2D Meshing of Hood in ANSA

Objective:

The objective of this project is to perform preprocessing i.e. geometry cleanup, midsurface extraction, and 2D shell meshing for the hood component of a car. After meshing, component thickness and material need to be assigned to the mesh. And the mesh should follow the following quality criteria,

S.no.	Quality criteria	Value
1	Target/Average length	5
2	Minimum Length	2
3	Maximum Length	7
4	Aspect	3
5	Warpage	15
6	Skewness	45
7	Jacobian	0.7
8	Minimum Quad Angle	45
9	Maximum Quad Angle	135
10	Minimum Tria Angle	30
11	Maximum Tria Angle	120
12	Tria Percentage	15

In this project, we will see the process of creating a 2D mesh for thin-walled components with complex features. For this purpose, ANSA software will be used.

Introduction:

The Hood of a car is a sheet metal component with a very small thickness compared to the other two dimensions. And, for such thin components, 2D shell meshing is preferred over 3D meshing. By doing so, we save a considerable amount of computational time in analysis and still get similar accurate results as from 3D mesh. This is achieved by extracting the midsurface of the component and assigning thickness to it so as to capture the original geometry. And, then the mesh is generated for the midsurfaces extracted.
Also, here we are considering that the mesh model would be used for crash analysis. Therefore, absolutely no rotating quads are allowed. And trias also needs to be avoided as much as possible.

Now, let's see the process to generate the 2D mesh.

Procedure:

First, the hood model is imported into the ANSA. The hood model contains five individual components as shown below.

The first step after importing the model is to properly analyze and understand the geometry. When a CAD model is imported into the ANSA, there might be several geometrical errors like missing/distorted surfaces, intersecting surfaces, etc. due to the format conversion process or inherent bad model. And, it is important to clear all these errors before starting meshing. So, the next step is to clean up the geometry. To ensure that all the surfaces are connected properly Faces>Topo tool is used for all the edges of each individual component at a time. Next, geometry check is performed by going to Checks>Geometry and running it for parameters as shown in the image below. Another image shows the errors detected.

Most of the errors were fixed automatically by right-clicking on the error>fix. Next, the orientation of all the faces is modified by going to Faces>Orient. This ensures that all faces are oriented similarly.

The next, step is to extract the midsurfaces for each component and keep them in separate property id. Midsurfaces are extracted using the manual method i.e. offsetting the surfaces of either face to the middle. First, the thickness of each component is measured using the Measure tool from Utilities>Measure. The outer panel and inner panel were found to be 0.75mm thick and the latch and hinges were found to be 1.2mm. As they are sheet metal components, the thickness is uniform across the component. Then, four properties are created by going to List>Properties>New. Thickness is assigned to each property and a Material 'Steel' is also created and assigned to each property. The image below shows the created properties with Ids 1,2,3,&4.

Next, midsurface is extracted using the Offset tool by going to Faces>Offset and selecting all the surfaces on one face. Then, half of the thickness is given as the offset value, the direction is checked and offset. Now, the property is assigned to the extracted midsurface by going to Faces>Set PID and assigning to the respective property. Similarly, all midsurfaces are extracted and property assigned for all the components.

As the Outer panel and Inner panel (except one surface) are symmetrical, only half midsurface is extracted. Similarly, both hinges are mirror images of each other, so midsurface is extracted for only one hinge.
Again, the extracted midsurfaces are checked for geometric errors and fixed. There were some geometrical issues as shown below, where surfaces are intersecting with each other. To remove this issue, all surfaces in that vicinity are deleted and a new surface is created by going to Faces>New>Fitted or COONS. The second image shows the repaired surface.

The final extracted midsurfaces are shown below.

Next, mesh parameters are configured by going to Utilities>Mesh Parameters. There, target length, minimum element length, and maximum element length are configured to 5, 2, & 7, respectively. All other parameters are kept as default for mixed and 1st order elements.

Next, quality criteria are configured by going to Utilities>Quality Criteria. And, the quality criteria file is saved for future reference. The created quality criteria parameters are shown in the image below.

The next step is to prepare the midsurfaces for meshing. For that, switch to the Mesh module. First, the shell element length is altered by going to Perimeters>Length and all the CONS are selected and target element length 5 is fed as length value. The same is done for all the Macros (surfaces).

Next, all the areas are checked for minimum element length and altered where elements might fail for minimum length. Similarly, CONS which are not essential to define a feature are removed by joining the surfaces using the Macros>Join tool. Also, the complete midsurface model is divided strategically into sections using Macros>Cut and Macros>Project Cut tool. This will help to generate a better quality mesh. Also, all the holes are rotated using the Perimeters>Slide tool to ensure the CONS are parallel to the nearby CON. This will help in generating a mesh with good flow. The result of the above steps is shown in the image below. The same process is repeated for all the midsurface components.

Orange CON (edge) represents the joined macros (surfaces) and yellow CON is the new split done to divide the geometry into sections. Also, elements would fail for minimum length in the hemming region. So, for the hemming region, it is split into half along its length and the CON above and below are removed by joining the macros (surfaces) as shown below.

Next, meshing is done using the Mesh generation>Best tool. This tool generates the mesh using the best algorithm applicable. Then, the created mesh is refined using the Shell Mesh>Reconstruct tool. It is ensured that there are no rotating quads. Also, trias are kept as low as possible. While dealing with trias, the following things need to be ensured.

• No back to back trias touching each other
• No opposite trias
• No trias touching the edges
• No trias on a feature
• Low concentration of trias in a region

To deal with trias, the following tools are used,

• Grid>Paste, to paste the nodes and move tria backward
• Elements>Split, to split an element and move tria forward
• Elements>Swap, to move the tria left or right
• Elements>Join, to join two trias to make a quad

After modifying the mesh, Shell Mesh>Smooth tool is used to smoothen the flow of the mesh. Any elements failing for quality criteria are also fixed by either remeshing or smoothing the elements. The created mesh is shown below,

Finally, after creating the mesh and clearing for quality criteria, the mesh is mirrored for the outer panel, inner panel and the hinges by going to Utilities>Transform>Copy. All the entities to be mirrored are selected and then mirrored using the mirror 3 points plane option. Then, the mesh is checked for equivalence by changing to the Topo module. The model is checked for any free CONS and pasted using the Topo tool if any. Again, the mesh is checked for quality criteria. Finally, the shell element representation is changed by going to Utilities>Quality Criteria>Presentation parameters and enabling the 'Draw shell as solid'.

Conclusion:

Geometry cleanup, midsurface extraction, and 2D meshing of the given hood model were successfully done. And all the elements pass the quality criteria. All the features in the model are captured properly with good mesh flow. Tria concentration is kept low at just 0.85%.