From the Tools tab, click the Application Options button.

Then choose the Sketch tab, as shown in Figure 3.1.

Click the Inventor button, and choose New

In the New File dialog box, click the Metric tab, and select the Standard(mm).ipt icon, as shown in Figure 3.10.

Click OK to create a new part file based on this template.

Pause your mouse pointer over the Line tool in the Sketch tab's Draw panel. (See Figure 3.11 for the location of the Line tool.)

Figure 3.11. Locating the Line tool on the Sketch tab

Note the tool tip that appears, providing the tool name, keyboard shortcut (in this case L), and a brief description of the tool. If you hover the pointer over long enough, a second stage of the tool tip appears with a more detailed description of the tool.

Click the Line button to start the Line tool.

Hover your mouse pointer over the dot in center of the drawing area. This is the 0,0,0 origin point that has been automatically projected into Sketch1.

Note that when your mouse pointer moves over the dot it changes to a green dot and shows a small glyph symbol. This green dot is a snap symbol indicating that a point, endpoint, or midpoint has been located. The glyph symbol indicates that a sketch constraint is being placed. In this case, it is a coincident constraint, which ensures that the endpoint of the line will stay coincident to the projected origin point. See Figure 3.12 for reference.

Figure 3.12. Endpoint snap symbol and coincident glyph

Start your line on this point by clicking the dot and releasing the mouse button.

Move your mouse pointer directly to the right, and you will see another glyph indicating that a horizontal sketch constraint is being placed (see Figure 3.13 for reference). The horizontal constraint ensures that the line will stay positioned horizontally. Note that if you move your mouse pointer so that the line is being drawn at an angle, the glyph disappears.

Figure 3.13. Creating a line with an automatic horizontal constraint

Notice the status bar at the bottom of the screen indicating the length and angle of the line as you move the mouse pointer. Click the graphics window while the horizontal glyph is displayed to create a line roughly 45mm long. Don't worry about getting an exact length. You will set the precise length later; for now, you are just "roughing in" a general shape. Note the line continues when the first line segment is placed, and you can add more segments as required.

Move your mouse pointer straight up to add another line segment, and note another glyph appears at the mouse pointer. This is a perpendicular glyph indicating that a sketch constraint is being placed that will hold the first and second line segments perpendicular (see Figure 3.14 for reference).

Figure 3.14. Creating a vertical line with an automatic perpendicular constraint

Click the graphics window to create the second segment at roughly 45mm long and perpendicular to the first segment.

Right-click, and choose Done to exit the Line tool. Note that the Esc key will also exit the active tool, as indicated in the right-click menu.

Right-click anywhere in the graphics window other than on the lines, and choose Show All Constraints (or press F8 on the keyboard). You will now see the sketch constraint icons for the constraints that were inferred as you created the line segments.

Hover your mouse pointer over the perpendicular constraint at the corner of the two line segments to see both lines highlighted, which indicates that these are the objects involved in this particular constraint definition.

Hover your mouse pointer over the yellow dot at the corner of the two line segments, and you will see two coincident constraints appear, as shown in Figure 3.15. Hovering your mouse pointer over each will highlight the line to which they belong. Coincident constraints are initially "rolled up" in this way because they are generally very numerous and tend to clutter the sketch when all constraints are shown.

Figure 3.15. Showing constraints

Click the X on any of the constraints to hide just that particular constraint.

Next right-click anywhere in the graphics area other than on the lines, and choose Hide All Constraints (or press F9 on the keyboard). You can toggle the visibility of all sketch constraints on and off as needed in order to determine how sketch entities are constrained together.

Let up on the corner, select the corner point of the two line segments, and hold down and drag around in a circle. You will notice that the horizontal line will stretch as required but will always remain horizontal; the vertical line will always remain perpendicular.

Select the uppermost endpoint of the vertical line, and drag around in a circular motion as well. Note the two lines will adjust lengths as permitted but will always honor the sketch constraints that they have placed on them.

Let up on the end of the line, and press F8 to show the constraints again.

Right-click the horizontal constraint.

Choose Delete to remove this constraint.

Press F9 to hide the constraints again.

Click the corner of the lines, and hold down and drag around in a circular motion. Note that the lines will stretch and adjust orientation but will maintain their perpendicular and coincident relationships.

Go to the Constrain panel of the Ribbon, and click the Horizontal Constraints icon, as shown in Figure 3.16.

Click the first line segment you sketched to set it back to horizontal.

To view the DOF arrows for your sketch entities, right-click anywhere in the graphics area that is not on a sketch object, and choose Show All Degrees Of Freedom. Your sketch should resemble Figure 3.18.

Notice the arrow indicators showing the DOF for each sketched line.

Drag an endpoint, and you will see the sketch lines will drag only in a direction or orientation that follows the DOF arrows. If your sketch becomes distorted in an undesirable way, use the Undo icon at the top of the screen or press Ctrl+Z to set it back as it was.

Figure 3.18. Showing the degrees of freedom in a sketch

To toggle the DOF visibility back off, right-click again, and choose Hide All Degrees Of Freedom.

Note that you can right-click an individual sketch object or a selection set of sketch objects and choose Display Degrees Of Freedom to show the DOF for just those selected objects.

Right-click and choose Show All Degrees of Freedom again to have these displayed for reference in the next steps.

On the Sketch tab of the Ribbon, click the Dimension icon in the Constrain panel, as indicated in Figure 3.19.

In the graphics area, click the bottom horizontal line, and drag down to display the dimension.

Click below the line to place the dimension, and you should see an Edit Dimension box, as shown in Figure 3.19. If you do not see the Edit Dimension box, you can right-click anywhere in the blank space of the graphics area and click Edit Dimension to ensure that this box shows up after placing each dimension. Then simply click the dimension to open this input box.

In the Edit dialog box, type Length = 45. Because you are working in a millimeter-based part file, the units are assumed to be 45mm, and Inventor will add the mm automatically.

Figure 3.19. Placing a dimension on the sketch

Notice the Edit Dimension box caption reads something such as d0. This indicates that this dimension parameter is named d0. Initially, Inventor names the first dimension used in the file d0, the next is named d1, and so on. By entering Length = 45, you are renaming the dimension from d0 to Length and changing this length value from the sketched value to a precise value of 45mm. You are not required to rename your dimensions, but it is good practice to name any that you intend to reference later.

Click the green arrow in the Edit Dimension box, or press the Enter key to set the dimension value. Take note that the dimension "drives" the sketch to be 45mm long. Also notice that some of the DOF arrows have been removed.

Click the 45mm dimension to edit it. Notice that the Edit Dimension box caption now reads Length and the value now reads 45mm.

Change the value to 50mm, and click the green arrow.

Next click the bottom horizontal line again and drag up, but do not click to place the dimension. You will see the same horizontal dimension displayed.

Click the top horizontal line, and drag down, and you will see the dimension change from the horizontal dimension evaluation the length of the bottom line to a vertical dimension evaluating the distance between the top and bottom lines.

Click the graphics window to place the dimension.

Enter Width=

Click the 50mm dimension you placed in the previous steps. Notice that clicking one dimension while editing another will create a reference between the two.

Complete the formula to read Width = Length/2, as shown in Figure 3.20.

Click the green arrow or press the Enter key to set the dimension value. Observe that the Width dimension is evaluated at half the Length dimension and that it displays an fx: before the value to denote that there is a function used to evaluate this dimension. Also notice that more DOF arrows have been removed as you have further defined the sketch.

Figure 3.20. Referencing one parameter to another

If your sketch has become a bit skewed, exit the Dimension tool by right-clicking and choosing Done (or by pressing the Esc key).

Click the top endpoint of the vertical line to the right, and drag it so that the profile general shape is restored.

On the Sketch tab of the Ribbon, click the Dimension icon in the Constrain panel, or just press D on the keyboard to start the Dimension tool again.

Click the vertical line to the right, and then click the diagonal line. Take care to click the lines and not the endpoints of the lines, because doing do will result in a different dimension type.

You will be presented with an edit box for an angle dimension. Enter Angle1 = 108, and click the green check mark.

Lastly, on the Sketch tab of the Ribbon, click the Equal button in the Constrain panel to place an equal constraint. Select the top horizontal line and the vertical line on the right to set those two lines equal.

Your sketch is now fully constrained and should resemble Figure 3.21.

On the Ribbon's Sketch tab, click Finish Sketch in the Exit panel. Or right-click in the graphics area and choose Finish Sketch from the menu.

Click the Inventor button, and then select Save.

Select the Chapter3 folder, and name the file mi_001.

Locate Sketch1 in the Model browser to the left of your screen, and either right-click and choose Edit Sketch or double-click the browser sketch icon.

Notice that the Sketch node listed in the browser consists of the sketch icon and the sketch name. Clicking the sketch name once and then again (don't double-click) allows you to rename the sketch. Therefore, you may want to develop a habit of double-clicking the sketch icon rather than the sketch name to set a sketch active for edits.

Look at the browser and notice that the rest of the browser nodes are grayed out and Sketch1 is highlighted, letting you know that the sketch is active for editing. You'll also notice that the sketch tools are available.

Click the Line tool in the Sketch tab's Draw panel. (Recall that you can access the Line tool by pressing the L key on the keyboard as well.)

Start the line at the bottom-left corner of the profile, keeping an eye on your mouse pointer to ensure that you see the green dot (indicating the endpoint) and the constraint glyph (indicating a coincident constraint is being inferred).

Set the second point of the line on the midpoint of the diagonal line. Again, you should see a green dot and a coincident glyph, as shown in Figure 3.22.

Figure 3.22. Placing a construction line

Right-click and choose Done to exit the Line tool.

Select the new diagonal line you just created.

On the Sketch tab (to the far right), click the Construction icon in the Format panel, as shown in Figure 3.23.

In the Sketch tab's the Draw panel, click the Polygon tool.

Select the midpoint of the diagonal construction line, keeping an eye on your mouse pointer for the green midpoint dot and the coincident glyph.

Leave the polygon settings at the defaults, and drag out the size and orientation to roughly match Figure 3.24.

Figure 3.24. Creating a polygon

In the Sketch tab's Constrain panel, click the Parallel constraint icon.

Choose any of the flats on the polygon and the diagonal profile line as shown in Figure 3.25 to make the two lines parallel.

Figure 3.25. Setting the two edges to be parallel

In the Sketch tab's Constrain panel, click the Dimension tool.

On the polygon, click two opposing points as shown in Figure 3.26 to create a dimension between the two points.

Figure 3.26. Creating a point to point aligned dimension

Pull your mouse pointer to the side to preview the dimension. Notice that the orientation wants to be horizontal or vertical depending upon the location of your mouse pointer.

Right-click and choose Aligned to force the aligned solution for this particular dimension.

Click the graphics window to place the dimension.

Enter Hex_Size = 0.375 in.

Click the green arrow or press the Enter key to set the dimension value. Notice that although you entered an empirical unit of inches, Inventor converted the value automatically to the file default of millimeters. This is a powerful function that allows you to use dimension inputs to do conversion calculations on the fly.

In the Sketch tab's Modify panel, click the Offset tool.

Before selecting any geometry, right-click anywhere that is not on the sketch geometry.

Ensure that the Loop Select and Constrain Offset options are both selected.

Click the polygon, and drag to the outside.

Click the graphics window to set the offset distance.

Right-click and choose Done (or press the Esc key) to exit the Offset tool.

In the Sketch tab's Constrain panel, click the Dimension tool (or press D on the keyboard)

To dimension the offset, select an edge of the original polygon, and then select the corresponding edge on the new offset polygon.

Drag the dimension out from the center of the polygon, and place it anywhere.

Enter Hex_Offset = 1/16", and click the green check mark. The result should appear similar to Figure 3.27.

Figure 3.27. The offset polygon

In the Sketch tab's Draw panel, click the Rectangle flyout, and choose Rectangle Three Point, as shown in Figure 3.28.

Figure 3.28. Accessing the Rectangle Three Point tool

Create the rectangle using the three points shown in Figure 3.29. Make certain that you are seeing the green snap dots and coincident constraints glyphs at each point.

Figure 3.29. Placing a three point rectangle

Right-click, and choose Done.

Double-click the 50mm Length dimension.

Replace the value of 50 with 60, and press the Enter key.

Take note that the vertical dimension retains the intent of your design and remains at half the Length value.

In the Sketch tab's Constrain panel, click the Dimension tool (or press D on the keyboard).

Select the vertical line on the right of the sketch, and click the graphics window to place the dimension.

You will be presented with a dialog box warning you that this dimension will overconstrain the sketch. Click Accept to place the dimension as a driven dimension.

Notice that the dimension is created in parentheses, denoting that it is driven by other parameters, and therefore is considered a reference parameter. Driven dimensions are useful in capturing dimensions for use in the calculations of other features.

Next switch from the Sketch tab to the Manage tab on the Ribbon.

Click the Parameters tool. This will open the Parameter dialog box listing all the dimensions you've created in this part as parameters, as shown in Figure 3.31.

Figure 3.31. Parameters dialog box

Change the Length value from 60mm back to 50mm.

Click Done to return to the sketch. Notice the dimensions have not updated.

To update the dimension, go to the Quick Access bar at the top left of the screen, and click the Update button, as shown in Figure 3.32. Notice that the sketch dimensions update and the Update button becomes grayed out letting you know that file you are working with does not require updates at this time.

Click the 50mm Length dimension.

In the Sketch tab's Format panel, click the Driven Dimension tool. Notice that the Length dimension is now set in parentheses, indicating that it is now driven rather than driving.

Double-click any blank area in the graphics window to unselect the previous dimension.

Select the vertical dimension that is in parentheses.

Click the Driven Dimension tool again to toggle this dimension from a driven to a driving dimension.

Double-click the vertical dimension to edit its value.

Enter Vertical_Leg = 15mm, and click the green check mark. Notice that the Vertical_Leg parameter now drives the Length parameter, which drives the Width dimension. You should be beginning to see the power of parametric design.

You can close this file without saving changes.

Click the Inventor button, and choose Open (or press Ctrl+O on the keyboard).

Browse for the file named mi_3h_001.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

Press the F8 key to show all the constraints. Note there is no tangent constraint between the large circle and the lines.

In the Sketch tab's Constrain panel, click the Tangent button. Click the line and circle, as shown in Figure 3.34.

Figure 3.34. Placing a tangent constraint

Repeat to set a tangent constraint on the top line and the same circle.

Right-click, and choose Done.

Press the F8 key to show all the constraints, and note the new tangent constraints.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_002.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Perpendicular button.

Click the line as shown in Figure 3.35, and then select either of the horizontal lines.

Figure 3.35. Placing a perpendicular constraint

Right-click, and choose Done.

Press the F8 key to show all the constraints, noting the new perpendicular constraint.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_003.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Parallel button.

Click the line as shown in Figure 3.36, and then select the lower horizontal line.

Figure 3.36. Placing a parallel constraint

Right-click, and choose Done.

Press the F8 key to show all the constraints, and note the new parallel constraint.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_004.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Coincident button.

Click the center of the circle and then on the center point, as shown in Figure 3.37.

Figure 3.37. Placing a coincident constraint

Right-click, and choose Done.

Next, click the endpoint of the vertical line at the top-right corner of the rectangular shape, and hold down as you drag to close the profile. Note that a coincident constraint is placed.

Press the F8 key to show all the constraints, and note the new coincident constraints, as shown by the yellow dots.

Hover your mouse pointer over the dots to see coincident constraint symbols.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_005.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Concentric button.

Click the edge of the circle and then the arc, as shown in Figure 3.38.

Right-click, and choose Done.

Press the F8 key to show all the constraints, and note the new concentric constraint.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_006.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Collinear icon.

Click the lines as shown in Figure 3.39.

Figure 3.39. Placing a collinear constraint

Right-click, and choose Done.

Press the F8 key to show all the constraints, and note the new collinear constraint.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_007.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Horizontal button.

Click the line as shown in Figure 3.40, noting the new horizontal alignment.

Figure 3.40. Placing a horizontal constraint

Next click both of the points as indicated in Figure 3.40, noting that they will line up horizontally.

Right-click, and choose Done.

Press the F8 key to show all the constraints, and note the new horizontal constraints.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_008.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Vertical button.

Click the line as shown in Figure 3.41, noting the new vertical alignment.

Figure 3.41. Placing a vertical constraint

Next click both of the points as indicated in Figure 3.41, noting that they will line up vertically.

Right-click, and choose Done.

Press the F8 key to show all the constraints, and note the new vertical constraints.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_009.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Equal button.

Click the two circles as shown in Figure 3.42, and notice that they become equal.

Figure 3.42. Placing an equal constraint

Click the lines as indicated in Figure 3.42, noting that they too will become equal. You can make two of the vertical lines equal if you'd like as well.

Right-click, and choose Done.

Press the F8 key to show all the constraints, and note the new equal constraints.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_010.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

Drag the corner as indicated in Figure 3.43, and notice that it may be repositioned freely.

In the Sketch tab's Constrain panel, click the Fix button.

Click the same corner as before.

Right-click, and choose Done.

Drag the corner again, and notice that it is now fixed to that position.

Figure 3.43. Placing a fix constraint

Next apply another fixed constraint to the vertical line next to the rectangle, and be sure to click the line rather than the endpoint.

Right-click and choose Done to exit the constraint tool, and then drag either endpoint of the line. While the line position is fixed, the endpoints are still free to change.

Press the F8 key to show all the constraints, and note the new fix constraints.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_011.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Symmetric button, as indicated in Figure 3.44.

Figure 3.44. Placing a symmetric constraint

Click the circle on the left, and then click the circle on the right.

Next click the centerline, and observe that the circles become symmetric.

Continue by clicking a line on the square on the left side of the sketch.

Click the corresponding line on the rectangle on the right. Notice that this time you did not need to select the centerline. When using the symmetric constraint, you need only to establish the centerline once.

Continue making the sketch symmetric by selecting lines on the left of the sketch and then selecting the corresponding line on the right side.

Right-click and choose Done when the sketch is symmetric.

Press the F8 key to show all the constraints; note the new symmetric constraints.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_012.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click it, and choose Edit Sketch.

In the Sketch tab's Constrain panel, click the Smooth button.

Click the spline and arc as indicated in Figure 3.45.

Figure 3.45. Placing a smooth constraint

Right-click, and choose Done.

Press the F8 key to show all the constraints; note the new smooth constraint.

You can exit the file without saving once you are finished.

From the Get Started tab, select the Open button.

Browse for the file named mi_3h_013.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open. The goal here is to re-create the oblong shape already present in the sketch.

In the Model browser, double-click Sketch1 to edit it. Or, right-click, and choose Edit Sketch.

Figure 3.49. Creating an arc with the line

In the Sketch tab's Draw panel, click the Line icon.

Click the projected origin point as the start point of the line, and then release the mouse button. This is the small dot located at 0,0 of the sketch.

Next pull your mouse pointer to the right, ensuring that you see a horizontal or parallel glyph, indicating that your line is horizontal.

Click the screen to set the second point of the line, and then release the mouse button.

Now to sketch an arc without exiting the Line tool, click and hold the endpoint you just created, and then (still holding down on the mouse button) drag your mouse pointer out to preview the arc. If the arc previews in the wrong direction, simply return your mouse pointer to the endpoint and try again. It may be helpful to "trace" the guideline cross and exaggerate the arc size to get the direction established and then bring your mouse pointer back in to get the size you want.

Release the mouse button to end the arc and continue the Line tool.

Continue creating line/arc segments, or right-click and choose Done to exit the Line tool. Practice this a few times, and you'll have it mastered in a short time.

From the Get Started tab, select the Open button.

Browse for the file named mi_3r_001.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

In the Model browser, double-click Sketch1 to edit it. Or, right-click, and choose Edit Sketch.

In the Sketch tab's Draw panel, click the Project Geometry icon.

Click the edges of the red oval-shaped profile.

When you have the complete profile projected into the sketch as shown in Figure 3.52, click the Finish Sketch button.

You can close the file without saving changes.

From the Get Started tab, select the Open button.

In the New File dialog box, click the Metric tab, and select the Standard(mm).ipt icon.

Click OK to create a new part file based on this template.

On the Insert panel of the Sketch tab, click the Insert AutoCAD File icon.

In the resulting dialog box, select the file Import1.dwg from the Chapter 3 directory of the Mastering Inventor 2010 folder.

Click Open to start the conversion process. Once the AutoCAD file opens, you will move into a series of Import Destination Options pages. The first page is mostly grayed out except for specifying units, constraining endpoints, and optionally applying geometric constraints upon import under most conditions. Set your selections as shown in Figure 3.55.

Click Finish to complete the import.

Open the existing file in AutoCAD.

From an open AutoCAD file, simply select the geometry you want to import, right-click, and choose Copy, thereby copying the selected objects to the Windows Clipboard.

Next, in Inventor and with a 2D sketch active for editing, simply right-click and choose Paste. You will be presented with a bounding box preview of the pasted entities.

At this point, you can right-click and choose Paste Options to ensure that the insert scale is correct or simply click the graphic window to place the pasted geometry.

From the Get Started tab, select the Open button.

Browse for the file named mi_3w_001.ipt located in the Chapter 3 directory of the Mastering Inventor 2010 folder, and click Open.

On the Model tab, click the drop-down arrow on the Sketch panel below the Create 2D Sketch icon, and then click the Create 3D Sketch icon. Or right-click in an empty area of the graphics window, and choose New 3D Sketch.

Notice that although this is a part file, it has some reference surfaces in it already. These were included simply to emulate a situation where you might be creating a part within the context of an assembly. You will learn more about creating parts within an assembly in the chapters to come.

There is also a 2D Sketch called Profile1 already in the Model browser; you'll use this sketch at the end of this exercise. Your goal is to create a 3D sketch running from the center of the connection input of the box, through each of the large holes in the flange brackets.

On the 3D Sketch tab, click the Spline tool icon.

You will see the Inventor Precise Input toolbar appear along with the 3D coordinate triad. The triad displays the X, Y, and Z planes and the corresponding axis in the form of three arrows. The red arrow indicates the x-axis, the green arrow indicates the y-axis, and the blue arrow indicates the z-axis. Notice that the triad is first positioned at 0,0,0.

Specify a start point for the spline by clicking the front, circular edge of the connection input.

Next click the center of the large hole of the first triangular flange bracket. It makes no difference if you choose the front or back edge of the hole.

Do the same for the other two flange brackets.

Right-click and choose Create to complete the spline.

Then right-click again, and choose Done to exit the Spline tool. Your screen should look similar to Figure 3.57.

Still in the 3D sketch, click the Line tool icon on the 3D Sketch tab.

Notice the return of the triad and Precise Input toolbar.

Click the endpoint of the spline to set the start of the line on this point.

You will see the triad move to the spline endpoint. Notice that the triad is not lined up with the bracket flange. To remedy this, you will use the Precise Redefine button found on the Precise Input toolbar.

Click the Precise Redefine button, as shown at the top of Figure 3.59.

Figure 3.59. Precise Redefine button

Then select the shaft of the red arrow.

Next click the bottom edge of the triangular flange bracket toolbar, as shown on the left of Figure 3.59.

Click the Precise Redefine button again, and this time click the green arrow shaft.

Then click the small edge indicated in the center of Figure 3.59. The triad orientation should now resemble the far right of Figure 3.59.

Next, click the triad plane between the blue and green arrows to isolate that plane to sketch on. It should highlight red and then stay shaded when selected, and you will see a 0 placed in the X cell of the Precise Input toolbar.

Fill out the rest of the input cells so that you have X=0, Y=6, Z = 0.5, and press Enter.

Note you can hit the Tab key to switch between the X, Y, and Z input cells. Values will be input as relative coordinates. Recall that with relative coordinates the new input coordinate point is based on the previous point rather than the absolute 0,0,0 origin point. You will now have a line running from the end of the spline out at 6 inches in the y-axis with a slight rise in the z-axis.

Still in the Line tool, right-click, and ensure that Auto-bend is selected in the right-click menu. Auto-bend will place a radius at the corners in your line route. The default radius size can be set by selecting Document Settings from the Tools tab and then going to the Sketch tab. Once bends are placed, they can be edited like any other dimension.

With the Line tool still active, click the plane between the green and red arrows on the triad to isolate the XY plane, and fill out the rest of the input cells so that you have X=4, Y=4, Z = 0. Press Enter on the keyboard to set this line. You will see a small dimensioned radius at the corner of your two line segments. This is a result of the Auto-bend option.

Right-click and choose Done to exit the Line tool. Your 3D sketch should resemble Figure 3.60.

Figure 3.60. 3D sketch path

Click the Dimension icon command in the 3D Sketch tab, and add dimensions as shown in Figure 3.61. Notice you want to edit the bend radius that was created with the line command.

Figure 3.61. 3D sketch dims

Right-click and choose Done to exit the Dimension tool.

Then right-click, and choose Finish 3D Sketch.

In the Model tab's Create panel, click the Sweep icon. Profile1 will be automatically selected as the sweep profile unless you have another unconsumed, closed profile sketch in your part, in which case you will need to select Profile1 manually.

Once the profile has been selected, ensure that the Path button in the Sweep dialog box is enabled, and then click the 3D sketch you just created. Your sweep should look like Figure 3.62.