Designing your Part (Autodesk Fusion)
This Guide demonstrates how to create a part using Autodesk Fusion 360. The designed part will be used with a Holder for the LIDAR Sensor.
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This Guide demonstrates how to create a part using Autodesk Fusion 360. The designed part will be used with a Holder for the LIDAR Sensor.
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Click Design > Create > Create Sketch. Select the top plane
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.
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.
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.
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.
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.
Click Create> Create Sketch. Select the top of the extruded body that was just created.
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.
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
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.
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.
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.
Click Create> Create Sketch. Select the top plane of the current model.
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.
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.
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.
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.
Click Modify> Chamfer. Select the inner corners on the part body from where the rectangular section was cut.
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.
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.
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.
