3D Sketching Using a 3D Sketch to Create an Oven Rack Frame

3D Sketching
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3D Sketching
Using SolidWorks, you can create 3D sketches. You use a 3D sketch as a sweep path, as a guide
curve for a sweep or loft, as a centerline for a loft, or as one of the key entities in a routing system. A
useful application of 3D sketching is designing routing systems.
This lesson introduces you to 3D sketching and describes the following concepts:
• Sketching relative to coordinate systems
• Dimensioning in 3D space
• Mirroring features
Next
Using a 3D Sketch to Create an Oven Rack
Frame
In this lesson, you build the outer frame of a wire oven rack by sweeping a circle along a 3D sketch.
After you complete half of the rack, you use the Mirror All function to finish the model.
First create the 3D sketch of the outer frame.
1. Click New (Standard toolbar) and create a new part.
2. Click 3D Sketch (Sketch toolbar).
3. Click Line (Sketch toolbar) and sketch a line about 135mm long on the XY plane
from the origin. The pointer changes to
while sketching horizontally on the XY plane.

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Sketch the line to an approximate length, then dimension to the exact length later.
4. Click Select (Standard toolbar), and select the beginning endpoint of the line.
5. In the PropertyManager, make sure that the endpoint is exactly at the origin (0, 0, 0 as shown
under Parameters), is Coincident with the origin (as shown in Existing Relations) and is
Fully Defined (as shown in Information ).
6. If the endpoint is not at the origin:
• Under Parameters, set X Coordinate, Y Coordinate, and Z Coordinate to 0.
• Click Fix in Add Relations.
Next
Now the point is Fully Defined, as shown in Information .
7. Reduce the size of the sketch to provide open sketching area on the right side of the graphics
area.
Using a 3D Sketch to Create an Oven Rack Frame (Continued)
8. Click Line (Sketch toolbar) and continue sketching the other lines from the endpoint of
the 135mm line. Each time you begin a new line, the origin for the current coordinate system
is displayed at the beginning of the new line to help orient you.
Sketch the following lines to an approximate length, then dimension to the exact length
later.
a. Sketch down the Y axis for 15.
b. Sketch along the X axis for 15.

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c. Press Tab to change the sketch plane to the YZ plane .
d. Sketch along the Z axis for 240.
e. Press Tab twice to change the sketch plane back to the XY plane.
f. Sketch back along the X axis for 15.
g. Sketch up the Y axis for 15.
h. Sketch back along the X axis for 135.
Next
Using a 3D Sketch to Create an Oven Rack Frame (Continued)
9. Dimension each of the lines as shown.

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10. Click Sketch Fillet (Sketch toolbar), and fillet each intersection with a 5mm fillet.
To fillet the intersections, select the point where two lines meet.
11. Click 3D Sketch (Sketch toolbar) to close the sketch.
12. Save the part as rack.sldprt.
Next
Using Sweep to Complete the Feature
To complete the base feature, sweep a circle along the 3D sketch path.
1. Select the Right plane in the FeatureManager design tree, then click Sketch (Sketch
toolbar) to open a 2D sketch on that plane.
2. Sketch a circle 5mm diameter circle at the origin.

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3. Click Exit Sketch (Sketch toolbar).
4. Click Swept Boss/Base (Features toolbar).
5. In the PropertyManager, under Profile and Path:
• Select the circle (Sketch1) for Profile .
• Select the 3D sketch (3DSketch1) for Path .
6. Click .
Next
Extruding the Supports
Create a support by extruding a circular sketch between the frames.
1. Select the Front plane in the FeatureManager design tree.
2. Click Extruded Boss/Base (Features toolbar).
3. Click Normal To (Standard Views toolbar).
4. Sketch a circle on what appears to be the face of the frame. (The Front plane is in the center
of the frame wire.) Watch for the inference lines that indicate the centerpoint of the circle is
horizontal to the origin.
5. Dimension the center of the circle 11mm from the origin.

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6. Dimension the diameter of the circle to 4
7. Exit the sketch.
8. Click Trimetric (Standard Views toolbar).
9. In the PropertyManager, under Direction 1:
• If necessary, click Reverse Direction so the arrow in the graphics area points in the
correct direction to meet the other side.
• Select Up to Surface in End condition.
• Select the opposite side of the frame for Face/Plane .
• If necessary, select Merge result. Merge result controls whether or not you create
separate solid bodies.
10. Click to complete the support.
Next
Patterning the Extrusion
Now pattern the extrusion.
1. Click View, Temporary Axes to turn on the display of all temporary axes.
The axes must be visible because you need to select them to create a pattern.

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2. Select Extrude1 in the FeatureManager design tree.
3. Click Linear Pattern (Features toolbar).
Extrude1 appears in Features to Pattern in the PropertyManager.
4. Click the temporary axis on the face of the frame where you sketched the circle.
The pointer changes to
when you move it over the axis.
In the graphics area, a preview of the pattern appears, and an arrow indicating the direction of
the pattern appears on the frame at the right end of the axis. In the Property Manager, Axis
appears in Pattern Direction.
5. Under Direction 1:
• Check the preview of the extrusions to make sure they are patterned towards the outer
edge, as shown below. If necessary, click Reverse Direction to change the pattern
direction.
• Set Spacing to 22.
• Set Number of Instances to 6.
6. Click .

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The extrusion pattern is completed.
Next
Mirroring All
Use the Mirror function to complete the wire rack.
1. Click View, Temporary Axes to hide the temporary axes.
2. Click Mirror (Features toolbar).
3. Rotate the half-rack and click on the end face of the frame.
Face appears in Mirror Face/Plane
in the PropertyManager.
4. Click Bodies to Mirror , then click anywhere on the rack.
5. Click to mirror the half rack body about the selected face.
6. Click Isometric (Standard Views toolbar).
The rack is completed.
7. Save the part.
Congratulations! You have completed this tutorial!