You are here

How to generate a cross section drawing for documentation purposes



Launching the utility

Use model

Detailed description

Include options


Conductor and Dielectric drawing options


Cross Section Generator is an application which gives customers the ability to generate a cross section drawing for documentation purposes. This document describes the features and use model of this toolkit.

Cross Section Generator covers the following aspects:

  • Generation of cross section documentation view in the layout database

  • Customizable content

    • Layer Name

    • Layer thickness (including total thickness)

    • Layer material

    • Via stack and via labels

  • Various graphics options

    • Symbol size, extra row/column spacing

    • Fill Scaling of layer thicknesses for better readability

  • Configuration stored in database


    Figure 1: Cross Section Generator


Launching the utility

Cross Section Generator can be started from Pulldown menu or by entering the command

tbx xsecgen in the console window.

Once the command has been launched a form appears.


Figure 2: Cross Section Generator main form


Use Model

The basic use model is as follows:

  • Launch PCB Editor.

  • Choose command Cross Section Generator

  • Specify the contents to be displayed besides the cross section geometry, e.g. layer name and layer thickness.

  • Click Preview

    A rectangle is attached to the cursor indicating the final size of the cross geometry including the selected label information. This will help you to work out the size of the

    complete geometry.


    Figure 3: Size preview

  • In PCB Editor choose RMB - Clear Preview in order to disable the preview.

  • Change parameters again if appropriate (e.g. symbol width in the Parameter section)

  • Click Generate

    Again, a rectangle is attached to the cursor indicating the final size. But now use LMB to specify the upper left location of the cross geometry.

  • The cross section is generated at the specified location. Behind the scenes Cross Section Generator creates a format symbol and places an instance in the database.

    Note: Using Edit – Move (find filter on symbols) you can move the cross geometry to another location. Cross Section Generator takes an existing symbol into account and updates the geometry at the same location with the new settings.

    Note: All settings are stored in the database. Cross Section Generator always reads settings from database first. Using Save to file and Load from file it’s possible to export and import configurations from other databases.


    Figure 4: Cross Section Generator example

    Note: Graphics data and text labels are written to MANUFACTURING

    subclasses Xsection_Cond, Xsection_Diel, Xsection_Via, Xsection_Via


    Figure 5: Cross Section Generator subclasses


Detailed description

Include options

Besides the basic cross section which is combination of conductor and dielectric layers additional information can be displayed.


Figure 6: Include options form


Figure 7: Include options

  • Layer name

    The name of the layer e.g. TOP, BOTTOM


    • Layer material

      The name of the material e.g. FR4, copper

    • Layer thickness

      The thickness of the conductor or the dielectric layer. If checked the total thickness is reported also.

    • Via stack

      If checked a via stack will be drawn to the drawing geometry for each via found in the design. The start and end layer is taken into account.

    • Inner pads

      Only available if optionVia stack is enabled. Using this option will alter the via stack shape in a way that a pad will be drawn also on inner layers.


      Figure 8: Via stack with and without inner pads

    • Via label

      Only available if optionVia stack is enabled. Using this option the name of the via will be added to the drawing geometry.


In this section basic drawing parameters can be specified.


Figure 9: Parameters

  • Symbol width

    Specifies the width of the basic cross section geometry which is represented only by conductor and dielectric layers.


    Figure 10: Symbol width

    • Row spacing

      Specifies an additional spacing in y direction between adjacent layers.

    • Column spacing

      Specifies the spacing in x direction between the label columns and the cross section geometry.


      Figure 11: Row and Column spacing

    • Text block

      Specifies the text block to be used for label information.

    • Scale layers

      Using this option different thicknesses are scaled which yields in a more realistic representation of the cross section. The layer with the smallest thickness will be drawn using a height specified by Min height. All other layers are scaled accordingly. Depending on the number of layers a linear scaling might not be always possible. Therefore other scaling options such “Log2”, “Log5” and “Log10” are available. The default is off, which means that all conductor layers and all dielectric layers are drawn with equal thicknesses specified by Conductor and Dielectric drawing options.


      Figure 12: Scaling options


      Figure 13: Log2 and Linear scaling example

4.3 Conductor and Dielectric drawing options

Drawing options for conductor and dielectric layers can be specified separately.


Figure 14: Conductor and Dielectric drawing options

  • Height

    Specifies the drawing height of the conductor or dielectric layer. The fields are only active as long as option Scale layers is inactive. In this case all conductor layers are drawn with one thickness and all dielectric layers are drawn with one thickness.

  • Style

Specifies the fill Fill, Unfill and Hatch both whereas the dielectric layers can be of type Fill, Unfill and Hatch diag.

  • Hatch width

    Specifies the line width for the hatch shape

  • Space

    Specifies the spacing for the hatch shape


    Figure 15: Conductor and Dielectric fill

    Note: The Hatch diag option for dielectric shapes will automatically alter between 45 and 135 degrees for better readability.