5-Beam SONAR Head Lesson

SETUP

  1. Click New on the Standard toolbar.

The New SolidWorks Document dialog box appears.

  1. Click Part.
  2. Click OK.
  3. Click Options on the Standard toolbar.
  4. Click on Document Properties
  5. Select ANSI
  6. Click on Units and select IPS
  7. Click on Material Properties and Select Aluminumand then Click OK

MAKING THE BASE PART

  1. Click Extruded Boss/Base on the Features toolbar.

The Front, Top, and Right planes appear in the graphics area.

  1. Move the pointer over the Top plane to highlight it, then click to select it.

The display changes so that the Top plane is facing you. A sketch opens on the Top plane.

  1. Click Circleon the Sketch toolbar.
  2. Move the pointer over the origin.

The pointer changes to . This indicates a coincident relation between the center of the circle and the origin.

  1. Click to place the center point on the origin.
  2. Move the mouse and notice a preview of the circle dynamically follows the pointer.
  3. Click to finish the circle.

DIMENSIONS

  1. Click Smart Dimensionon the Dimensions/Relations toolbar.
  2. Select the circle.

Notice the preview of the diameter dimension.

  1. Move the pointer to where you want the dimension and click to add the dimension.
  2. In the Modify box, type 3.5.

EXTRUDING THE BASE FEATURE

  1. Click Exit Sketch on the Sketch toolbar.

You exit the sketch when you are done with the 2D profile and are ready to create the 3D cylinder.

The settings for the extrusion appear in the PropertyManager in the left panel.

  1. In the PropertyManager, under Direction 1:
  2. Select Blind in End Condition.
  3. Set Depthto 1.
    Notice the shaded preview of the extrusion.
  1. Click OK.

SAVE THE PART

  1. Click Save on the Standard toolbar.
  2. In the dialog box, type 5-Beam SONAR Head for File name.
  3. Click Save.

SKETCHING THE BOSS (Screw Mount)

  1. Click Extruded Boss/Base on the Features toolbar.
  2. Select the top face of the part.
  3. Click Bottom on the Standard Views toolbar.
  4. Click Circle on the Sketch toolbar.
  5. Move the pointer to the center of the base cylinder.

The pointer changes to.

Note: The ring boss is concentric with the base cylinder because you started both at the origin.

  1. Click to place the center of the circle.
  2. Move the pointer and click to finish the circle.

DIMENSIONING THE BOSS

  1. Click Smart Dimension on the Dimensions/Relations toolbar.
  2. Select the circle.
  3. Move the pointer and click to place the dimension.
  4. In the Modify box, type 0.75.

VIEW IN TRIMETRIC

  1. Click Trimetric on the Standard Views toolbar for a better view of the model.

CENTER HOLE

Create a circle for the center hole using the Hole Wizard.

  1. Click Hole Wizard and select Hole
  2. Change the Size to ½ inch and Hole Type & Depth to Through All
  3. ClickNext
  1. Select the top face of the part
  2. Move the pointer over the center of the top and position the hole.
  3. Make sure the position is at 0.00, 1.00, 0.00.
  1. Click to complete the circle
  2. Click Finish

SECONDCENTER HOLE

Create a circle for the center hole (Do not use the Hole Wizard).

  1. Click Extruded Cut on the Features toolbar.
  2. Select the top face of the part.
  3. Click Top on the Standard Views toolbar.
  4. Click Circle on the Sketch toolbar.
  5. Move the pointer over the origin.
  6. Click to place the center of the circle.
  7. Move the pointer and click to finish the circle.
  8. Click Smart Dimension on the Dimensions/Relations toolbar.
  9. Select the circle.
  10. Move the pointer and click to place the dimension.
  11. In the Modify box, type 1.0.
  12. Click Exit Sketch on the Sketch toolbar.
  13. Click Trimetric on the Standard Views toolbar (optional).
  14. In the PropertyManager, under Direction 1, select Blind for End Condition.
  15. And a Depth of 0.3125.
  16. Click OK to complete the circle.

HORIZONTAL HOLES (for wires)

Create a circle for the side holes.

  1. Click Extruded Cut on the Features toolbar.
  2. Select the right face of the part.
  3. Click Right on the Standard Views toolbar.
  4. No plane is currently available to create the hole so we will use the right plane. To use the right plane click at the edge between the two bars (see picture). A parallel symbol should appear. When the parallel symbol appears, drag it down by holding the left button and dragging it.

The attributes of the part will appear.

  1. Select Right Plane
  2. Click Circleon the Sketch toolbar.
  3. Move the pointer above the origin to a point around ½ inch (middle).
  1. Click to place the center of the circle.
  2. Move the pointer and click to finish the circle.
  3. The parameters of the circle should be:

or

  1. Click Smart Dimension on the Dimensions/Relations toolbar.
  2. Select the circle.
  3. Move the pointer and click to place the dimension.
  4. In the Modify box, type 0.25.
  1. Click Exit Sketch on the Sketch toolbar.
  2. Click Trimetric on the Standard Views toolbar.
  3. In the PropertyManager, under Direction 1, select Through All for End Condition.
  4. Also check the box for Direction 2, select Through All for End Condition. This is needed to make the hole on both sides of the plane.
  5. Click OK.

Make a second through-hole using the Back Side and the Front Plane with all of the other parameters the same, then Click Trimetric on the Standard Views toolbar. The part should look like:

30 DEGREE SIDE ANGLE CUTS

To create the side angle cuts, a new set of planes at 35 degrees for each cut must be used. First, because there are no additional non-curved reference points the axis of the side holes will be used to aid in specifying the 35 degree plane angles.

  1. Turn the Temporary axes on.
  1. Insert a plane from the Reference Geometry menu (see figure).
  1. Select one of the temporary axis, select the angle option and type in 35 degrees and then select the top of the part. This will give you a plane as seen below:
  2. Next create a plane that is offset by 0.75 inches above the first plane to position the 1st cut. Select the right viewing orientation and then select the wire frame view to see how the plane intersects the part.
  3. Next extrude a cut using this plane. After selecting Extruded Cut, rotate the view to the front. It will ask you to select a reference plane for cutting. Select the second plane on drawing. Select rectangle for the shape to cut and create the rectangle over the plane. The view should look like the next figure.
  4. Exit sketcher .
  5. Next rotate the figure to the right plane. The view should look like:
  6. Click the change direction button to cut the material in the correct direction. Make sure to increase the D1 so the yellow is above the part.
  7. If your click on the preview button the view will look like:
  8. Click the OK button to complete the cut and rotate to the trimetric view.
  9. This procedure is to be done on all four sides.
  10. Finally, the four side sonar transducer holes need to be bored. First select , then select the plane and use the circle button to orient where the hole will be. Use an X of 0.00 a Y of 0.50 and a radius of 0.375inches.
  11. After Next enter the depth of the hole, i.e., 0.3125 inches.
  12. The hole should look like the next figure.
  13. Repeat this procedure for the other three holes.