Simple propeller guard tutorial PDF

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Download Simple propeller guard tutorial PDF

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To create a simple propeller guard Open a new part in Solidworks

Click on the top plane and sketch toolbar, "sketch"

On the sketch toolbar click the arrow at the side of the square, on the drop down menu select "center rectangle"

Hover over the origin until you see and orange dot, click to select it, then click to one side and above the origin. Right click and click select to exit the tool.

You can then use "smart dimension" to set the size you require to fit on your car. Click on the Features toolbar, select "extruded boss/base"

Select the thickness of the base that you require at "D1"

Choose the front face of the block you have just drawn and sketch toolbar, "sketch", if the drawing surface is not facing you, click on the arrow at the side of "view orientation", select the "normal to"

button. This will turn the selected plane to face you.

select "centreline" and click on the origin, drawing vertically up to an appropriate height to allow for the propeller.

Click on the "Circle" sketch tool, hover over the top of the centre line and click the dot when it turns orange, moving out and then click on the origin to set the size. The size of the circle can be set using the "smart dimension" tool.

Draw another circle from the centre of the first, to inside the diameter. Use "smart dimension" to set the distance between the inner and outer circle.

Click on the Features toolbar, "extruded boss base" and choose the "D1" dimension to suit. Click the tick.

Click on the rear surface of the circle, on the same side as the base block. Click "sketch"

Turn the sketch "normal to" your view point. In the centre of the circle you have drawn, to find the centre hover near the middle and it should show up

. Click on the centre and move out, click again to set your size. set the diameter of the circle using "smart dimension"

Using the "line" sketch tool draw a line from the centre of the small circle to the outer edge of the large ring.

Click on the "offset entities" sketch tool , click on the line you have drawn, ensure you have ticked the box for "bi-directional" on the side bar, choose how far you want the line to be on either side of the original line.

When you are happy with the distance, click the tick. Draw a line across the bottom to join the ends of the outer lines. Click the tick when done

To trim the lines inside the circle that are not needed use "trim entities" choose "power trim", click and hold the button on the left of the lines you want to remove, drag through and release on the other side.

Click on the central line that you have drawn, in the side bar that opens, tick the box that says "for construction". Click the tick.

Click on the arrow at the side of "linear sketch pattern", select "circular sketch pattern"

Ensure the parameters box is blue (if it contains anything, you can click on the box, right click and delete it) then click the centre of the circle. Ensure that "equal spacing" is ticked and choose how many times you want to repeat the pattern. Under "entities to pattern" choose the two outer lines that you have just drawn and the line at the bottom that connects them. click the tick when you are happy with it.

Trim the lines using "trim entities", as shown.

In the centre of the circle, draw another circle to be a hole for the bar to attach to the propeller.

Select the "features" toolbar, click "extruded boss/base", choose "D1" dimension to suit.

Under "Direction 1" on the sidebar, at the side of "blind" direction arrow, click this to reverse the direction of the extrude. Click the tick.

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Click on the front plane and click "sketch", turn the view to "normal to".

Click on "convert entities" blue.

on the toolbar, ensure that the "entities to convert" box is highlighted

Click on the top edge of the base and the rear edge of the large diameter that sits perpendicular to the end of it. Click the tick.

Draw a line to connect the two extremes, joining the propeller cage upright line below the centre hole drawn.

Using "trim entities", trim the dangling edges of the lines outside the triangle shape you have drawn. Click the tick.

On the features toolbar, select "extruded boss/base". Under "direction one, change the tab "blind" to "mid plane". Under "selected contours" ensure the box is highlighted blue and click inside the triangle region you have drawn. then click the tick.

Click on the top surface of the base, click "sketch", on the "View Orientation", click "normal to"

Draw a "centerline" on either side of the base. Click "circle" and draw what will be some fixing holes on the surface aligned on the centreline you have just drawn..

Use the "smart dimension" tool to dimension the hole sizes and distance from the edge and the hole next to.

On the "Features" toolbar, click "extruded cut" Ensure the four holes you have drawn are highlighted, under "Direction 1" change "blind" to "through all". Click the tick.

Don't forget to save your finished part....