Bumper Design

OBJECTIVE: To create the Bumper's Plastic-Component using the Class A Surface that is provided. Desired Thickness of the Plastic Component is 3mm with 3 degrees as the Draft Angle.

 

Firstly, we have to create the required Tooling-Axis for the given Class A Surface while meeting the requirements of the necessary Draft Angle & then perform the Draft-Analysis Operation on the Class A Surface itself.

After that, we have to create the required Class B & Class C Surfaces using which we have to create the Final Plastic Component and perform Draft Analysis on it.

MAIN REPORT:

Types of Surfaces and their Importance for an Automotive Plastic Designer:

• Class A Surface: Class A is an aesthetic surface with the highest quality finish. Most Class A Surfaces for an Automotive Component are made using 'Autodesk-Alias' based on the final Concept-Sketch. All Class A surfaces should have 'Curvature-Continuity' which means the continuity between the surfaces should share the same boundary. It is taken as a reference by the Automotive Plastic Designer to create 'Class B' and 'Class C' Surfaces.

 

• Class B Surface: The Class B Surface resides below the Class A Surface at a certain thickness. It is created using Engineering Principles that consist of all the necessary features such as Ribs, Bosses, Snaps, etc. This surface isn't visible to the observer from the outside.

 

• Class C Surface: The Class C Surface is the surface created between the Class A and Class B surfaces to join them with each other.

 

Now, we will begin by checking the State of Connectivity for the Class A Surface and ensure that there are no gaps between the surfaces as all the surfaces should be joined well together with each other and shouldn't consist of any discontinuities between them.

 

Our Class A Surface:

 

There are two methods to inspect the State of Connectivity for the Class A Surface:

1. Using the 'Join' Command' from the 'Operations Toolbar':

First, we'll click on 'Join Command' and select our Class A Surface. Then, we have to ensure that the 'Check Connexity' option is marked as shown in the images below. It will check for any gaps that may be present between our surfaces. Then, we'll click on the 'Preview' button and if it doesn't show any 'Connexity Error' on our surface then it means our surface is well-connected and there are no discontinuities between it.

In our case, there are no 'Connexity Errors' for the given Class A Surface.

 

2. Using the 'Boundary' Command' from the Operations Toolbar:

In this case, we have to click on the 'Boundary' command and then select the Class-A Surface. After that, we'll click on the 'Preview' button to highlight all the boundaries on the Class-A surface and check if there are any internal boundaries other than the outer edge.

In our case, there are two boundaries present on the Class-A Surface one of which is the Outer-Edge Boundary & the other is Inner Hole-Boundary meant for the Fog-Light's section. Hence, we can conclude that all the surfaces are well connected. 

 

PROCEDURE TO CREATE THE MAIN TOOLING AXIS:

There are two different methods that we can use to create the Main Tooling Axis for our Class A Surface.

1. Using a Vertex to create a line along the axis which allows us to view all the holes & exposes a maximum surface area of the Class A Surface.

2. Using Inertia Method to find out the Center of Gravity and create a line along it.  

 

First, we'll view the Class A Surface from all three axes to determine the most suitable axis along which the Main Tooling Axis can be created.

A) VIEW ALONG THE Z-AXIS:

From the above image, we can observe that not much area of the bumper is exposed here and we cannot view either the hole section, not the cutout section from this viewpoint hence this will not be the appropriate direction for the Main Tooling Axis.

 

B) VIEW ALONG THE Y-AXIS:

From the above image, we can observe that although more area is exposed along this axis compared to the previous axis it is not sufficient as it'll be difficult to create the hole section and the cutout section from this direction. 

C) VIEW ALONG THE X-AXIS:

From the above image, we can observe that here the maximum amount of the bumper's surface area is exposed and we can view both the hole section & the cut-out section of the bumper concurrently hence making this direction the most suitable choice for the Main Tooling Axis.

 

FIRST METHOD TO CREATE THE MAIN TOOLING AXIS:  

Now, to create our Main Tooling Axis using the first method, we'll choose a vertex as shown in the image below to create a line using the 'Line-Definition' command while choosing our Line-Type as 'Point-Direction' where our direction will be towards the X-Axis.

We're not 100% certain that this will be our Main Tooling Axis and to finalize it we have to perform Draft-Analysis and find out if that'll be the appropriate direction. 

 

SECOND METHOD TO CREATE THE MAIN TOOLING AXIS:  

We'll click on the 'Measure Inertia' icon from the 'Measure Toolbar' as shown below:

We'll select our Class A Surface that will open up the 'Measure Inertia' dialogue box as shown below:

After that, we'll click on the 'Create Geometry' option in our Measure Inertia Window that'll open up the 'Creation of Geometry' window. 

There we'll choose 'Non-Associative Geometry' and then click on 'Center of Gravity' to create the required C.G point as shown below:

 

Now, using the 'Line-Definition' command while choosing our Line-Type as 'Point-Direction' we'll create a line along the X-Axis as shown below:

 

 

DRAFT ANALYSIS FOR THE CLASS A SURFACE USING THE MAIN TOOLING AXIS FROM THE FIRST METHOD:

Now, We will perform a Draft Analysis on the Class A Surface itself using the Main Tooling Axis created using the First Method:

Before starting with a Draft Analysis Operation, we will go to the 'Customize View Parameters' option under the 'View Toolbar'. Then we will enter the 'Customize View Mode' where we will go under the 'Mesh' option and select 'Material' and press 'OK'. 

To start the Draft Analysis in the 'Generative Surface Design Workbench', we will go to 'Insert' and then look for the option called 'Analysis'. Once found, we will go under that and click on 'Feature Draft Analysis. This will open the 'Draft Analysis' Dialogue box. There, we will ensure that under 'Mode'  we have selected 'Quick Analysis', under 'Display' we will select 'Show or Hide the Color Scale' and then select '3 Degrees' as the permissible draft angle. Then, under 'Direction' we will choose the icon with the symbol of the compass on it which stands for 'Use the Compass to define the new current draft direction'.

It is evident from the above image that the Draft-Analysis on our Class A Surface was successful and the component is feasible to manufacture.

 

DRAFT ANALYSIS FOR THE CLASS A SURFACE USING THE MAIN TOOLING AXIS FROM THE SECOND METHOD:

It is evident from the above image that the Draft-Analysis on our Class A Surface was successful and the component is feasible to manufacture.

Hence, we can see that the Draft Analysis was successful along both the Tooling Axes, and hence either one of them can be used as our Main-Tooling Axis. 

 

PROCEDURE TO CREATE THE CLASS B SURFACE:

We'll start the procedure by creating an offset for the entire Class A Surface at a distance of 3mm as that is the desired thickness for our final plastic component.
As this is a complex surface hence the offset will fail to offset every element according to our necessity. It'll select some sub-elements that belong to the filleted regions by themselves that we have to remove to get the rest of the surface that is offset.

This warning will be shown when we'll try to offset the Class A Surface.

These 'Sub-Elements' will get selected by themselves to be removed if we want to obtain the rest of the offset surface.

In the above image, CATIA is showing us the filleted regions where these sub-elements are located that are going to be removed after the offset operation.

 

 

 

 

Now, we're going to fix these patches by recreating these sub-elements using various tools such as Extract, Untrim, Extrapolate, Multi-Sections Surface, Trim, etc. 

1. FIRST REGION:

CLASS A SURFACE: GREY IN COLOR GREY 

CLASS B SURFACE: LIGHT BROWN IN COLOR BROW

From the above image, we can notice that two patches that were present on the Class A Surface are not present on the offset surface. These regions are shown using the arrows and we need those patches of surface to perform further operations. Hence we will extract those surfaces from the Class A Surface and Offset them. After offsetting both these surfaces, we'll use the 'Join-Command' to connect them with our primary offset surface. These steps are shown below:

Extracting the missing surface from the Class A Surface(Grey)

 

Offsetting the extracted surface by 3mm which is shown by pale pink color.

Then we'll repeat these steps for the other missing surface as shown below:

Now, we'll join the two offset surfaces with our primary offset surface using 'Join Command' as shown below:

From the above image, we can notice that when we are using the boundary command on the joined surface, there are no gaps between the primary offset surface and the newly created surfaces and hence missing surfaces are recreated to be used for any further operation.

From the above image, we can see that the missing filleted surface that we have to recreate is having a radius of 3.5mm. To recreate this filleted surface we're going to extract their adjacent surfaces to eventually extrapolate and trim them. Finally, we'll provide an edge fillet between their intersection to create a filleted edge region having a radius of 3.5mm.

EXTRACTED SURFACE:

EXTRAPOLATED:

 

EXTRACTED THE SURFACE AT THE OTHER END OF THE FILLETED REGION USING COMPLEMENTARY MODE WHILE EXTRACTING: 

 

EXTRAPOLATED:

TRIM OPERATION:

 

PROVIDING EDGE FILLET:

THIS PATCH IS NOW FIXED AS SHOWN BELOW:

 

2. SECOND REGION:

First, we'll inspect the radius of the filleted region. For that we'll extract a surface and untrim it as shown below:

Then, we'll untrim it and create a point using 'Point Type' as 'On the Curve' and choose a middle point. Next, we'll try to create a circle using the 'Three Point' type circle and use the measure tool to find out the value of the radius

As the surface was mostly flat, the circle command created an octagon with a radius value of 1.878mm as shown below:

 EXTRACTING THE SURFACES FROM ONE OF THE ADJACENT SIDES OF THE FILLETED REGION:

EXTRACTED:

CREATING BOUNDARY WITH LIMITS ON THE EXTRACTED SURFACE TO USE FOR EXTRAPOLATION:

EXTRAPOLATED:

EXTRACTING THE SURFACE AT THE OTHER SIDE OF THE FILLETED REGION USING COMPLEMENTARY MODE:

EXTRAPOLATING THAT SURFACE:

TRIM OPERATION BETWEEN THE TWO EXTRAPOLATED SURFACES TO CREATE AN INTERSECTING REGION: 

RESULTS AFTER THE TRIM OPERATION:

From the above image, we can see that the required intersecting region between these two surfaces has been created, and now we're going to provide an edge-fillet value to that intersecting edge.

PERFORMING THE EDGE FILLET OPERATION ON THAT INTERSECTING EDGE WITH THE VALUE OF 2MM:

Using the Boundary Command we can verify if there is any remaining section from this region that needs to be fixed.  

It is evident from the above image that there are no additional boundaries but only one that is present at the edge of this region and hence this region can be stated as fixed.

 

3. THIRD REGION:

 

From the above image, we can notice that a certain section of the filleted region is missing and we’re now going to fix it.

We'll begin our procedure by extracting the non-filleted surfaces as shown below:

EXTRACTED SURFACES:

After obtaining the extracted surfaces, we'll untrim all of them.

UNTRIMMED SURFACES:

Now, we'll extrapolate these untrimmed surfaces as much as possible to recreate our desired patch of the region.

SHOWING EXTRAPOLATED SURFACES USING VARIOUS COLORS:

Now, we'll trim these extrapolated surfaces.

TRIM OPERATION:

Now, we'll extract all the surfaces except this region using 'Complimentary-Mode' while using the extract command as shown below:

Now, we'll extrapolate the extracted surface along a limited boundary as shown below:

In the above image, both the extracted surface and extrapolated surface are shown so that we can notice the amount of extrapolation.

Now, we wanted to trim the above surface with our inner box section but if we trim it now it is leaving a boundary along  the lower edge and hence we're going to carry out a few more operations using Extrapolate, Multi-Sections Surface, Join, etc to obtain the surface that is shown below:

 After that, we're going to trim this surface with our initial trimmed surface as shown below:

From the above image, we can observe that 'Trim-Operation' was successful as there are no inner boundaries present after the trim operation is completed.

Now, we'll cutoff the protruding section of the surface that isn't necessary using 'Split Command' using ZX-Plane as shown below:

 

Now, we're going to apply the edge fillets at specified locations as necessary. We're measuring these fillet values from the previously offsetted surface while fixing the second region as shown below:

In the image below, when we'll try to measure the value for this edge fillet using the measure tool, we'll notice that it'll not provide us with a fillet radius but instead, we'll get a length as shown in the 'Measure Item' window and hence we need to work around this issue and find out the actual fillet radius for this edge. 

To find out the actual edge fillet for this edge we'll use the ‘Extract-Command’ to extract this surface. Then, we'll untrim this surface and create a point using the 'Point Definition' command with 'Point Type' as 'On the Curve' and create a middle point. After that, we'll create a circle using the 'Three-point Circle' command and finally measure its radius as shown below:

We'll repeat these steps for the adjacent edge too as shown below:

 Finally, we've all the necessary values to perform the edge-fillet operations on our third region and hence we'll proceed with that as shown below:

From the above image, we can notice that all of our Edge-Fillet Operations were successful as we have fixed this region as well.

 

Finally, our Class B Surface is fully constructed and ready as shown below:

 

 

PROCEDURE TO CREATE THE CLASS C SURFACE:

Now, we're going to create the 'Class C Surface' while using the 'Class A Suface' as the Reference Surface. We'll start that procedure by creating boundary segments all along the Class A Surface using the 'Boundary Command' with limits and then we'll use the 'Sweep Command' to create segments of Class C Surfaces using those boundaries  as shown below:

In the above image, the boundary is made using the boundary command by choosing the vertices of the Class A Surface as limits to create our desired boundary. We have to use limits so that we can create good-quality surfaces using those boundaries. If the boundary is created without considering the complex shape of the Class A Surface then in certain instances longer than usual boundaries will lead to poor-quality surfaces.

After creating the boundary we will use the 'Sweep Command' where we'll use its 'Subtype' as 'With Reference Surface' so that we can use the Class A Surface as our reference surface. We'll select the boundary as our Guide Curve and use the angle of 90 degrees to create our required surface as shown below:

 

Now, generally, we'll continue the above-mentioned steps but in certain instances, we'll come across such complex boundaries using which required surfaces cannot be made conventionally as it'll lead to poor quality surfaces that cannot be used in further operations as it can lead to the generation of gaps or even overlapped regions.

One such conflicting region is shown below where we can see that two surfaces are overlapping with one another and the boundary between them is shaped in such a way that if we used the Sweep Command to create the required surface it'll only result in further poorly constructed surfaces.

Hence to avoid those instances we'll use a workaround using 'Multi-Sections-Surfaces'. Steps that should be taken before using the Multi-Section Surfaces command are shown below:

First, we have to create points on both surfaces using the Point Command and then construct lines with respect to those points and corners as shown below:

Then, we'll use the 'Split Command' to cut both surfaces with respect to the lines as shown below:

After this we'll use the Multi-Section Surfaces command to create the surface between these two surfaces as shown below:

Here, we have used those two lines that we previously constructed for the split operation as limits for the surface and the edge boundary from the Class A Surface as the Guide Curve to create this Multi-Section Surface. 

We'll use the combination of Sweep & Multi-Section Surfaces depending upon the kind of surfaces we'll deal with as we move along the edge of the Class A Surface to create the Class C Surface shown below:

We have to construct two Class C Surfaces. One is the Outer Class C Surface as shown below:

 

Another Class C Surface will be created for the section intended for the Fog-Light as shown below:

Now, we have all the required surfaces: Class A, Class B & Class C

To proceed forward we have to add Class A & Class C together using the 'Join Command'.

First, we'll add the Outer Class C Surface with our Class A Surface as shown below:

 

Then, we'll add the Inner Class C Surface with this as shown below:

Finally, we have to use the Trim Command to trim the Combination of Class A & C surfaces with Class B Surface to obtain the final body that we can eventually use to create a solid body but before doing that we'll create an intersection between the combination of Class A & C with Class B to check whether there are any gaps or overlapped regions that can prevent us from performing that trim operation.

We'll go to Tools from the drop-down menu and go to 'Options' where we'll enable 'Surface Boundaries' that will allow us to check the quality of the intersection as shown below:

At most of the regions, the intersection will be suitable to perform the Trim Operation as shown below:

 

Although at one region we'll notice that there is an issue with the boundary of the Class B Surface as shown below:

From the above image, we can notice that the Class B Surface is not intersecting properly with the Class C Surface at two instances and hence that is going to prevent us from performing the 'Trim Operation'. 

To fix this issue we're going to extrapolate the Class B Surface at those regions so that it intersects properly with the Class C Surface as shown below:

Now, when we'll create another intersection with the 'Extrapolated Class B Surface' then the above issue will be resolved as shown below:

After that, we're going to perform the Trim Operation with the Class B Surface that will create the hollow final body for the bumper with no boundaries.

Using the 'Measure Tool' we'll be able to measure the 'Wall Thickness' after the Trim Operation is done as shown below:

Finally, we'll go to the Part Workbench and use the option 'Closed Surface' from the 'Surface-based Features' toolbar to convert the final trimmed body into a solid body as shown below:

 

After that, we’ll perform Draft Analysis on the Final Part in Part Workbench:

DRAFT ANALYSIS FOR THE FINAL PART USING THE MAIN TOOLING AXIS FROM THE FIRST METHOD:

We'll click on the 'Draft Analysis' under the 'Analysis' Toolbar in the Part Workbench.

Then, we’ll click on the Compass Symbol under 'Direction' which stands for 'Use the Compass to define the new current draft direction'. 

We'll drag the compass and place the compass on the Main Tooling-Axis.

Then, we'll select 'Show or Hide the Color Scale' under 'Display' and define our Draft-Angle as 3-Degrees.

After that, we'll click the surface of the Final Part the results of which are shown below:

In the Draft-Analysis,

Green Colour stands for regions where the Draft-Angle is more than 3 degrees,

Blue Colour stands for regions where the Draft-Angle is between 0-3 degrees , &

Red Colour stands for regions where the Draft-Angle is lower than 0 degrees

It is evident from the above images that the Draft Analysis is successful and the Final Solid Part is feasible to manufacture

 

DRAFT-ANALYSIS FOR THE FINAL PART USING THE MAIN TOOLING AXIS FROM THE SECOND METHOD:

We'll repeat the steps mentioned above from the previous Draft-Analysis.

It is evident from the above images that the Draft Analysis is successful and the Final Solid Part is feasible to manufacture.

 

TREE STRUCTURES:

1. CLASS A SURFACE:

 

2. MAIN TOOLING AXIS USING VERTEX METHOD:

 

3. MAIN TOOLING AXIS USING INERTIA METHOD:

 

4. MAIN OFFSET & FIRST PATCH OF CLASS B SURFACE: 

   

 

5. SECOND PATCH OF CLASS B SURFACE: 

 

6. THIRD PATCH OF CLASS B SURFACE:

  

   

 

7. CLASS C SURFACE ELEMENTS:

   

   

   

   

   

 

8. CLASS C JOIN OPERATIONS:

 

9. PART BODY & DRAFT ANALYSIS: 

 

10. PUBLICATIONS:

 

3D VIEWS OF THE FINAL PART WITH PROPER COLOR CODE OF THE DRAFT ANGLE IN VARIOUS ORIENTATIONS:

1. FRONT VIEW:

 

2. TOP VIEW:

 

3. ISOMETRIC VIEW:

 

THE REQUIRED CATPART IS ATTACHED WITH THIS REPORT IN A ZIP FILE.