Saturday, June 11, 2011

Understanding and Using Sketch Linetypes and Geometry

Platform: Autodesk Inventor Professional


Level of difficulty: Beginners.



Author: Ndianabasi Udonkang



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In Autodesk Inventor, sketch linetypes are used to further enhance the capturing of design intent in the 2D sketch environment. Sketch geometry such as lines, circles, arcs, ellipses, rectangles, polygons, and splines can be assigned different linetypes for different purposes. There are four types of linetypes in Autodesk Inventor, namely:


  1. Normal linetype;
  2. Construction linetype;
  3. Reference linetype; and
  4. Centerline linetype.

Each of these linetypes, when assigned to geometry in the sketch environment, gives rise to the four types of sketch geometry, namely:


  1. Normal sketch geometry;
  2. Construction geometry;
  3. Reference geometry; and
  4. Centerline geometry.

 


Figure 1



Normal Linetype and Geometry


When geometry is initially sketched, it appears with a continuous linetype. This is called normal sketch geometry. The normal linetype is the default linetype for sketch geometry unless the centerline or construction linetypes tools have been activated on the Format panel of the Sketch tab. Normal linetypes are primarily used for defining profiles, path, and guide rails for sketched features. [Note: Sketched features are those features that are derived or generated from sketches. They include extruded, revolved, lofted, and swept features.]


Figure 2



In Figure 2, a sketch, consisting mainly of normal linetype geometries, is shown.



Construction Linetype and Geometry


The construction linetype is used to represent geometry that would not directly participate as profile, path, or guide rails of sketched features. Construction geometry is used for as aid for constructing and constraining normal geometry. Construction geometry is vital in capturing design intent. For example in Figure 3, a construction line is used to define the size of the entry slot of a machine clip.


Figure 3


Creating Construction Geometry


Use the following steps to create construction geometry.


  1. In the Sketch environment, go to Sketch tab > Format panel and click the Construction tool.
  2. On the graphics windows, create any geometry your choice, the geometry will be displayed as a construction geometry.
  3. Deactivate the construction geometry mode by clicking on the Construction tool on the Format panel and continue drawing normal geometries.

Converting Existing Geometry to Construction Geometry


If you’ve already drawn geometry and you wish to convert it to construction geometry, follow these steps.


  1. On the graphics window, select the geometry you want to convert to construction geometry.
  2. Go the Sketch tab > Format panel and click the Construction tool. The geometry is converted to construction geometry.

This method is the fastest and ensures that you do not forget to deactivate the construction mode when using the first method.


Figure 4



Centerline Linetype and Geometry


The centerline linetype is used for creating centerline geometry. When centerline geometry is placed in a sketch, it is automatically recognized by the Revolve tool as the “Axis of Revolution.” When a dimension is placed between a centerline geometry and other geometries, a diameter dimension is automatically created.


Figure 5



Creating Centerline Geometry


Use the following steps to create construction geometry.


  1. In the Sketch environment, go to Sketch tab > Format panel and click the Centerline tool.
  2. On the graphics windows, create any geometry your choice, the geometry will be displayed as a centerline geometry.
  3. Deactivate the centerline geometry mode by clicking on the Centerline tool on the Format panel and continue drawing normal geometries.

Figure 6



Converting Existing Geometry to Centerline Geometry


If you’ve already drawn geometry and you wish to convert it to centerline geometry, follow these steps.


  1. On the graphics window, select the geometry you want to convert to centerline geometry.
  2. Go the Sketch tab > Format panel and click the Centerline tool. The geometry is converted to Centerline geometry.


Reference Geometry


Reference geometry is created by projecting part faces, edges, and vertices onto the current sketch plane. Sketch geometry belonging to another sketches and work features ( such as work point and work axis) can also be projected to the current sketch. Reference geometry is the best way to ensure that a sketch is linked parametrically to an already existing part or sketch. Reference geometry remains associative to the original part vertices, edges, faces, and work features. Reference geometry can be used to define the profile or path for a sketched feature.


Properties of Reference Geometry


  1. Reference geometry cannot be dimensioned.
  2. It cannot be trimmed
  3. It can be mirrored
  4. It cannot be drawn. However, it can be created by using the Project Geometry tool or activating the Autoproject Edges option on the Application Option dialog box.

Creating Reference Geometry


Autoproject Options


Reference geometry is created automatically when you use a planar face of an existing part as the sketch plane. The edges of the selected face are projected on to the new sketch, but this depends on the Autoproject Options on the Application Option dialog box. To activate the Autoproject Option, follow these steps.


  1. On any environment, go to the Ribbon > Tools tab > Options tab > Application Options tool.
  2. On the Application Options dialog box, click on the Sketch tab and go to the lower section. Check the checkboxes with the labels: “Autoproject edges for sketch creation and edit” and “Autoproject edges during curve creation.”
  3. Click Apply and close.

Figure 7



Figure 8



 


Autoproject edges during curve creation


When this checkbox is activated on the Application Options dialog box, edges of existing parts can be projected on to sketch plane during sketching by hovering the cursor over them.


Autoproject edges for sketch creation and edit


When this checkbox is activated on the Application Options dialog box, the edges of planar faces are projected on to the current sketch plane.


Project Geometry Tool


The Project Geometry tool is used to project additional part faces, edges, vertices, and work features on to the sketch plane as reference geometry. When the Project Geometry tool is launched, you are asked to select the faces, edges, vertices, or work features that will be projected. One selected, the reference geometry is created on the current sketch plane which remain associative with the original faces, edges, vertices, or work features. By being associative, it means that the reference geometry depends on the original faces, edges, vertices, or work features and will update if they are changed.


To create reference geometry using the Project Geometry tool, follow these steps:


  1. On the Sketch tab of the sketch environment, go to Draw panel > Project geometry tool.
  2. Select the faces, edges, vertices, and/or work features of interest. Reference geometry is created on the current sketch plane.

Figure 9


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