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Presentation Transcript

Slide 1:

Learning Objectives: Use various tools to create a geometry. Dimension a sketch. Apply constraints to a sketch . Modify a sketch. Use the Modify Dimensions dialog box. Edit geometry of a sketch by trimming. Mirror a sketch. Use drawing display options.

Slide 2:

The Sketch Mode Using the Sketch mode, you can draw a 2D sketch of the product and assign required dimensions and constraints to it. The following steps outline the procedure to use the Sketch mode: Using the Sketch Mode Sketch the required section geometry Entering the Sketch Mode Add the constraints and dimensions to the sketched section Add relations to the sketch if needed Regenerate the sketch If the Intent Manager is on while sketching then the sketch is automatically regenerated. To enter the Sketch mode, choose the Create a new object button from the File toolbar. The New dialog box will be displayed with other Pro/ENGINEER modes.

Slide 3:

When you enter the Sketch mode, the initial screen appearance is similar to the one shown in figure. This figure also shows the Sketcher Tools toolbar that will be displayed on the right of the drawing area. The buttons in this toolbar are used to draw sketches. The various drawing options are also available in the Sketch menu in the menu bar. When you enter the sketcher environment, the Intent Manager is on by default. The Sketcher Environment Initial screen appearance in the Sketch mode

Slide 4:

When you enter the sketcher environment, the Select items button is chosen by default. If this button is chosen, the sketcher environment is said to be in the selection mode. In the selection mode, you can select entities of the sketch to edit or to invoke the shortcut menu. The options in the shortcut menu can be used to apply various operations on the selected item. Working with the Sketch in the Sketch Mode

Slide 5:

To draw lines, there are three tool buttons in the Sketcher Tools toolbar. To view these buttons, choose the black arrow on the right of the Create 2 point lines button. The flyout with three tool buttons appears. Drawing a Line Placing a Point Drawing a Sketch Using the Sketcher Tools Toolbar When you are in the sketcher environment, the Sketcher Tools toolbar on the Right Toolchest , contains the tools to draw, dimension, and modify a sketch. Choose the Create points button from the Sketcher Tools toolbar to place a point. One of the applications of a point is that it is used to dimension a sketch if placed at the corners of the sketch.

Slide 6:

Drawing a Line Using the Create 2 point lines Tool Drawing a Line Using the Create lines tangent to 2 entities Tool Drawing a Centerline Using the Create 2 point centerlines Tool Drawing a Rectangle The Create 2 point lines button is used to create a line by selecting two points in the drawing area. The Create lines tangent to 2 entities button is used to draw a tangent between two entities such as arcs, circles, or a combination of these. You can draw horizontal, vertical, or inclined centerline using the Create 2 point centerlines button. Choose the Create rectangle button from the Sketcher Tools toolbar to draw a rectangle.

Slide 7:

To draw a circle there are four tools and one tool to draw an ellipse in the Sketcher Tools toolbar. To view the tools available to draw circles and ellipses, choose the black arrow on the right of the Create circle by picking the center and a point on the circle button. The flyout with five buttons appears. Drawing a Circle Drawing a Circle Using the Create circle by picking the center and a point on the circle Tool As the name suggests, the Create circle by picking the center and a point on the circle tool is used to draw a circle by specifying the center of the circle and a point on it.

Slide 8:

Sketch of a flange Drawing a Construction Circle A construction circle is a circle that is used to align entities, create diametrical or radial dimensioning, and to reference entities. To create a construction circle, draw a circle and then hold down the right mouse button on it to invoke the shortcut menu as shown in figure. Choose the Construction option from the shortcut menu. The Construction option in the shortcut menu

Slide 9:

Drawing a Circle Using the Create concentric circle Tool Drawing a Circle Using the Create circle by picking its 3 points Tool Drawing a Circle Using the Create a circle tangent to 3 entities Tool Drawing an Ellipse Using the Create a full ellipse Tool To draw a concentric circle, choose the Create Concentric circle button. After selecting this button you need to select a curve to determine concentricity. To draw a circle by selecting three points, choose the Create circle by picking its 3 points button. The Create a circle tangent to 3 entities tool is used to draw a circle that is tangent to three existing entities. This tool references other entities to draw a circle. Choose the Create a full ellipse button from the flyout in the Sketcher Tools toolbar to draw an ellipse.

Slide 10:

To draw an arc, there are five tool buttons in the Sketcher Tools toolbar. To view them, choose the black arrow on the right of the Create an arc by 3 points or tangent to an entity at its endpoint button. The flyout appears with five buttons. Drawing an Arc Drawing an Arc Using the Create an arc by 3 points or tangent to an entity at its endpoint tool The Create an arc by 3 points or tangent to an entity at its endpoint tool is used to draw arcs tangent from the endpoint of an existing entity or by defining three points in the drawing area. Figure A and B shows the creation of an arc using the Create an arc by 3 points or tangent to an entity at its end point.

Slide 11:

Drawing an Arc Using the Create concentric arc Tool The Create concentric arc tool is used to draw an arc concentric to an existing arc. You will have to select an entity to which the arc will be concentric. The entity selected must be an arc or a circle. Figure A Figure B

Slide 12:

Drawing an Arc Using the Create an arc by picking its center and endpoints Tool Drawing an Arc Using the Create an arc tangent to 3 entities Tool Drawing an Arc Using the Create a conic arc Tool Choose the Create an arc by picking its center and endpoints button to draw an arc by selecting its endpoint. The Create an arc tangent to 3 entities tool is used to draw an arc that is tangent to three selected entities. The Create a conic arc tool is used to draw a conic arc.

Slide 13:

After you draw a sketch, the next step involves the dimensioning of the sketch. The basic purpose of dimensioning in Pro/ENGINEER is to control the size of the sketch and to locate it with some reference. The Create defining dimension button is used to manually dimension the entities. You can also choose Sketch > Dimension to display a cascaded menu as shown in Figure A . Dimensioning the Sketch Dimensioning a Sketch Using the Create defining dimension Button or the Normal Option The Create defining dimension tool is used for normal dimensioning of sketch. Figure A Dimensioning options

Slide 14:

Linear Dimensioning of a Line Dimensioning the Basic Sketched Entities To add linear dimension to a line, select it or its end points. Then press the middle mouse button to place the dimension. Angular Dimensioning of an Arc To add angular dimension to an arc, select its ends by pressing Of the arc by pressing the left mouse button and then select a point on the arc. Angular dimensioning technique Approximate locations of the cursor to achieve different dimensions

Slide 15:

Diameter Dimensioning For diameter dimensioning, click on a circle twice. Then place the dimension at the desired location by pressing the middle mouse button Radial Dimensioning For radial dimensioning, click on the entity once. Then place the dimension at the desired location by pressing the middle mouse button. Diameter dimensioning technique Radial dimensioning technique

Slide 16:

Dimensioning Revolved Sections Dimensioning technique for revolved sections To dimension a revolved section, click on the entity to be dimensioned. Next, select the centerline about which you want the section to be revolved. Once again select the original entity that you want to dimension. Place the dimension at the desired location by pressing the middle mouse button

Slide 17:

Constraints are the logical operations that are performed on the selected geometry to make it more accurate in defining its position with respect to the other geometry. Working with Constraints Constraints dialog box Choose the Impose sketcher constraints on the section button from the Sketcher Tools toolbars to display the Constraints dialog box. This dialog box is used to apply the constraints that are listed next. Make a line or two vertices vertical Make a line or two vertices horizontal. Make two entities perpendicular. Make two entities tangent. Place point on the middle of the line.

Slide 18:

Create same points, points on entity or collinear constraint. Make two points or vertices symmetric about a centerline. Create Equal Lengths, Equal Radii or Same Curvature Constraint. Make two lines parallel. The Explain option of the Constraints dialog box provides information about the constraints that are applied to a sketch. Explain Option

Slide 19:

The need to disable a constraint arises when you are drawing an entity. For example, if you draw a circle at some distance apart from a circle, the system tends to apply the equal radius constraint when the sizes of the two circles become equal. If at this moment you do not want to apply the equal radius constraint, right-click to disable the equal radius constraint. Disabling Constraints Select a weak dimension or a weak constraint from the drawing area. The selected dimension or constraint is highlighted in red. Press and hold the right mouse button to invoke the shortcut menu. Choose the Strong option from the shortcut menu to make the constraint strong. Converting a Weak Constraint into a Strong Constraint Shortcut menu to convert weak Dimension to strong

Slide 20:

Modifying the Dimensions of a Sketch There are four ways to modify the dimensions of a sketch. These methods are listed next. Using the Modify Dimensions dialog box Modify Dimensions dialog box You can select one or more dimensions from the sketch to modify. When you select dimension(s) from a sketch, they are highlighted in red. If you want to select more than one dimension, hold down the CTRL key and select the dimensions by clicking on them. You can also use CTRL+ALT+A or define a window to select the dimensions in the sketch.

Slide 21:

Modifying Dimensions by Double-Clicking Modify Dimensions Dynamically Using the Edit menu When you choose the Modify option from the Edit menu , a check mark appears to the left of the Modify option in the Edit menu. You can select a dimension from the sketch to modify. When you double-click on a dimension, the pop-up text field appears. Enter a new dimension value in this field and press ENTER or use the middle mouse button . When you bring the cursor to an entity, the color of the entity changes to cyan. Now, if you hold down the left mouse button, you can modify the entity by dragging the mouse. You will notice that as the entity is modified, the dimensions referenced to the selected entity are also modified.

Slide 22:

While applying constraints or dimensions, the system may sometimes prompt you to delete one or more highlighted dimensions or constraints. As soon as the conflict occurs, the Resolve Sketch dialog box will be displayed as shown in figure. Resolve Sketch Dialog Box Resolve Sketch dialog box Delete When you choose the Undo button, the section is brought back to the state that was just before the conflict occurred. The Delete button is used to delete a selected dimension or constraint that is enclosed within the yellow box. Select the dimension or the constraint to delete before you choose the Delete button from the Resolve Sketch dialog box. Undo

Slide 23:

To delete a sketched entity, select it by defining a window by dragging the cursor around the entity, the color of the selected entity changes to red. Right-click in the drawing area and hold down the right mouse button until a shortcut menu appears. Now, choose the Delete option from this menu to delete the selected item. Deleting the Sketched Entities Dim > Ref Explain To restore the last deleted item, choose the Undo button. This button is available in the Edit toolbar on the Top Toolchest . When you choose the Explain button, the system provides you with information about the selected constraint or dimension. The information will be displayed in the message area. When you choose the Dim > Ref button, the selected dimension is converted to a reference dimension.

Slide 24:

When creating a design, there are a number of places where you need to remove the unwanted and extended entities. You can do this by using the tool buttons available for trimming. Trimming the Sketched Entities Dynamically trim section entities Tool Divide an entity at the point of selection Tool The Divide an entity at the point of selection tool is used to divide an entity into any number of parts or entities by specifying points on the entity. This tool button deletes the selected entities or a portion of the entity from where it intersects.

Slide 25:

Mirroring the Sketched Entities Trim entities (cut or extend) to other entities or geometry button The Trim entities (cut or extend) to other entities or geometry button is used to trim two entities at their corners. Trimming the lines The Mirror selected entities button is used to mirror sketched geometries about a centerline. This tool button helps to reduce the time for the creation and the dimensioning of symmetrical geometric entities.

Slide 26:

Inserting Foreign Data Into The Sketch The Insert foreign data from palette into the active object tool helps you to insert certain standard or user-defined features such as polygons, profiles, shapes, stars and other previously created sketches in the sketch mode. Choose the Insert foreign Data from palette into the active object button from the Sketcher Tools toolbars, the Sketcher Palette dialog box will be displayed, as shown in figure. The options in this dialog box will be used to insert predefined shapes into the sketch. The Sketcher Palette dialog box

Slide 27:

You can enlarge or reduce the drawing display using various drawing display tools provided in Pro/ENGINEER. Drawing Display Options Zoom In Zoom Out Refit object to fully display it on the screen Redraw the current view

Slide 28:

In this tutorial, you will draw the sketch for the model shown in Figure A . The sketch is shown in Figure B . (Expected time: 30 min) Tutorial 1 Figure B Sketch of the model Figure A Model for Tutorial 1

Slide 29:

Figure C Partial sketch with weak dimensions Start a new object file. Set the working directory. Draw lines using the tool button for creating lines, see Figure C .

Slide 30:

Figure D Sketch with all the entities, weak dimensions, and weak constraints Figure E Sketch with dimensions and constraints Draw an arc and a circle using respective tool buttons, see Figure D . Dimension the sketch and then modify the dimensions of the sketch, see Figure E . Save the sketch.

Slide 31:

In this tutorial, you will draw the sketch for the model shown in Figure A . The sketch is shown in Figure B . (Expected time: 30 min) Tutorial 2 Figure B Sketch of the model Figure A Model for Tutorial 2

Slide 32:

Figure C Sketch with weak dimensions and weak constraints Figure D Sketch after dimensioning Set the working directory and start a new object file. Draw the sketch using the tool button for creating lines, see Figure C . Dimension the required entities and then modify the dimensions of the sketch, see Figure D . Save the sketch.

Slide 33:

In this tutorial, you will draw the sketch for the model shown in Figure A . The sketch is shown in Figure B . (Expected time: 30 min) Tutorial 3 Figure B Sketch of the model Figure A Model for Tutorial 3

Slide 34:

Set the working directory and start a new object file. Draw the sketch using the sketcher tool buttons. Dimension the sketch and then modify the dimensions of the sketch, see Figure C . Figure C Sketch with dimensions and constraints Save the sketch.

Slide 35:

In this exercise, you will draw the sketch for the model shown in Figure A . The sketch is shown in Figure B . (Expected time: 30 min) Exercise 1 Figure B Sketch of the model Figure A Solid model for Exercise 1

Slide 36:

In this exercise, you will draw the sketch for the model shown in Figure A . The sketch is shown in Figure B . (Expected time: 30 min) Exercise 2 Figure B Sketch of the model Figure A Solid model for Exercise 2

Slide 37:

In this exercise, you will draw the sketch for the model shown in Figure A . The sketch is shown in Figure B . (Expected time: 30 min) Exercise 3 Figure B Sketch of the model Figure A Solid model for Exercise 3

Slide 38:

In this exercise, you will draw the sketch for the model shown in Figure A . The sketch is shown in Figure B . (Expected time: 30 min) Exercise 4 Figure B Sketch of the model Figure A Solid model for Exercise 4

Slide 39:

Exercise 5 In this exercise, you will draw the sketch for the model shown in Figure A . The sketch is shown in Figure B . Figure A Solid model for Exercise 5 Figure B Sketch of the model