Week 9 - Project - Master Section Development

AIM - 

The Aim of this project to develop a closed surface model by using of the master section and developed B side feature for locked the degree of freedom of the component. Here we can use B Pillar master section providing by the OEM Standards.

ABSTRACT:-
The report details about the Design Life Cycle in Automotive Industry with a practical working model of B PILLAR COVER on the B PILLAR of Car Interior. The report explains the steps followed in creating the tooling axis followed by detail methods in creating B-Surface, Class C Surface and to closed body. The Attachment features creation is also reported by following the design guidelines and finally analysis of Draft to prevent the failure and improve the feasibility of manufacturing the part in plastic injection moulding.

OBJECTIVE:

• To ensure proper tree structure is followed.
• Creating a tooling axis and following design rules.
• Creating CLASS B and C surface using CLASS A surface as an input. 
• Following the master section to create flange.
• Following the master section for thickness and to create the closed volume.
• Following the master section to create Attachment features.

Given Class A Surface and Master Sections:

                                                                       

DESCRIPTION:

MASTER SECTION:

Master Sections are the guides for design requirements which shapes the component after technical styling of Class A Surfaces The body frame is mainly composed of floor longitudinal beams, upper side beams, door side beams, and front cover, the rear beam, A-pillar, B-pillar, C-pillar, and other load-bearing beam structures are composed.

Master Sections are parameterized model of the vehicle body that outlines the guide for NPD Team.
In this Report B Pillar Cover Creation with detailed procedures of Surface Development and Attachment features are covered.

OVERVIEW DESIGN LIFE CYCLE AUTOMOTIVE INDUSTRY:
The Stages of Design Life Cycle are:

• Concept Sketches: Concept sketches are rough idea of free hand sketch obtained through styling team and will be used to prepare the Model. It is usually done through pen and paper and through the painting software. This will be used to generate the concept for preparing the model by incorporating various styles and information obtained through the stakeholders.
• CLASS A Creation: -After finalizing the concept the sketches are usually worked in software’s such as Autodesk Alias to create Class A Surface.
• Clay Modelling: -The Class A Surface is concurrently worked by clay modelers to brainstorm and benchmark the styling of the product and later the Concept is validated by bringing up a rough clay model and then it is passed on to the Design team for the preparation of New Product Design (NPD) CAD.
• NPD CAD-This where the development of surfaces to parts in CAD kick off and Design engineer’s involvement is vital in this stage. The Designers will work on the Input Class A surfaces which are validated from the Feasibility team.

PROCEDURE:

The procedure followed in creation of the plastic New Product Design are

• Tooling Axis
• B Surface Creation
• C Surface Creation
• Closed Body Creation
• B Side feature Creation
• Side core Axis creation
• Draft Analysis

The given Class A input is analysed to envision the part to manufacture and Tooling axis or Tooling Direction or Die line is the direction that moulds pull apart in injection moulding. There are two mould pieces names core and cavity.

Thus, tooling direction determines Mould separation and also becomes vital in developing the plastic product which is drafted to desired nominal angle for feasible clearance and ejection of final part from the mould.

CREATION OF TOOLING AXIS:
The Steps Followed in creating Tooling Axis:

• A Reference Point is created along the Surface zero and new Axis system is created.
• The X Direction and Y direction along the Class A were used to create Tooling direction.
• Finally, the Tooling axis is created by bisecting the two lines which provide the Master section, and it is published. Class A Surface as input using surface operation commands Class B is developed.
• The tooling Axis determines the direction of Class C boundary swept with draft direction and Draft provide in tooling axis direction.
• When viewing from tooling direction normal all the parts that are drafted should be visible, so it gives a rough idea to determine product manufacturing in Injection moulding.

In B Pillar Model there are Two Tooling Directions one on Main tooling and other on Lifter Side that is used to eject the parts during injection moulding.

Lifter Axis is used because the Attachment feature is bounded by close walls.

Extract the sides of the Master Section.

    

Extract the sides of the other Master Section Also.

   

Then create a bisector for these Extracts.

  

Then the bisection of these bisectors is the Actual tooling axis created.

  

CREATION OF CLASS B SURFACE:

To create the Class B Surface, select the Class A surface and offset the surface to 2 mm.

  

After offsetting the surface, we can observe that the CLASS B surface is having a patch / missing surface. This surface needs to be fixed by manually creating a surface.

To create a surface over the patch, we first need to extract the boundaries of that edges separately and using the “multi section” option a new surface can be created. Now join this patch surface with the offset surface to form a CLASS B surface.

   

So, to clear this use multi section surface option to close the gaps formed.

   

The gaps formed is closed and the Class B Surface Formed is Ok.

   

CREATION OF FLANGE:

From the master section it can be observed that the B Pillar is having Flange but the CLASS A surface which was given to us as input do not have any Flange

  

So, to create a Flange on both A & B surfaces we first need to extract the boundaries of the CLASS A / B surface as shown in figure below.

  

After extracting the boundaries, apply a smooth option to it to avoid any surface continuity issues.

Surfaces of CLASS A / B which are attached to the boundary need to be extracted first which will act as a reference surface for the Flange while sweeping.

Now sweep the boundary with the reference surface (surfaces which we extracted) and give an appropriate angle such that the Flange is aligned with the master section.

  

Offset the Swept Surface to 2mm.

  

Similarly, Do it on the other side of the B Pillar.

 

  

 

Now Join the Sweep surface with the Class A surface and the Offset surface with the Class B Surface to get surfaces attached with a Flange.

 

CLASS C SURFACE CREATION:

To create a CLASS C surface, first extract the boundaries (all edges separately) of the CLASS A surface (the surface with FLANGE) as shown in below figure.

  

After extracting the boundary, we need to perform smooth (max. Deviation as 0.001mm) operation on it to create a continuous tangent surface.

  

Now using the ‘sweep’ option create the surface. To perform this operation, go to the Toolbar > Sweep > Profile type > Line > Subtype > With draft direction > Guide curve 1 - (select the extracted boundaries) > Draft direction - (select the tooling axis) > angle as 3 deg and give any suitable length and press ok.

Note: The boundaries of the CLASS A surface need to be extracted separately and the sweep operation also needs to be performed separately. It is not possible to create a C surface with a single sweep following the Draft Direction.

  

Once these sweep surfaces are created, trim them to join the surfaces. This will give us a CLASS C surface.

   

FINAL TRIM:

To create the B Pillar component, we need to join all these surfaces (i.e., CLASS A, B and C surfaces).

First join the CLASS A surface with the CLASS C surface and then trim this joined surface with the CLASS B surface to get the final output.

  

CLOSED SURFACE:

Since these surfaces are hollow, we need to close it to form a thick solid component. 

Using the “CLOSE SURFACE” option in PART WORKBENCH, a solid body from the surface can be formed. This will give us a solid component.

   

ENGINEERING FEATURES:

DOGHOUSE:

Doghouse is an engineering feature that is used in plastic trim design. It is used as a supporting feature for other engineering features like snaps, locators etc. that are mounted on the Doghouse to increase their strength and to avoid the sink marks.

To create a Doghouse, we need to follow the master sections which were given to us as an input. The top surface and the supported walls of the Doghouse on which the locator is laid is created by simply extracting the lines from the master section in a sketch and extruding it to a certain length as shown in figure below.

      

Now with the Help of Master Section 2 extract a line to create a closing surface to the Doghouse.

     

Trim it with the main surface and Give a thickness of 2mm to it and Draft it to an angle of 0.5degrees.

      

Locators are a great way to make sure the parts we are putting together fit the way we want them to fit. To create a 4-way locator, we need to create a sketch with two lines intersecting each other perpendicularly forming a ‘+’. Once the sketch is created, pad it to form a locator.

Note: The 4 - way locator is created on the top surface of the Doghouse following the master section.

A draft of 0.5 deg is given to the locator and a chamfer of 5 mm at 45 angles is given to the top edges of the locators.

     

The inner walls of the Doghouse are created at an offset value of 1.2mm from the outer walls and the top surface for the inner walls is created by intersecting the CLASS A surface with the back wall of the Doghouse.

This surface is then split with the close solid to create the inner walls of the Doghouse.

    

    

    

To draft the inner walls of the Doghouse, a lifter axis is first created and then a 0.5 deg draft is given to it following the draft direction of the lifter tooling axis.

The inner walls of the Doghouse are created at an offset value of 1.2mm from the outer walls and the top surface for the inner walls is created by intersecting the CLASS A surface with the back wall of the Doghouse.

This surface is then split with the close solid to create the inner walls of the Doghouse.

   

RIBS:

Ribs are created to increase the strength of a part without increasing the thickness of its walls. Because less material is required, ribs can be a much more cost-effective solution as well.

To create a rib, we first need to draw a straight line (where we want a rib) in the sketcher workbench. After creating the line, extrude it and pad it.

   

   

Since we need to create multiple ribs which are 50 mm apart, first go to the CLASS A / B surface and extract the boundary/edge where the flange is connecting to the main body. Now using these boundaries, create repetition points which are at 50mm from each other.

Now copy the rib (solid body) which we created and paste it in the main tree structure. Using the translate option the copied rib can be moved from one point to another. Repeat the above step for creating all the ribs and position it on the points that we have created using the repetition points option.

Offset the CLASS B surface to 10 mm and trim the ribs with it removing the excess portion of the ribs and give a draft of 0.3 to the ribs.

  

Create the ribs on the other side also.

  

Once all the engineering features are created, add it /trim it to/with the main body i.e., B Pillar and give appropriate fillet value to all parts of the body.

  

DRAFT ANALYSIS ON FINAL MODEL:

To perform Draft Analysis on the 3D CAD model, go to menu bar > select insert > Analysis > Feature Draft Analysis.

To give draft direction, use the compass and align it with the tooling axis which we created for the model. Once it is properly aligned, select the surface of the model which will show us the draft angle given on the component. Make sure the draft angle on the component is having 3 deg draft value (component showing green in colour). 

MAIN TOOLING AXIS:

  

LIFTER TOOLING AXIS:

  

Note: Draft value ranging from 0 - 3 deg will show the component Blue in colour.

Using the Analysis option under Display Tab, we can check / analyse the exact draft value at any point on the given model.

3D CAD MODEL:

  

Tree Structure: