Hide Table of Contents

Relative to Model View

A Relative to Model View is an orthographic (front, right, left, top, bottom, and back) view defined by two orthogonal faces or planes in the model and the specification of their respective orientations. You can use this view type to set the first orthographic view in a drawing to a view different than the default.

You can then create additional orthographic views with the Projected View tool.

For standard parts and assemblies, the entire part or assembly is shown in the resulting relative view. For multibody parts, (such as weldments), only the selected body is used.

To insert a relative view:

  1. Click Relative View art\DRW-RELV.gif on the Drawing toolbar, or click Insert, Drawing View, Relative To Model. The pointer changes to .

  2. Switch to a model that is open in another window, or right-click in the graphics area and select Insert From File to open a model.

  1. In the PropertyManager, under Orientation, First, select an orientation (Front, Top, Left, and so on), and select the face or plane for that orientation in the drawing view.

  1. Under Orientation, Second, select another orientation, orthogonal to the first, and select another face or plane for that orientation in the drawing view.

  1. If using a multibody part, in the PropertyManager, make selections under Scope.

  2. Click OK and return to the drawing document. The pointer changes to .

  3. In the PropertyManager, select properties then click in the graphics area to place the view.

  4. Click OK .

If the angle of the face in the model changes, the views update to maintain the orientation as originally specified.



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

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Relative to Model View
*Comment:  
*   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:




x

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
x

Web Help Content Version: SOLIDWORKS 2011 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.