and trailing tooth edges, relative to the original route path of the net being tuned.
• Tooth Width – displays the width of the top of the tooth.
• Min Joint – displays the minimum length of the first colinear track segment placed before the first tooth is created.
• Min Height – displays the minimum allowable tooth height.
• Actual Height – displays the current tooth height, measured from the centerline of the original route path being tuned, to the centerline of the tooth's top track segment. Press the or shortcut keys to interactively decrease/increase the actual height of the sawtooth during placement.
• Step – the increment value which the Actual Height field is decreased/increased by when using the or shortcut keys during sawtooth placement or clicking the buttons at the right of the Actual Height field.
• Single Side – enable to create the tuning pattern so that it only projects in one direction from the original route path. Press the S shortcut during placement or interactive editing to toggle the option on or off.
• Fixed Size – enable to fix the Sawtooth Height to the current height and to remove any teeth that are not at that fixed size.