Adding Drawing Views

The first view will be an unassociated general view.  It is likely it will be an orthographic view from which you can create projected views.  The view will need to be oriented using the Geometric References or Angles options.

Double-click a view to change its properties.

 

Types of Views

A – initial view unassociated to any other view – General view

B – Projected view from A

C – Projected view from A then sectioned – section arrows in A

D – Detailed view magnifying the area indicated in A

E – Isometric view – created as a General view

F – Auxiliary view projected from a chosen, non orthographic reference

2000.view.types

 

Line display

Part drawing – always show hidden line except in isometric views

GA – no hidden line

 

General (orthographic) – A view that you orient and is not dependent upon any other view for its orientation.

 

 

  • RMB in the graphics area > Insert General View…
  • pick a position for the view
  • select planar references (surfaces or datum planes) to face to Front and Top
  • momentary RMB to toggle through selectable references
  • change direction to Front, Back, Top or Bottom to change reference direction

 

Projection – An orthographic projection of an object as seen from the front, top, right, or left.  First or third angle?

 

 

 

Section – a cross sectional view is often needed to clarify and annotate internal detail – remember, never dimension hidden detail, dimension the cross section.  A perpendicular datum plane in the parent view is used as the ‘cutting’ plane to allow a projected view to be showed in Cross Section (xsec)

 

 

Before creating a section view, set up a Cross Section in the view manager in the model file.

To show the view as a cross-section, use the View Properties> Sections options.

Adding section arrows

Arrows are needed in the parent view to show the position of the cutting plane.  Pick the xsec view > RMB and choose add arrows > choose the view to which to add the arrows.

 

Detailed – A view that you create by taking a portion of an existing view and scaling it for dimensioning and clarification purposes. The boundary for the detailed view can be a circle, ellipse (with or without a horizontal or vertical major axis), or a spline.

 

 

Common tab > Views or Layout tab> Model Views

Read the bottom text area for prompts

  • pick a point on the part to show the centre of the detailed area
  • you are prompted to draw a spline curve to represent the extents of the detailed area
  • DON’T start the spline tool from the sketch toolbar, just pick 4 points to define the detailed area.
  • MMB to finish the spline
  • pick a position to place the view
  • change the scale accordingly

 

Auxiliary – A view created by projecting 90 degrees to an inclined surface, datum plane, or along an axis.

 


 

General (isometric) – An isometric view can help us better visualise the 3D form.  Use the orient view icon in the part file to create an appropriate view or the view orientation area of the view properties dialogue box to create your view.  Rotate around the vertical axis 45 degrees, rotate around the horizontal axis 35 degrees.

 

 

 

 

Specifying how much of the model is visible in a View

Using other options in the View Properties > View Type options, you can specify how much of the model is visible in the view.

 

Full View – shows the entire model – default setting

Half View – shows only the portion of the model on one side of a datum plane

Useful for saving space when you have a symmetrical model

 

Broken View – removes mid section from of a model between two points and moves the remaining sections close together.

Generally used to save space and increase view size when you have a long thin volume with a uniform section

 


Partial View – shows only the portion of the view that is contained within a boundary

 

 

Line display

The settings wireframe, hidden line, no hidden line or shaded will affect the way your view are displayed.  Showing hidden detail is the preferred option, but if this makes the view unreadable because of an extreme amount of internal detail then use no hidden line – make sure you are consistent in any associated views

The line display setting can be controlled independently within each view through the view properties window.  Isometric views are generally not shown with hidden line detail, their main function is to show the general form.

 

Deleting unwanted lines

Common situation is when you have a mirrored part with normalcy across the symmetry plane or merged surface patches at G2/curvature continuous – this will create tangent/patch edges which shouldn’t be there as there is no abrupt change in radius.

Also, stray, random lines can be created if the system cannot fully resolve the geometry.

Layout tab > Edit > Edge Display > Erase Line