Challenge

Door Arm Rest Design

Aim - Create the Door Armrest component using the given Class-A Surface of the armrest and the the door.

Objectives:

Create CLASS B and Class C Surface for the Door Armrest using the given Class A Surface.
Use the given Class A Surface of the Door for reference.
Use the Close Surface feature to make a solid body from the surface.
Use the publication option and publish the Class A, Class B, Class C Surfaces and the tooling axes.

Tooling Axis:

The first step in creating the other surfaces is the construction of the Tooling Axis.

Extract the boundary of the hole in the Class A surface and fill it. Create a point on the surface at the centre using the Point command.
Put the Class A surface in the material mode and open the Feature Draft Analysis Tool.
Select the surface and drag the compass onto the surface.
Now the orientation of the compass can be changed and the draft analysis can be visualized simulataneously.
Lock the compass at the position where the draft analysis gives the best results.
Use the previously created point and the compass direction to construct a line which is the main tooling axis.
Follow the same steps for the pocket region and lock the compass orientation
Extract the rib surface and untrim it:
Create a point at the centre of the untrimmed surface. Create a line using the point and the direction of the compass.
This will be the second tooling axis.
Finally, use the Publish feature to publish both the tooling axis and the Class A Surfaces.

Class B Surface:

Pocket:

Extract the pocket surfaces from the Class A surface:
Untrim the extracted surfaces and then extrapolate the untrimmed surfaces such that they intersect each other:
Offset the extrapolated surfaces to a distance of 2.5mm and trim them together:

Middle Surface:

Fillet Surface:

The fillets at the backside of the Class A surface can not be created directly because is both the surfaces are trimmed together, there will only be a single surface but there are two fillets:
Extract the fillet edges from the Class A surface:
Create midpoints on both the extracted curves and join them to construct a line:
Use the multi extract feature to extract the shared edges of both the fillets which will act as a guide curve:
Use the Sweep feature with subtype as 'With Reference Surface'. Choose the previously created line as the profile and the extracted curve as the guide curve:
Use the Surface Simplification feature on the swept surface. Extrapolated the smooth surface and offset it to 2.5mm:

Inclined Strip:

Back Surface:

There are two surfaces on the back wall. Extract both the surfaces and untrim them:
Extrapolate and offset both the surfaces to 2.5mm:

Top Surface:

Hole:

At the bottom of the Class A Surface, there is a hole with inclined cylindrical walls. Firstly extract the boundary of the hole and then the cylindrical surface:
Extrapolate the surface in both directions and create its offset of 2.5mm:

Final Trims:

Before trimming all the surfaces together, the inclined surface needs to be modified.
On the inclined surface, create curves using the 'Parallel Curve' feature such that the curves do not touch the pocket surface.
Trim these curves and split the inclined surface using these curves:
Trim the pocket surface and the middle surface together:
Trim the upper back surface and the last trimmed surface together:
Trim the fillet surface and the last trimmed surface together:
Trim the modifies inclined split surface and the last trimmed surface together:
Trim the top surface and the last trimmed surface together:
Now trim the lower back surface and the last trimmed surface together:
Finally, trim the frustum surface with the last trim:

Fillets:

Provide fillets on edges taking reference from the Class A surface.
The fillet radius needs to be chosen keeping in mind the thickness of the component such that when the final part is created, it has a uniform thickness of 2.5mm:

Class B Surface

Class C Surfce:

Extract the enclosing walls of the outer flange using the Multiple extract feature:
Use the Swep feature using the extracted boundary as the guide curve and the Class A surface as the reference surface
Now extract the hole boundary and similarly speep it using the Class A surface as the reference surface.

Closed Surface:

Join the Class A surface and the Class C surfaces using the Join feature:
Finally, trim the the above surfaces and the Class B Surface:

Closed Surface

Solid-Body:

Use the Close Surface feature and select the above surface to create a solid part.

Part Body

Draft Analysis:

For the draft analysis, open the Feature Draft Analysis tool and drag the compass to the main tooling axis and select the body:

Draft Analysis (main tooling axis)
For the draft analysis of the pocket region, gain open the feature draft Analysis tool and drag the compass to the second tooling axis and select the body:

Draft Analysis (side core tooling axis)

Conclusion:

The main tooling axis and the side core tooling axis have been created successfully using the Feature Draft Analysis Tool.
Class B and Class C surfaces have been successfully created using the Class A surface as the reference.
Final Closed Surface has been created by using the Trim and Join feature.
The part body has been created using the final closed surface.
Draft analysis has been successfully done on the part body.

Ship work like this
in your own course.