Pre-processing for the suspension assembly of a car for NVH in ANSA

Objective:

The objective of this project is to perform FEA preprocessing for the rear suspension assembly of a car, i.e., check for the geometrical errors and mesh with the given element Quality criteria. After meshing the component the thickness has to be assigned for mid surfaces. Use tetra elements to model non-uniform thickness components. And, use connections to connect the components.
All the elements in the model should clear the following quality criteria and the features in the model have to be captured properly with good mesh flow.

For preprocessing tasks, ANSA preprocessor is used.

Introduction:

FEA

Finite element analysis (FEA) is a numerical method for solving physical engineering problems. The basis of FEA is to make calculations at only a limited number of points (nodes) and then interpolate the results for the entire domain (surface or volume). Any continuous object has infinite degrees of freedom and it's just not possible to solve the problem in this format. The finite element method reduces degrees of freedoms from infinite to finite with the help of discretization, i.e., meshing (nodes & elements). Therefore, meshing is nothing but discretization of a continuous system with an infinite degree of freedoms to a finite degree of freedoms.

Types of mesh

There are three types of meshing done for any model,

• 1-D: 1-D meshing is done for components where one dimension is very large in comparison to the other two dimensions. The area of cross-section is given as a parameter to the mesh elements to capture the original geometry properly. This is done with line-shaped elements like rod, bar, beam, etc. Practical applications of 1-D meshing are long shafts, beams, etc.
• 2-D: 2-D meshing is done for components where two dimensions are very large in comparison to the third dimension (thickness). The thickness is given as a parameter to the mesh elements to capture the original geometry properly. 2-D meshing is done with 2-D elements like quads and trias. Practical applications of 2-D meshing are sheet metal components, plastic components, etc.
• 3-D: 3-D meshing is preferred for components where all the three dimensions are comparable to each other. Mesh elements used for 3-D meshing include tetra, penta, hex, and pyramid. Practical applications of 3-D meshing are transmission casing, crankshaft, etc.

Factors deciding the mesh element type

The mesh element type to be used to model a certain component depends on the following three factors.

• Geometry size and shape: For analysis software needs all three dimensions. It can not make calculations unless and until geometry is defined completely (via meshing i.e. nodes and elements). Geometry could be categorized as 1D, 2D, or 3D based on dominant dimensions, and the type of element is selected accordingly.
  By doing 2D meshing over 3D meshing for thin components, we save a considerable amount of computational time in analysis and still get similar accurate results as from 3D mesh. But 2D meshing is not preferred for thick parts or parts with variable thickness as then the results obtained are not accurate.
  
  And in cases of components with varying thickness or thickness more than 5mm, it is recommended to mesh the model using 3D elements such as tetra, hex, penta, etc. Though brick/hex meshing would give more accurate results, it is usually a much harder and time taking process to model each and every component using hex elements. While tetra meshing is comparatively an easy and fast process. And, also tetra mesh gives fairly accurate results to prefer this method over hex meshing. Thus, hex meshing is only done for very critical components like vehicle frame mounting bushings. Thus, it is the job of the CAE engineer to weigh in the benefits and drawbacks of each before deciding the type of mesh to be generated.
  
  
• Based on the type of analysis: The type of analysis should be considered while selecting the mesh type. For eg. for the crash and non-linear analysis, priority is given to mesh flow lines and brick elements over tetrahedron. For structural and fatigue analysis, quad, hex elements are preferred over trias, tetras, and pentas.
  
  
• Time allotted for the project: The type of mesh also depends on the time allotted for the project. For eg., if time is less, 3D meshing tetras are preferred over hexas. When time is no constraint, an appropriate selection of elements, mesh flow lines and good mesh quality is recommended.

Based on the above knowledge, the given suspension assembly needs to be modeled. As per the general practice, components with uniform thickness and less than 5mm will be midmeshed using the 2D elements. Also, we are considering the NVH application for the model, so, quads are preferred. Rotating quads are not at all acceptable and trias should be minimized as much as possible. And, for thick components, 3D tetra meshing will be done.

Procedure:

First, the suspension model is imported into the ANSA workspace. And all the components are arranged into separate PIDs. The given suspension assembly model is shown below,

It is a half model, after modeling it will be mirrored to get the complete model. The assembly model consists of a total of 21 individual components. The overview of the preprocessing process followed as follows,

• Analyze and understand the geometry properly
• Perform geometry cleanup for the component
• Check the thickness of the component and decide the type of mesh
• Take midsurface of thin components and again perform geometry cleanup
• Generate surface mesh according to the quality criteria
• Check the surface mesh for quality and repair the failing elements
• Define volumes and generate tetra mesh
• Check for failing elements and repair if any
• Deploy connections

1D mesh:

In the suspension subassembly model, the 'coiled spring' has a cross-sectional radius of 5mm. So, it can be modeled using 1D elements only, as it has a uniform and very small cross-section compared to its helical length. The coiled spring is modeled with CBAR elements. A CBAR element is a kind of simplified CBEAM element and should be used whenever the cross-section of the structure and its properties are constant and symmetrical.

To model the spring, first, a middle curve is created for the spring by going to Topo>Curves>Middle tool. Next, the created curves are joined to form a single curve using the Topo>Curves>Connect>Multi tool. Then a COG point is created for the curve to define the orientation using the Topo>Points>On COG tool.
Then, switch to the NASTRAN module and go to Elements>CBAR. In the pop-up window, check the 'Orientation with node(s)' option and change the selection type to the curve box. Next, the curve is selected and then the 3D point is selected. Next, element length is given as 4. Then, a New PID is created and under parameters, the area is defined by giving the radius 5mm. And it calculates all other parameters automatically. And, 1D elements are thus created. The created 1D elements can be represented as solid by going to Utilities>Quality criteria>Presentation Parameters>Line elements cross-section and checking the Draw mode-as solids option.

2D mesh:

The condition for 2D midmeshing is that the component must be of uniform thickness and less than 5mm. In the suspension assembly, two components, namely, bracket and lower strut mount were found to have a uniform thickness of 3mm. So, these two components are midmeshed.

First, both components were analyzed and checked for geometrical errors by going to Utilities>Checks>Geometry. No geometrical issues were found. Next, midsurface is extracted. For 'bracket', midsurface is extracted automatically by going to Topo>Faces>Mid surface>Skin tool. Skin tool automatically generates the midsurface and assigns it to a new PID.
And, midsurface for the 'lower strut mount' is extracted by offsetting one face of the component to the middle using the offset tool by going to Topo>Faces>Offset. And then the two faces were joined by extending the cylindrical midsurface to the base circular midsurface. Next, the extracted midsurface is assigned to a new PID by going to Topo>Faces>Set PID>New, and thickness is set to 3mm. The extracted midsurface for both components is shown in the image below,

Now before meshing, mesh parameters and quality parameters are fed into ANSA. Mesh parameters are configured by going to Utilities>Mesh parameters and quality parameters are configured by going to Utilities>Quality criteria. The mesh quality parameters configured are as follows,

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 4 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 none were found. Similarly, CONS which are not essential to define a feature are removed by joining the surfaces using the Macros>Join tool.

The next step is to mesh the midsurface. Meshing is done using the Best tool available under Mesh>Mesh generation>Best. After, generating the mesh, the mesh is reconstructed by going to Mesh>Shell mesh>Reconstruct tool wherever required to improve the mesh and eliminate any off (failing) elements. After reconstructing the mesh smooth tool is used to improve mesh flow and eliminate any off elements.

It is ensured that there are no rotating quads. Also, trias are kept as low as possible. While dealing with trias, the following things should be kept in mind,

• 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

The final mesh generated is shown below,

3D mesh:

Rest all components were 3D tetra meshed because they had non-uniform thickness or/and thickness more than 5mm. The following is the general process to be followed for tetra meshing in ANSA:

• Properly analyze and understand the geometry
• Perform geometry cleanup
• Configure Mesh parameters and quality criteria
• Generate 2D tria mesh for all the surfaces
• Check for minimum and maximum length and repair the falling elements
• Define model as a closed volume
• Generate tetra mesh
• Check for tet collapse, dips, and kinks on the surface and repair the falling elements

The first step is to properly analyze and understand the geometry for each individual component. It is important to understand the geometry and plan for meshing before starting meshing. There might be some geometrical issues like missing surfaces, duplicate/intersecting surfaces, etc. This is usually due to the format conversion process from the CAD format to the ANSA format or due to an inherent bad CAD file. All these issues need to be taken care of before meshing.

Next, the geometry check is performed for each component by going to Checks>Geometry. And, all the issues were automatically fixed by ANSA using the auto fix. Also, at some places, geometry was not proper for some components like distorted surfaces. Such surfaces were deleted and recreated using the Topo>Faces>New tool.

Now, the next step is to prepare the model for meshing. Mesh parameters and quality parameters are fed into ANSA. Mesh parameters are configured by going to Utilities>Mesh parameters and quality parameters are configured by going to Utilities>Quality criteria. The element type is changed to ortho tria and all other parameters are kept default. For 3D tetra mesh only tet collapse criteria is considered. The mesh and quality parameter used for the surface mesh of the components is as follows,

The next step is to prepare the components for surface 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 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 a little 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. There were few fillets where elements would fail for minimum length. All such fillets were first identified by going to Tools>Features>Parameters. In the parameters dialog box, 'fillets' is checked and the minimum element length value is entered in the maximum radius parameter and then click 'Recognize'.

And, ANSA detects all the fillets meeting the criteria and lists as shown in the image below. All such fillets were split into half and macros (surfaces) joined automatically by right-click>Design actions>split.

After the automatic split, some manual intervention might be required to organize the double CONS. The images below show some of the fillets defeatured in this way for 'tire' and 'rim' components. Orange CON (edge) represents the toggled CON and yellow CON is the new split done to divide the fillet into half.

Next, meshing is done for all the surfaces using Mesh generation>Best tool. Then, the created mesh is refined using the Shell Mesh>Reconstruct tool.

Ortho tria elements are used to generate mesh for curved surfaces and normal trias are used to generate mesh for plain surfaces. The reason to do so is that ortho trias give a better mesh flow for curved surfaces but results in a large number of nodes and elements compared to when done using normal trias. That's why to capture the geometry accurately and optimize the mesh quality and the number of nodes, curved surfaces are meshed with ortho trias and flat surfaces are meshed with normal trias.

The images below show the surface meshed models of the suspension subassembly components.

The next step is to define volumes for 3D meshing. To do that switch to the Volume mesh module and go to Volumes>Define>Auto Detect. For this tool to work the model must be already surface meshed which is already done. The tool is run for the whole database. And as expected, it detected 18 closed volumes and defined them automatically under properties with type PSOLID.

The next step is to generate the tetra mesh. For that, there are two tools under the Unstructured Mesh, namely Tetra Rapid, and Tetra FEM. Both can be used to generate the tetra mesh according to the quality criteria. In our case, the Tetra FEM tool is used to generate the tetra mesh. This tool generates the tetra mesh by taking surface mesh as reference and the quality criteria as parameters to be followed.

Finally, the generated tetra mesh is checked for quality criteria and all the failing elements were repaired by going to Improve>Fix quality. Next, the tetra mesh is checked for any dips or kinks on the surface and fixed using the Improve>Align tool.

The generated tetra mesh can be visualized by hiding a few elements, as shown in the image below,

Connections:

Next, connections are deployed for the FE model of the suspension assembly for NVH. To make connections switch to the NASTRAN module in ANSA. The suspension sub-assembly has mainly two types of connections, i.e., bolt and seam weld. In our FE model, RBE2 elements and seam weld elements are used to model these connections. Rbe2 elements are also used to connect components together and constraint the model.

Following are some of the connections deployed for the suspension subassembly.

Seam Weld

The two components shown in the image below are parallel to each other, so they are connected using a seam weld connection.

To create a seam weld, first, a curve is created at the location (highlighted edge in the image below) of the connection using the Topo>Curves>Cons2Curve tool.

Next, the created curve is converted into a connection by going to Assembly>Convert>Curve and the created curve is selected, then seam weld is selected as the connection type. Next, the connection is realized by going to Assembly>Connections Manager, and the seam weld connector is selected. Then in the connection manager, both parts are selected as P1 and P2 respectively.
As both the parts are parallel, therefore, overlap shell is selected as the 'FE rep type'. And other parameters used are shown in the image below,

Next, the connection is realized successfully as shown in the image below,

Bolt

Next, bolt connections are deployed using the rbe2 elements cluster method, i.e., the boundary nodes of the holes are selected as the slave nodes and connected together forming a cluster of rbe2 elements with a master node at the center. The rbe2 cluster is created by going to NASTRAN>elements>rbe2>many nodes and all the nodes at the boundary of the hole are selected and the degree of freedom (CM) is set to 123456, i.e., constrained in all directions. The image below shows the rbe2 clusters deployed for the rim and hub components.

2 node rbe2 constraints

Some components also need to be constrained so as to model the physical scenario during analysis. For eg. The strut and upper strut mount are shown in the image below. If not constrained, the strut would be free to move inside and out of the hole in the upper strut mount during the NVH analysis and therefore the analysis results will be wrong.

Therefore, such components need to be constrained together using the two-node rbe2 elements. The two-node rbe2 is created by going to NASTRAN>elements>rbe2>two nodes and the nodes to be connected are selected and selection is confirmed. This can be done in two ways, i.e., use four rbe2 elements to constraint the components in all directions as shown in the image below. Or pair of loops of nodes can also be connected together with two-node rbe2 elements.

Similarly, all the connections are deployed for the suspension assembly.

Finally, the complete model is reflected using the to obtain the full suspension assembly.

Conclusion:

Preprocessing for the suspension assembly is successfully done. The FEA meshed model is made with good mesh quality and all the features are also captured properly. There are some elements failing in the surface tria mesh generated because of geometrical constraints and couldn't be repaired. The 3D tetra mesh has zero elements failing. Finally, all the necessary connections are deployed successfully to constrained the model.