PLASTIC DESIGN OF A COIN HOLDER USING CATIA V5

PLASTIC DESIGN OF A COIN HOLDER USING CATIA V5

OBJECTIVE

To design a coin holder used in automobiles using Catia V5 using a Class-A surface as input and performing draft analysis on the component to ensure manufacturability

INTRODUCTION

Manufacturing process: Injection Molding

Brief about the process

It is a manufacturing process used for the mass production of plastic components. It works by injecting molten material (plastic) into a mold. Under the application of heat and pressure, the material solidifies into the required shape. Once the product cools, it is ejected from the mold with the help of ejector pins.

Terms in the injection molding process associated with this project

Draft

To facilitate easy removal of components from the mold, it is necessary to add a taper all along the surface with reference to the tooling direction. This taper is termed as a draft and its value ranges from 0.5 degrees to 3 degrees, with the latter being the most widely accepted norm.

The Draft analysis command in CATIA enables to detect if the drafted part can be removed in an easy manner. This analysis is performed based on colour ranges identifying zones on the analyzed element where the deviation from the draft direction at any point, corresponds to specified values.

Tooling direction

The direction along which the core pulls apart from the cavity is termed as the Dyeline or the Tooling direction.

Software : CATIA V5

CATIA (an acronym of Computer Aided Three-dimensional Interactive Application) is a multi platform software suite for CAD, CAM, CAE, PLM and 3D , developed by the French company Dassault Systèmes.

The version of CATIA used for this project is V5. For the target model, the features in the part and surface workbench were extensively used.

Target Model: Coin holder used in automobiles

A coin holder is a plastic component usually found in automobile interiors especially as a part of the door arm rest.

Terms in CAD associated with this project

Class-A Surfaces

The aesthetic/free-form surface which constitutes the visible outer layer of a component can be termed as a Class-A Surface. In this project, the Class-A surface of a coin holder which is composed only of curvature continuous surfaces is used as the input for performing the draft analysis.

B and C Surfaces

The B surface forms the inner components and acts as a base for the Class-A surface. C surface connects the A and B surfaces and thereby provides a thickness for the final component

Tools in CATIA associated with this project

• Sketcher workbench: Point, Line, Intersect 3-D elements
• Part workbench: Close surface
• Surface workbench: Boundary, Extract, Multiple extract, Untrim, Extrapolate, Offset, Trim, Join, Edge fillet

Methodology in CATIA associated with this project

Bisecting line method

Since draft is measured with reference to a tooling axis, the first step after importing the model into CATIA was the creation of a tooling axis. To incorporate for tool clearances due to the presence of tapered surfaces in the part, the bisecting line method was used to create the tooling axis.

After converting the surface into a 2D profile using the Intersection command from the surface workbench, two inclined lines were created using the endpoints of the 2D curves which represented the tapered faces. Using a bisecting line type, a third line was created along the centre point which signified the coincidence of the tapered faces. This line was the required tooling axis for this component.

NOTE: This project did not have features which needed a titled tooling axis and hence the tooling axis was created using a bottom face extract and creating a line through the centre point.

Draft Analysis

The draft analysis command in CATIA helps to detect whether the drafts provided in the model will facilitate easy removal of the component during manufacture.

This analysis is performed based on colour ranges identifying zones on the analyzed element where the deviation from the draft at any point, corresponds to specified values.

• When the draft angle value of the surface is equal or smaller than a graduated value, the color below the graduated value is applied
  
  
• When the draft angle value of the surface is greater than the greatest graduated value, the color above this graduated value is applied
  
  

In this project, the required draft for all surfaces were chosen as 3 degrees and hence the quick mode option in draft analysis was chosen which incorporated two different colours for two input values.

B and C surface creation

The B surface was created by offsetting the Class-A surface and then extrapolating it to accommodate the entire area of the Class-A surface.

The C surface provided the thickness and acted as the joining surface between Class A and B surfaces.

The Class A and C surfaces were made into a single surface using the Join command in the surface workbench. This was then trimmed (Trim tool) using the B surface to create the final component. The model was then converted into a solid using the Close Surface command.

DETAILED PROCEDURE

1. Importing the Class-A Surface and checking for surface irregularities

• The Class-A Surface model of the coin holder is imported into the Catia workspace

• Since the model was imported, a detailed check to detect surface irregularities was done using the Boundary tool

2.Creation of the main tooling axis

• The first step towards checking the component for manufacturability was to conduct a draft analysis on the imported Class-A Surface
• To successfully perform a draft analysis, a proper tooling axis needed to be determined first, along which the mould halves separated
• In any model, the pocket/bin area should be the focus area for tool clearance. Keeping this in mind, the bin area for the coin holder was considered for determining the main tooling axis
• The base face of this bin was extracted and it was found that the all the side walls were perpendicular to the base

• Hence a centre point was created in the extracted face and an axis system was inserted into it

• Then, a line was created in the Z direction which was chosen as the main tooling axis

3.Performing draft analysis on the Class-A Surface

• To check the component for manufacturability, a draft analysis needed to be done before proceeding to the subsequent stages
• Using the Feature Draft Analysis tool offered by CATIA, the performance of the model under a 3 degree draft condition was analysed
• The draft direction was chosen by dragging the compass and coinciding it with the tooling axis
• The quick analysis mode was chosen since the draft value chosen for this project was 3 degrees for all the surfaces of the component
• It was observed that the Class A Surface was clearing the draft conditions successfully

4.Creation of B surface

• Once the analysis on the class-A model was done the next step was to create the B-Surface for the model
• The Class-A Surface features were analysed and according to the B-surface creation procedure followed in this project, different regions were selected and assigned different colours and appropriate names

• The steps followed for each areas were the same:

1. The surfaces to be made into the B surface were first extracted using the extract tool
2. To remove dependencies with the original surface, these extracted surfaces were then made independent using the untrim tool
3. In order to join these independent surfaces, they needed to be extended to form interference between adjacent surfaces. For this the extrapolate tool was used
4. To remove unwanted extensions in the surfaces after interference, the trim tool was used and the result was a single surface
5. Since the idea behind creation of a B surface is to have an offsetted surface from the input class A surface, the next tool used was the offset tool

Step 1: Extracting the required surfaces

Step 2 : Untrimming the surfaces

Step 3: Extrapolating the surfaces

Step 4 : Trimming the surfaces

Step 5: Offsetting the surfaces

• Proper fillets were added to the sharp corners using the edge fillet tool

Fig: B Surface

5.Creation of C surface

• The C surface forms the connection between the Class-A and B surfaces and is essentially the thickness of the final component
• The C surface was formed using the sweep tool
• For this command, the side flanges and its boundary were extracted from the Class-A Surface and then swept to form the C surface

Fig: Extracted surface and boundary for creation of C surface

Fig: Sweep Tool

• The cutout in the bin area was also added to the C surface using the sweep tool

6.Creation of the final surface model

• To create the final surface model, the B and C surfaces were first trimmed and joined together using the trim tool

• The combined surfaces were then joined with the Class-A Surface using the join tool to create the final surface model of the coin holder

7.Creation of the solid model

• Before converting the surface model into a solid model, the part was first opened using in the part workbench
• The close surface tool was used to convert the surface model into a solid model

8.Performing draft analysis on the solid model

• Similar to how the draft analysis was done on the Class-A surface, a separate analysis was done for the solid model as well, with respect to the main tooling axis

9.Publishing the necessary components

• Publishing geometrical elements makes them available for different users and is important from an assembly context
• In this project, the Class-A, B, C surfaces and the tooling axis were published

DRAFT ANALYSIS: RESULTS (With standard views)

• Class-A surface:

• Solid model:

FEATURE TREE OF THE MODEL

STANDARD VIEWS OF THE SOLID MODEL

TOP VIEW

SIDE VIEW

FRONT VIEW

ISOMETRIC VIEW

CONCLUSION

This project imparted a great deal of knowledge regarding the creation of tooling axis, concept of side core and performing proper draft analysis on a component which are essential steps to ensure a design is fit for manufacture. It also provided valuable insights on the design of a plastic component using Class A, B and C surfaces using CATIA.