🐺Designing your Part (Autodesk Fusion)

1_Create Part Body Sketch

Click Design > Create > Create Sketch. Select the top plane

Sketch Part Body Rectangle

Click Create> Rectangle> Center Rectangle. Select the point in the middle of the screen. Drag to draw a rectangle. Click Create > Sketch Dimension. Select the ends of the rectangle and dimension 11mm height and 56.35mm length.

Sketch Part Body Mounting Hole

Click Create> Circle> Center Diameter Circle. Draw a circle to the left of the rectangle center. Click Create> Sketch Dimension. Click the center of the circle then the center point of the rectangle and enter a distance of 24.803mm.

Add Constraints To Mounting Hole Sketch

Click the eye Icon next to Origin in the browser tree to show the x,y axis. Click Constraints> Coincident. Select the center point of the circle then the red line (x-axis) from the center of the rectangle.

Mirror Mounting Hole Sketch

Click Create> Mirror. Select the circle sketch. In the Mirror dialog click Mirror Line and select the green (y-axis) line from center of the rectangle. Click ok on the Mirror Dialog. Click Finish Sketch.

2_Extrude Part Body

Click Create >Extrude. Select inside of the sketch profile of the part body rectangle. In the Extrude dialog, select symmetry from the drop down list next to the direction parameter. Click the "Whole Length" button next to the measurement parameter. Enter a distance of .08inch in the distance field and click ok.

3_Create Part Body Posts Sketch

Click Create> Create Sketch. Select the top of the extruded body that was just created.

Sketch Post

Click Create> Circle> Center Diameter Circle. Draw a circle in the the rectangle to the left of the center point. Click Create> Sketch Dimension. Select the center of the newly drawn circle and enter a diameter of 3.888mm.

Mirror Post Sketch

Click Create> Mirror. Select the sketch of the newly drawn circle. In the Mirror dialog click "Select" next to the "Mirror Line" parameter. Click the green line (y-axis) in the middle of the rectangle. Click ok on the Mirror dialog

Constrain Post Sketch

Click Constraints> Coincident. Select the center of the newly drawn circle then select the red line(x-axis) in the center of the rectangle. Click Create> Sketch Dimension. Select the center point in the circle located to the left of the rectangle center point then click the center point of the rectangle. Enter a distance of 13.411mm. Click Finish Sketch.

4_Extrude Post

Click Create> Extrude. Select the inside of each of the circles from the sketch. In the Extrude dialog, enter a distance of 3mm and a Taper Angel of -2. Click ok on the Extrude dialog.

Add Fillet To Posts

Click Modify> Fillet. Select top edge of Posts. In the Fillet dialog, leave all settings the same and enter a fillet value of .5mm. Click ok on the Fillet dialog.

5_Create New Rectangle Sketch

Click Create> Create Sketch. Select the top plane of the current model.

Sketch New Rectangle

Click Create> Rectangle> 2-Point Rectangle. Click on the top edge of the model, left of the model center and draw a rectangle to the right of model center.

Add Constraints To New Rectangle

Click Constraints> Symmetry. Click the left side then the right side of the new rectangle and click the green line(y-axis )in the middle of the model.

Add Dimensions To New Rectangle

Click Create> Sketch Dimension. Click the left edge of the new rectangle then the center point of the model and enter a dimension of 14.498mm. Click the bottom edge of the new rectangle then the top edge of the model and enter a dimension of 1.552mm. Click Finish Sketch.

6_Extrude Rectangle

Click Create> Extrude. Select the inside of the rectangle from sketch. Pull extrude arrow handle down through part body. In Extrude dialog, change Extend Type to "All" from Drop down list. Verify that "Cut" is selected from the Operation drop down list and click ok on the Extrude dialog.

7_Add Chamfer Feature

Click Modify> Chamfer. Select the inner corners on the part body from where the rectangular section was cut.

8_Mirror Features

Click Create>Mirror. In the Mirror dialog, select Features from the Object Type drop down list. Select the last two features (extrude and chamfer)from the timeline at the bottom of the screen. In the Mirror dialog, click "Select" in the Mirror Plane field. Click on the x-plane(Plane above the red line- x-axis in the middle of the model). Click ok on the Mirror dialog.

9_Add Fillets To Part Body

Click Modify>Fillet. select all vertical edges around the part body. In the Fillet Dialog, enter a value of 1mm. leave all other parameters default and click ok.

10_Export Part

Click Design> Utilities> Make> 3D Print. Select Part. In 3D Print dialog, Select "High" from the drop down list next to Refinement. Verify that in the Output section, "Send To 3D Print Utility" check box is unchecked. Click ok to save to a location.