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1) Creating Corners

This task shows how to create a rounded corner (arc tangent to two curves) between two lines using trimming operation. You can create rounded corners between curves. Click the Corner icon

from the Operations toolbar. The possible corner options are displayed in the Sketch tools

toolbar: the Trim All Elements option command is activated by default. Select the two lines. The second line is also highlighted, and the two lines are joined by the rounded corner which moves as you move the cursor. This lets you vary the dimensions of the corner. Enter the corner radius value in the Sketch tools toolbar. You can also click when you are satisfied with the corner dimensions.

2) Creating Chamfers

This task shows how to create a chamfer between two lines trimming either all, the first or none of the elements, and more precisely using one of the following chamfer definitions:

Angle/Hypotenuse, Length1/Length2, Length1/Angle. Click the Chamfer icon from the Operation toolbar. The possible chamfer options are displayed in the Sketch tools toolbar. Trim All / First / No element. Select the two lines. Click when you are satisfied with the dimensions of the chamfer.

3) Trimming Elements

Trimming two elements: This task shows how to trim two lines (either one element or all the

elements). Create two intersecting lines. Click the Trim icon from the Operations toolbar. The Trim toolbar options display in the Sketch tools. The Trim All option is the command activated by default. Select the first line. Position the cursor on the element to be trimmed. The location of the relimitation depends on the location of the cursor.

Trimming one element: This task shows how to trim just one element. Click the Trim icon

from the Operations toolbar. Click the Trim One Element option . Select the two curves. First curve will only be trimmed by second curve.

4) Breaking and Trimming

This task shows how to quickly delete elements intersected by other Sketcher elements using

breaking and trimming operations. Click the Quick Trim icon from the Operation toolbar (Relimitations subtoolbar). The possible trim option commands are displayed in the Sketch tools toolbar. These options are Rubber In, Rubber out, and Break.

5) Closing Elements

This task shows how to close circles, ellipses or splines using relimiting operation. Click the Close

icon from the Operation toolbar (Relimitations subtoolbar). Select one or more elements to be relimited. For example, a three point arc. The arc will now be closed.

6) Complement an Arc (Circle or Ellipse)

This task shows how to complement an arc (circle or an ellipse). Create a three points arc. Click on

the arc to be complemented to select it. Click the Complement icon from the Operation toolbar (Relimitations subtoolbar). The complementary arc appears for selected arc.

7) Breaking Elements

The Break command lets you break any types of curves. The elements used for breaking curves

can be any Sketcher element. Click the Break icon from the Operations toolbar. Select the line to be broken. Select the breaking element The selected element is broken at the selection. The line is now composed of two movable segments.

8) Creating Symmetrical Elements

This task shows you how to repeat existing Sketcher elements using a line, a construction line or

an axis. Select the profile to be duplicated by symmetry. Click the Symmetry icon from the Operations toolbar. The selected profile is duplicated and a symmetry constraint is created on the

condition you previously activated the Dimensional Constraint option from the Sketch tools toolbar.

9) Translating Elements

This task will show you how to perform a translation on 2D elements by defining the duplicate mode and then selecting the element to be duplicated. Multi-selection is not available. Click the

Translation icon

from the Operation toolbar (Transformation subtoolbar). The Translation Definition dialog box displays and will remain displayed all along your translation creation. Enter the number of copies you need. The duplicate mode is activated by default. Select the element(s) to be translated. Click the translation vector start point or select an existing one. In the Translation Definition dialog box, enter a precise value for the translation length. Click OK in the Translation Definition dialog box to end the translation.

10) Rotating Elements

This task will show you how to rotate elements by defining the duplicate mode and then selecting

the element to be duplicated. Click the Rotation icon from the Operations toolbar (Transformation subtoolbar). The Rotation Definition dialog box appears and will remain displayed all along the rotation. De-activate the Duplicate mode, if needed. Select the geometry to be rotated. Here, multi-select the entire profile. Select or click the rotation center point. Select or click a point to define the reference line that will be used for computing the angle. Select or click a point to define an angle. Click OK in the Rotation Definition dialog box to end the rotation.

11) Scaling Elements

This task will show you how to scale an entire profile. In other words, you are going to resize a

profile to the dimension you specify. Click the Scale icon from the Operation toolbar (Transformation subtoolbar). The Scale Definition dialog box appears. Select the element(s) to be scaled. Enter the center point value in the Sketch tools toolbar or click the center point on the geometry. Enter Scale Value in the displayed Scale Definition dialog box. Selected elements will be scaled according to scale factor.

12) Offsetting Elements

This task shows how to duplicate an element of the following type: line, arc or circle. Click the

Offset icon from the Operations toolbar (Transformation subtoolbar). There are two possibilities, depending on whether the line you want to duplicate by offset is already selected or not: If the line is already selected, the line to be created appears immediately. If the line is not already selected, select it. The line to be created appears. Select a point or click where you want the new element to be located. The selected line is duplicated. Both lines are parallel.

You can also apply one or more offset instances to profiles made of several elements. You can offset elements by using tangency propagation or point propagation, by creating an offset element that is tangent to the first one, by creating several offset instances.

13) Projecting 3D Elements onto the Sketch Plane

This task shows how to project edges (elements you select in the Part Design workbench) onto the

sketch plane. Click the Project 3D Elements icon from the Operations toolbar (3D Geometry subtoolbar). Multi-select the edges you wish to project onto the sketch plane. The edges are projected onto the sketch plane. These projections are yellow.

14) Intersecting 3D Elements with the Sketch Plane

This task shows how to intersect a face and the sketch plane. Select the face of interest. Click the

Intersect 3D Elements icon from the Operations toolbar (3D Geometry subtoolbar). The software computes and displays the intersection between the face and the sketch plane. The intersection is yellow.

15) Creating Silhouette Edges

This task shows how to create silhouette edges to be used in sketches as geometry or reference

elements. Click the 3D Silhouette Edges icon from the Operation toolbar (3D Geometry subtoolbar). Select the surface. The silhouette edges are created onto the sketch plane. These silhouette edges are yellow if they are associative with the 3D. You cannot move or modify them but you can delete one of them which means deleting one trace independently from the other.

Cutting the Part by the Sketch Plane

This task shows how to make some edges visible. In other words, you are going to simplify the sketch plane view by hiding the portion of material you do not need for sketching. Select the plane on which you need to sketch a new profile and enter the Sketcher workbench. Click the Cut Part by

Sketch Plane icon on the Tools toolbar to hide the portion of part you do not want to see in the Sketcher. You can now sketch the required profile.

Customizing for Sketcher

Select the Tools -> Options command to display the Options dialog box. The Options dialog box appears. Expand the Mechanical Design option, and then click Sketcher. The Sketcher tab appears, containing the following sets of options: Grid: options available Display, Primary spacing, Graduations, Snap to point and Allow Distortions Sketch Plane: options available Shade sketch plane, Position sketch plane parallel to screen. Geometry: options available Create circle and ellipse centers. Constraints: options available Create detected constraints Colors: options available Visualization of diagnostic.