Hide Table of Contents

Editing a Table View

In this example, you edit a saved table view and:

  • Rename a sketch feature
  • Add a sketch dimension
  • Move a column
  • Unconfigure a parameter
  1. In the ConfigurationManager, expand Tables .

    The table you just created (Material) appears with two others that were saved previously.

  2. Right-click Base and click Show Table.

    The table view opens in the Modify Configurations dialog box. It contains three dimensions from Sketch1.

  3. In the dialog box, double-click Sketch1.

  4. Type Base Sketch and press Enter.

    The sketch name changes to Base Sketch in the dialog box.

  5. Click Apply.

    The sketch name updates in the FeatureManager design tree.

    Now add another sketch dimension.

  6. Beside Base Sketch, click , select J, and click in a blank area.

    A column for J appears, and the dimension appears in the graphics area.

  7. Under J:
    1. For 20, type 90 and press Enter.
    2. For 25, type 100.
  8. Click Apply.

    Now rearrange columns in the table.

  9. Select the column heading J, drag the column and drop it to the left of column L.

    Now unconfigure a parameter.

  10. Click column heading N.

    The dimension appears in the graphics area.

  11. Right-click column heading N and click Unconfigure.

    The active configuration's value for N is applied to all configurations.

  12. Click Save table view .
  13. Click OK.

    12.5 20 25

Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

Subject:   Feedback on Help Topics
Page:   Editing a Table View
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:


We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again

Web Help Content Version: SOLIDWORKS 2010 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.