PCB_Dlg-ImpedanceFormulaEditorImpedance Formula Editor_AD

您正在阅读的是 15.1. 版本。关于最新版本,请前往 PCB_Dlg-ImpedanceFormulaEditor((Impedance Formula Editor))_AD 阅读 18.1 版本

The Impedance Formula Editor dialogThe Impedance Formula Editor dialog

Summary

This dialog allows you to view and (if required) modifythe formulae used to calculate Impedance and Trace Width when using impedance-controlled routing.

Access

The dialog is accessed from the PCB Editor by clicking the Impedance Calculation button in the Layer Stack Manager dialog. The latter is accessed by choosing Design » Layer Stack Manager from the main menus.

Options/Controls

Microstrip Tab

Click this tab to access formulae used when a route has a plane layer present on only one side of it (referred to as a microstrip).

  • Calculated Impedance - this region of the tab presents the current formula used in the calculation of the routing impedance. The formula can be modified as required, either directly in-situ or through use of the Query Helper, accessed by clicking the Helper button. The default formula is:

(60/SQRT(Er*(1-EXP(-1.55*(0.00002+TraceToPlaneDistance)/TraceToPlaneDistance))))*LN(5.98*TraceToPlaneDistance/(0.8*TraceWidth+TraceHeight))

  • Calculated Trace Width - this region of the tab presents the current formula used in the calculation of the routing trace width, which is used in the impedance formula. The formula can be modified as required, either directly in-situ, or through use of the Query Helper, accessed by clicking the Helper button. The default formula is:

((5.98*TraceToPlaneDistance)/EXP(CharacteristicImpedance/(60/SQRT(Er*(1-EXP(-1.55*(0.00002+TraceToPlaneDistance)/TraceToPlaneDistance)))))-TraceHeight)/0.8

The following pair of buttons are available for each formula region:

  • Helper - click to access the Query Helper dialog with the current formula loaded ready to make changes as required. While you can modify the formula directly in its region, especially if you are proficient with the Query Language, the Query Helper provides additional support with function keywords, operators and a syntax checker.
  • Default - click to load the region with the default formula.
Note that if the plane layer is not adjacent to the signal layer then the nearest plane layer will be used in the calculations.

Stripline Tab

Click this tab to access formulae used when a route has planes present on both sides of it (referred to as a stripline).

  • Calculated Impedance - this region of the tab presents the current formula used in the calculation of the routing impedance. The formula can be modified as required, either directly in-situ, or through use of the Query Helper, accessed by clicking the Helper button. The default formula is:

(80/SQRT(Er))*LN((1.9*(2*TraceToPlaneDistance+TraceHeight)/(0.8*TraceWidth+TraceHeight)))*(1-(TraceToPlaneDistance/(4*(PlaneToPlaneDistance-TraceHeight-TraceToPlaneDistance))))

  • Calculated Trace Width - this region of the tab presents the current formula used in the calculation of the routing trace width, which is used in the impedance formula. The formula can be modified as required, either directly in-situ, or through use of the Query Helper, accessed by clicking the Helper button. The default formula is:

((1.9*(2*TraceToPlaneDistance+TraceHeight))/(EXP((CharacteristicImpedance/(80/SQRT(Er)))/(1-(TraceToPlaneDistance/(4*(PlaneToPlaneDistance-TraceHeight-TraceToPlaneDistance))))))-TraceHeight)/0.8

The following pair of buttons are available for each formula region:

  • Helper - click to access the Query Helper dialog, with the current formula loaded, ready to make changes as required. While you can modify the formula directly in its region, especially if you are proficient with the Query Language, the Query Helper provides additional support with function keywords, operators and a syntax checker.
  • Default - click to load the region with the default formula.
Note that if the plane layers are not adjacent to the signal layer then the nearest plane layers will be used in the calculations. Note also that an offset stripline configuration is not supported.

 

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

软件的功能取决于您购买的Altium产品级别。您可以比较Altium Designer软件订阅的各个级别中包含的功能,以及通过Altium 365平台提供的应用程序所能实现的功能。

如果您在软件中找不到某个讨论过的功能,请联系Altium销售团队以获取更多信息。