Week 9 - Project - Master Section Development

Aim: To design B-Pillar lower using the Master section.
Objectives:
Create a closed body of the Given B pillar Lower.
Crete tooling axis and follow design rules.
Follow the Master section to create a flange.
Follow the master section for thickness and to create the Closed volume.
Follow the master section to create Attachment features.

DESCRIPTION:

MASTER SECTION:

Master Sections are the guides for design requirements that shape the component after the 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 guidelines for the NPD Team. In this Report, B Pillar Cover Creation with detailed procedures of Surface Development and Attachment features are covered.

OVERVIEW OF DESIGN LIFE CYCLE AUTOMOTIVE INDUSTRY:

The Stages of the Design Life Cycle are:

Concept Sketches: Concept sketches are rough ideas of freehand sketches obtained through the 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 from the stakeholders.

CLASS A Creation: -After finalizing the concept the sketches are usually worked in software such as Autodesk Alias to create Class A Surface.

Clay Modelling: -The Class A Surface is concurrently worked by clay modellers 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.

PROCEDURE:

The procedure followed in the 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 the 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 the final part from the mould.

Step 1: Create a tooling axis.
For creating the tooling axis first we extract these 4 boundaries.

ook a point between this 2 lines

then draw a bisecting line between this two line by using point

again bisect the remaining two lines

and finally, bisect the resultant lines.

finally, we got the tooling axis

Step 2: Draft analysis on Class A surface

Step 3: Creation of Class B & C Surface.
According to the Master section, our component has a 2 mm thickness so we offset the class A surface by 2mm.

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 are 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 does 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 the 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. and now provide the fillets by measuring in class A

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

trim the sweep after extrapolating them.

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.

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.

ENGINEERING FEATURES:

DOGHOUSE:

Doghouse is an engineering feature that is used in the 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 input. The top surface and the supporting walls of the Doghouse on which the locator is laid are created by simply extracting the lines from the master section in a sketch and extruding them to a certain length as shown in the figure below.

thicken the surface by 2 mm since the given master section is 2 mm

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.

now translate the dog house by taking the midplane between the master section reference by plotting the plane using a parallel through the plane.

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 that are 50mm from each other.

Now copy the rib (solid body) that we created and paste it into 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 them 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 giving 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 OF 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 values 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.

tree structure:

CONCLUSION:

A component with the engineering features such as ribs dog house, flanges has been created by using the design considerations and rules for the given class A surface and draft analysis is performed.