Configuring PCB Accordion Object Properties in Altium Designer

Parent page: Accordion

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 Accordion object properties are available for editing in the Properties panel when an Accordion is selected in the workspace.

The Accordion mode of the Properties panel

Net Information

• Net Name - displays the name of the net.
• Net Class - displays the net class.

Target Length

• Source
  • ​Manual - enter the length in the Target Length 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 Length - displays the target length being defined by the rules. Note that the most stringent combination of the rules is used.
  • ​Clip to Target Length - enable to ensure that the final length does not exceed the target length. When enabled, the Amplitude and Gap values are automatically adjusted to achieve the target length.

Pattern

• Style - this region is used to select the current amplitude wave pattern. There are three pattern styles: Mitered Lines, Mitered Arcs, and Rounded. The PCB Editor will attempt to match the target length by adding segments to the length according to the defined target length. The region below updates accordingly to show the currently selected pattern style.
  The Rounded style is the most compact and Mitered Lines is the least compact
• ​Max Amplitude - shows the current maximum allowed amplitude of tuning segments. Edit this field to change the maximum allowable amplitude, which can be defined in either mm or mil units. To specify the units when entering a number, add the mm or mil suffix to the value. You also can use the - or + to decrease or increase the value. The Increment field displays the current increment when you increase or decrease the value and can be edited as required. 
• Gap - shows the current distance between "legs" of the amplitude pattern. Edit this field to change the gap, which can be defined in either mm or mil units. To specify the units when entering a number, add the mm or mil suffix to the value. You also can use the - or + to decrease or increase the value. The Increment field displays the gap size increment when you increase or decrease the value and can be edited as required. 
• Miter - shows the miter (corner) value of the pattern. Edit this field to change the value. You also can use the - or + to decrease or increase the value. The Increment field displays the miter percentage increment when you increase or decrease the value and can be edited as required.