In this session we will see how to build a model of a Bike Crank.
What is a Bike crank?
It is one of the components of a bicycle.
One end of the bike crank is connected to the sprocket wheel while the other end is
connected to the pedal.
When the bicycle rider presses his foot on the pedal, the bike crank revolves and causes
rotation of the sprocket wheel which drives the chain, this in turn drives the rear wheel.
So... how can we build this bike crank model?
Let’s analyze the shape first and plan how to build the model:
First we will take a look at the technical drawing.
Looking at the views, we can consider the bike crank as a rectangular shaped rod with
both ends having a circular shape.
So, we can first sketch the base using dimensions from the top view and then pull it to create
the base model of the bike crank.
Once we have the base model, we can create the holes at both ends.
Notice that the square shaped hole on the left side and the circular hole on the right
side cut through the entire thickness of the crank.
So, to save time and reduce the number of operations, you can first create the square
and circle sketches, then pull both the faces to create the holes.
Afterwards, you can sketch the circle around the square shaped hole and pull it downwards
to create a cut.
Finally, we need to create the slot at the center and add chamfers to the edges of the crank.
Looks like we have our plan!
First we’ll create the base, then the holes and finally, the slots and chamfers...
So let’s get started!
Open a new session of Discovery.
Close the Welcome screen and click the New button to open a new session.
By default, Discovery opens in the Explore stage which can be seen at the bottom of the window.
For this exercise, let us switch to Model stage.
Move the cursor over the left arrow of the Stage navigator at the bottom of the window
to highlight the Model stage and select it.
Set the plan view by pressing the letter V on your keyboard, and sketch the base shape
on the XY plane.
We will first sketch the circular ends of the crank.
Select the Circle sketch tool.
Click the origin to define the center of the circle.
Then move the cursor away from the center and type in 30 as the diameter and press Enter.
The first circle representing one end of the bike crank is created.
Next, we need to create one more circle at the other end.
The drawing shows that this circle is located 170 mm from the circle sketch that we just created.
With the Circle sketch tool still active, place the cursor at the origin but don’t click.
Instead, hit the Shift key to activate the reference dimensions.
Without exiting the first circle, move the cursor slightly to the right.
Make sure that the other reference dimension remains at 0.
Specify the horizontal reference dimension as 170 mm and press Enter.
The center of the circle is now defined at a distance 170 mm from the origin.
Move the cursor away from the center and type in 25mm as the diameter and press Enter.
The circle representing the other end of the bike crank is created.
We now need to connect the 2 circles.
From the drawing, we can see that the base shape is symmetric about the horizontal axis.
So, instead of creating the same sketch lines on both sides, we can take advantage of the
mirror functionality within sketching.
Select the Construction Line tool and create a construction line of any length along the
horizontal red axis.
Press S to activate the Select tool, then right click on the construction line and select
“Set as Mirror Line”.
This will make the construction line a mirror line and automatically create mirrored entities
of any sketch created above or below the construction line.
Let’s go back to the drawing.
If we look closely at the top view, we can see that there is a slanted line making an
angle of 1 degree with the horizontal axis.
The ends of this line are connected to the arcs and these arcs are connected to the circles
that we have sketched.
The arc dimensions are not provided.
However, it can be understood that these 2 arcs are tangentially connected to the slanted
line and the circle.
If we can get the dimensions of the slanted line, we can create the connecting arcs easily
using the Tangent Arc tool.
We can also see that one end of the slanted line is located 20 mm to the left and 10 mm
up from the center of the smaller circle.
Also, the length of this line is 130 mm.
So lets create it.
Select the Line sketch tool.
Hover the cursor at the center of the 25mm circle and press the Shift key.
Move the cursor left and specify a horizontal dimension of –20 mm
and vertical dimension of 10 mm.
Then press Enter.
The start point of the line is now defined.
Now let’s create a line with a 1 degree angle and length of 130 mm.
Notice that its mirrored entity will also get created.
Now, select the Tangent Arc tool.
Select either end point of the line to start creating a tangent arc.
Next, move the cursor over the nearby circle until you see a tangent constraint appearing.
This is indicated by two small parallel lines near the cursor.
Click on this location to complete the arc.
Similarly, create a tangent arc at the other end.
Notice that the new arc also gets created on the lower side of the horizontal axis.
We now have the outer sketch ready.
But, we need to remove the inner portions of the 2 circles in order to create a single
closed loop.
Select the Trim Away tool and click the inner circular sections to delete them.
The sketch is now ready to be converted to a solid model.
Return to 3D mode by pressing D on your keyboard and then press H to go to the home view.
Select the Pull tool and select the surface.
Drag the surface up and specify a thickness of 10 mm.
We have now finished building the base of the model.
Let’s create the 2 holes which are passing through the crank.
Select the top face of the base and go to the Plan view by pressing V on the keyboard.
Go to Sketch mode and select the Circle tool.
Hover the cursor over the circle on the right side of the crank and locate the center point.
Place a circle of diameter 12 mm.
Before moving forward, go to the Display tab and activate Fade Scene for convenience.
Next, we need to create the square shaped hole.
Notice that if we use the Rectangle tool, the rectangle will be aligned along the X
and Y axis.
However, the drawing shows that the edge is at a 45 degree angle with the center axis.
One way we can do this is to use the Line tool and create 4 lines at 45 degrees.
A better way is to use the Rectangle tool and create the square shape, then switch to
3D mode, create a hole, and simply rotate the hole by 45 degrees.
So lets do it!
Activate the “Draw from center” option from the Options panel.
Click the origin and create a rectangle of 12mm by 12 mm.
Return to 3D mode and press H for the home view.
The Pull tool is already activated.
First, select the circular face, then press the Ctrl key and select the square face.
Then pull both faces down to cut holes through the entire thickness of the crank.
The next step is to rotate the square shaped hole.
Select the top face and go to the Plan view.
Select the Move tool, then click and drag a box around the square.
At the bottom right of the window, you should see text indicating 4 faces are selected.
Select the Blue curved axis and drag it counterclockwise, then hit the Spacebar and specify an angle
of 45 degrees.
This completes the rotation of the square hole.
Next, we need to create a circular hole around the square shaped hole.
Select the top face again and go to Sketch mode.
Select the Circle tool and create a circle at the origin of diameter 20 mm.
Return to 3D mode and press H on the keyboard to go back to the home view.
The Pull tool is already activated.
Select the face around the square hole.
The front view of the drawing indicates that this hole has a depth of 3 mm.
So press the Spacebar and type a value of 3.
Then hit the Enter key.
Click Select in the toolbar to exit the Pull tool.
Notice that an extra square face is also created.
Select it and delete it using the Delete key on your keyboard.
The next step is to create the slots along the center of the bike crank arm.
A more efficient way to do this is to create a hole and then pull its center axis to create
the full-length slot.
Let’s see how we can do this.
Select the top face again and switch to Sketch mode.
Go to the plan view and click the Circle tool and create a circle of diameter 8 mm located
at a distance 85 mm from the origin.
This is half the distance between the 2 holes.
Start the Pull tool and pull the circular face downward by 2 mm.
With the Pull tool still active, hover the cursor over the cylindrical face to highlight
its axis.
Once highlighted, select the axis.
From the Options panel enable “Pull both Sides”
The drawing indicates that the length of the slot is 120 mm.
Press the space bar and specify a value of 120mm.
Repeat these steps on the other side of the crank to create a similar slot.
When you select the other face for sketching, you will see a mirror plane.
Select that plane and delete it before you proceed to sketching the circle.
The last step is to create the chamfers.
Double click on any outer edge of the model to select the entire edge loop.
Once selected, click the Pull tool.
Select the Chamfer option from the Options panel and press the Spacebar.
Specify a value of 1.5 mm and press Enter.
Repeat this process for the opposite side of the bike crank
and the circular edges located on the top face.
We can improve the look of the bike crank by modifying the color and the rendering options.
Select the body and click the Display tab.
You can change the color from the Color panel.
The bike crank is going to be made of metal, so we can try to give it a shiny appearance.
Select the body again from the model tree and expand the Rendering Style menu.
Select Metallic.
Finally, we can shut off the display of solid and tangent edges.
Select the Edges menu and clear the selection next to Tangent and Solid.
Let's save the bike crank model.
Go to the File menu indicated by the 3 horizontal lines.
Click the Save button and save the file.
We have now finished designing the bank crank.