A grommet is a component employed in automobiles. It is used at the connection of the door of the automobile to the BiW. The BiW is the part of the vehicle after all the sheet metal parts have been welded together on the vehicle. BiW is termed before painting and before moving parts (doors, hood, deck lids and fenders), the engine and chassis sub-assemblies, or trim (glass, seats, upholstery, electronics etc.) have been assembled into the frame structure.
Figure 1 – Generic Grommet at the door (For representational purposes only)
Figure 2 – Body in White of the vehicle (For representational purposes only)
The Grommet serves the function of protecting the electrical wiring that passes from the door of the vehicle to the BiW from possible mechanical or chemical attacks, dust, rain and temperature changes. It acts as housing for the electrical wires that pass through it. The material selected for the grommet for this thesis, is called EPDM-30. It is a Hyperelastic material, meaning that it requires a particular material model for the Strain Energy density function. The material model that is used for this grommet is the Marlow Model.
The aim of this project is to digitize the process of the grommet’s design i.e. – perform numerical simulations on the grommet and improve its design. Currently, the Grommet design process involves a conventional approach with various hardware tests. Grommet digitization accelerates the design process and reduces the time required during the design stages. This provides a high potential for reducing prototypes, hardware tests and development time.
To understand the behaviour of the Hyperelastic material during the kinematics of door closure.
To identify the points of maximum stress on the Hyperelastic material during the opening and closing of the door.
The prescribed methodology for the project is given via the following chart –
Figure 3 – The methodology of the project
The initial step is to obtain the CAD data of the grommet, and to subsequently mesh it. For the mesh, we use a method called Hexamodelling, wherein the mesh used is called hex-mesh. This method is used as it gives a smooth mesh flow between the solid elements and the shell elements, and also provides accurate results when it is integrated. Also, with hex mesh, the computing time is faster and it is recommended when the geometry is complicated.
Hypermesh software is used to mesh the component. The mesh consisted of a particular set of steps which were followed in order to complete it.
The first portion that was meshed was the convolute portion. A 2D mesh of one section of the convolute was done, and the rest of the sections were filled through translation of the meshed section. The 3D mesh was obtained by revolving the 2D meshed section around the axis of the convolute.
Figure 4 – 2D mesh of the convolute area
Figure 5 – Revolving the convolute mesh about the axis gives the 3D structure
The next step was to project the bottom faces of the convolute section onto a reference plane. The reference plane would then be meshed using shell mesh option. The reference plane is important for the geometry because the elements on this plane would be projected onto different sections of the lower portion of the grommet, in order to accurately capture the geometry. This is faster rather than creating elements on the bottom planes, which is cumbersome and time consuming.
Figure 6 – Mesh of the reference plane area
After the reference plane has been meshed correctly, the same elements are projected onto different planes in order to successfully capture the geometry of the lower portion of the grommet.
Figure 7 – Projection of the reference plane mesh onto different planes to accurately capture the geometry
After all the surfaces have been projected onto the right planes, an option called SolidMap is used. This option creates solid elements between two plane surfaces. And since the elements are the same on both the plane surfaces, there will be straight rows of solid elements that are attached between these two surfaces. The procedure is repeated for the entire bottom portion of the grommet.
Figure 8 – Solid Map option creates solid elements between the different planes
After the bottom surfaces have been meshed, the sides at the bottom need to be meshed. For this, a 2D mesh is constructed at the bottom surfaces, and using the solid map option, the 2D mesh is extended into a 3D mesh along a node path. In this case, the node path is the edge of the meshed portion. In this way, the entire bottom portion geometry has been captured and meshed completely.
Figure 9 – Solid Map of the side portions of the grommet component.
The next focus is at the top portion of the Grommet. The section above the convolute portion is tricky to mesh, since there is variable thickness at different points in the section. So the mesh is directed upwards, taking small portions of 2D sections, and revolves the shell mesh to get the solid mesh. At one portion however, there is a little logic involved. Since the section is extruded outward, and also has variable internal thickness, it is split into three subsections. The three sub sections are meshed using 2D shell mesh initially, and then rotated to fit into the geometry of the Grommet appropriately.
The topmost section of the grommet which attached to the door is modelled in a similar fashion. Shell mesh is done for the surfaces, following which the meshed surfaces are projected onto different planes and slid map function creates 3D elements which can complete the meshing aspect of the Grommet.
The completed mesh of the grommet component is shown in the following figure-
Figure 10 – Completely meshed grommet
Figure 11 – Completely meshed grommet
The Grommet has a few parameters which are important, and can affect its behaviour during the door kinematics. The parameters are described in the following picture.
Figure 12 – Various parameters of the grommet
1. Pitch – The distance between a point on the crest or trough to the same point on the adjacent crest or trough of the grommet convolutes.
2. Length – The total perpendicular distance from the base covering the entire convolute profile.
3. Height – The perpendicular distance between a crest and a trough.
The original dimensions of the above parameters are depicted in the following table –
Serial Number ParamaterDimensions (in mm)
1. Length 83.178
2. Height 4.985
3. Pitch 6
4. Thickness 1.4
5. Number of Convolutes 14
Table 1 – Dimensions of the grommet parameters
Another aspect that needs to be considered during the meshing stage is the element quality check. This is important because, the solution of the problem depends on the quality of the mesh. Therefore, element quality checks are very important and are a mandatory process during the meshing of the component. Moreover, if a few elements fail during the meshing stages, element quality checks provide a means of identifying the failed elements and rectifying these failed elements.
There are a few parameters that are considered, which make up the various element quality checks. They are as follows-
Skewness – It is calculated in tria elements by finding the minimum angle between the vector from each node to the opposing mid-side and the vector between the adjacent mid-sides at each node of the element. 90 degrees minus the minimum angle found is reported.
Figure 13 – Skew parameter in element quality check
Skew in quad elements is calculated by finding the minimum angle between the two lines joining opposite mid-sides of the element. 90 degrees minus the minimum angle is reported. For 3D elements, the skew check is performed on all faces.
Aspect Ratio- it is calculated in 2D elements by dividing the maximum length side of the element with the minimum length side. For 3D element, it is performed on all the faces.
Warpage- it is calculated in 2D elements by splitting a quad into two trias and finding the angle between the two planes which the trias form. The quad is then split again, this time using the opposite corners and forming the second set of trias. The angel between the planes which the trias form is found. The maximum angle found between the planes is the warpage of the element. Warpage in 3D elements is performed on all the faces individually.
Jacobian- it is a ratio of a measure of the deviation of a given element from an ideally shaped element. The Jacobian value ranges from -1.0 to 1.0, where 1.0 represents a perfectly shaped element. The ideal shape of an element depends on the element type. The check is performed by mapping an ideally shaped in parametric coordinates onto the actual element defined in global coordinates. For example, the coordinates of the corners of an ideally shaped quad element in parametric coordinates is (-1,-1), (1,-1), (1, 1) and (-1, 1). The determinant of the Jacobian related the stretching of the parametric space required to fit into the global coordinate space. As the element becomes more distorted, Jacobian value approaches zero.
The following figure depicts acceptable quality standards for elements during meshing.
Figure 14 – Acceptable quality standards to be considered during meshing
The following table consists of criteria are used in evaluating the quality of the mesh. The above mentioned criteria are considered to be of higher importance compared to the rest.
Figure 15 – Ideal and worst values of various element quality check parameters
The next step is to complete assembly of the components. Initially, the completely meshed portion of the grommet is checked with the geometry to verify if the mesh has captured the entire geometry properly.
Figure 16 – The grommet mesh has captured the grommet geometry accurately
The CAD data of the BiW and Door is taken, i.e. – the geometry. The midsurfaces are extracted from the portion of the door and BiW, since we require only a part of the door and BiW for our reference, and this will reduce the computing time. Also, the BiW and the door are meshed for representing the said components. This is achieved by taking the midsurfaces and 2D meshing of the midsurfaces. For the BiW, it is essential to verify if the mesh is inside the geometry and captured it correctly.
Figure 17 – Mesh of BiW has captured the geometry accurately
Initially, the Grommet is attached to the door clamping point, and kept straight, i.e. – in its undeformed position. The BiW is changed from its vertical position to its horizontal position. This is done because if it is kept in its original position (vertical), then it would be difficult to attach the grommet and also obtain the bends that are present in real time. It would not allow the grommet to show the bends at the convolute portion. This would mean that the boundary conditions and in turn, the simulation would be inaccurate. The assembly of the grommet with the door and the BiW is shown in the figure below.
Figure 18 – The assembly of the grommet with the door and BiW, door (blue) and BiW (yellow)
After the BiW has been kept in the horizontal position, we attach the undeformed grommet to the horizontal BiW. We then calculate the x, y and z distances from the horizontal BiW to the vertical BiW. By knowing these distances, the BiW can be moved from the horizontal position to its original vertical position and the bends on the grommet can be visualised and the simulation can be carried out correctly. The following table specifies the distances between the original position of the BiW and the horizontal position of the BiW by taking three nodes common to both positions as a reference point. These three nodes are the reference nodes at the BiW area. Their displacements are given as follows –
Node Numbers Displacement values(in mm)
111618 – X 19.987
111618 – Y 79.920
111618 – Z -15.064
111619 – X 19.106
111619 – Y 27.568
111619 – Z -63.435
111620 – X 19.631
111620 – Y 54.386
111620 – Z -29.240
Table 2 – Displacement values for the BiW to move it for attaching the grommet
The following figure shows the movement of the components in the steps defined.
Figure 19 – The movement of the components during the simulation
Then we perform the Dynamic Explicit Simulation. There is a difference between the Implicit and Explicit methods. An Explicit FEM analysis does the incremental procedure and at the end of each increment updates the stiffness matrix based on geometry changes (if applicable) and material changes (if applicable). Then a new stiffness matrix is constructed and the next increment of load (or displacement) is applied to the system. In this type of analysis the hope is that if the increments are small enough the results will be accurate. One problem with this method is that you do need many small increments for good accuracy and it is time consuming. If the numbers of increments are not sufficient the solution tends to drift from the correct solution. Perhaps most importantly, this method does not enforce equilibrium of the internal structure forces with the externally applied loads. An Implicit FEM analysis is the same as Explicit with the addition that after each increment the analysis does Newton-Raphson iterations to enforce equilibrium of the internal structure forces with the externally applied loads. The equilibrium is usually enforced to some user specified tolerance. So this is the primary difference between the two types of analysis, implicit uses Newton-Raphson iterations to enforce equilibrium. This type of analysis tends to be more accurate and can take somewhat bigger increment steps. One drawback of the method is that during the Newton-Raphson iterations one must update and reconstruct the stiffness matrix for each iteration. This can be computationally costly. (As a result there are other techniques that try to avoid this cost by using Modified Newton-Raphson methods). If done correctly the Newton-Raphson iterations will have a quadratic rate of convergence which is very desirable. Hence Dynamic Explicit method of simulation is used.
The Hypermesh file is export into ABAQUS format as an input (.inp) file. The input file consists of model and history data. The model data consists of the information used to define the component being analyzed. The history data consists of information to define what happens to the component- the sequence of loading or events for which the response of the component is attained. The history data is divided into a number of steps, each defining a separate part of the simulation. By having knowledge of this input file, it is easier to make changes to the constraints in the input file which saves time.
The following picture shows the actual input file for the grommet and the important terms are defined as shown.
Figure 20 – ABAQUS input file with nodal definition
Figure 21 – ABAQUS input file with element definition
The input file has the following terminology associated with it –
*HEADING – This line specifies the heading of the file, or the name in which it has been saved.
*NODE – This refers to the node definition. It comprises of the node number, followed by the X, Y and Z coordinates which identify where that node is placed in the system.
*ELEMENT – This is used to define the elements that belong to a part or a component. The type specifies the type of elements used for the component. In this case, C3D8R elements refer to an 8 node brick element with reduced integration points. The element set that these elements have been assigned to is written after the element type.
The following picture has the following terminology associated with it-
Figure 22 – ABAQUS input file with biaxial test data definition
The first line describes a comment on the material used for the grommet, EPDM 30. The next few lines speak about the material properties.
*MATERIAL – This command is used to indicate the start of a material definition. The name of the material is written next.
*DENSITY – This command specifies the density of the specified material.
*DAMPING – This command is used to provide material damping for mode based analyses and direct integration analyses. The alpha command is used as a damping control parameter. The beta command is used as an implicit operator for the time integrator.
*HYPERELASTIC – This option is used to define material constants for a general hyperelastic material. Marlow refers to the type of material model being considered. Poisson refers to the Poisson’s ratio, which accounts for compressibility. This option is only used when there are no lateral strains specified in the uniaxial, biaxial or planar test data.
*BIAXIAL TEST DATA – Refers to the biaxial test data for that particular material. It can be used for the Marlow model. The data is from a biaxial test that has been conducted experimentally and the values are that of nominal stress and the nominal strain.
The following figure shows the Step data along with its associated terminology.
Figure 23 – ABAQUS input file with first step definition to move the BiW and simultaneously open the door
*STEP – This is used to begin a step definition, which has a sequence of commands which are executed as per order. It is defined along with its name.
*DYNAMIC – This option is used to define a dynamic stress/displacement analysis using explicit integration in ABAQUS Explicit. The order of definition for dynamic explicit analysis in the command line is- minimum time period, maximum time period, minimum time increment, maximum time increment.
*BOUNDARY – This option is used to prescribe boundary conditions at nodes or to specify the driven nodes in a submodelling analysis. The OP=NEW parameter removes any boundary conditions that are currently in effect. The AMPLITUDE parameter is used only when some of the variables have prescribed non zero magnitudes. This parameter associates the variables to an amplitude curve which prescribes the non-zero magnitudes.
In the step 2 definition, the boundary command is responsible for movement of the BiW from the horizontal position to its vertical position, and also for the subsequent opening of the door.
*CONTACT – This command is used to indicate the start of a general contact definition.
*CONTACT INCLUSIONS – This command is used to specify self-contact surfaces and surface pairings that should be considered by the general contact algorithm. The ALL EXTERIOR parameter is used to specify self-contact for a default unnamed, all-inclusive surface that includes all analytical rigid surfaces.
*CONTACT EXCLUSIONS – This option is used to exclude self-contact surfaces and surface pairings from consideration by the general contact algorithm. Since the first surface name is omitted, the default all-inclusive element based surface defined is assumed.
*SURFACE PROPERTY ASSIGNMENT – This option is used to modify the surface properties for surfaces that are involved in general contact interactions. It is used in conjunction with *CONTACT option. The PROPERTY parameter is used to specify the type of property being assigned. The option of FEATURE EDGE CRITERIA is used to control which primary feature edges are and secondary feature edges should be activated in the general contact domain.
*CONTACT CONTROLS ASSIGNMENT – This option is used to modify contact controls for specific contact interactions within the domain considered by the general contact algorithm. It is used in conjunction with the *CONTACT option. The AUTOMATIC OVERCLOSURE RESOLUTION parameter is used to store offsets instead of adjusting nodes during the initial overclosure resolution between surface pairs in the general contact domain. STORE OFFSETS is the overclosure resolution method.
*VARIABLE MASS SCALING – This option is used to specify the mass scaling during the step for part of or the entire model. The DT option is used to set the desired stable time increment for the element set provided. If this parameter is ignored, then all variable mass scaling definitions from the previous steps are removed, and the scaled mass matrix from the end of the previous step is carried over to the next step. The TYPE=BELOW MIN option is used to scale the mass of elements whose element stable time increments are below the value assigned to DT. The masses of these elements will be scaled so that the stable time increments equal the value assigned to DT. The FREQUENCY option is used to provide the increment steps for which the mass scaling calculations are to be performed. For example, FREQUENCY = 10 will scale the mass at the beginning of the step and at increments 10, 20, 30 etc.
*OUTPUT – This option is used to write contact, nodal, energy, element or diagnostic output to the output database. In ABAQUS/Explicit it is used to write incrementation output to the output database. The FIELD parameter is used to indicate that the output requests used in conjunction with the *OUTPUT option will be written to the output database as field-type output.
*NODE OUTPUT – This option is used to write nodal variables to the output database.
*ELEMENT OUTPUT –This option is used to write the element variables to the output database.
The following figure depicts the various parameters used in causing the door to close –
Figure 24 – ABAQUS input file with second step definition to close the door
The parameter that is responsible for the closing of the door is the *BOUNDARY parameter. The opening and closing angle of the door is found to be 70°. This is given as input in the parameter definition as 4 i.e. – rotation about X axis. The value 1.3439 is given in radians, which amounts to 70 degrees.
Another important point to note was that, for EPDM 30 material, the uniaxial test data was also available. It was written in the ABAQUS input file as depicted by the following figure.
Figure 25 – Uniaxial test data for EPDM 30 material
Thus, from both the set of data, a comparison can be made by implementing both data into the analysis and verify if the biaxial data gives better results.
Also, from the uniaxial and biaxial data, it is possible to construct the stress-strain graphs since the data is given in terms of nominal stresses and nominal strains. The graphs of the uniaxial and biaxial data are shown in the following figures.
Figure 26 – Stress-strain graph for uniaxial and biaxial data
From the graph, it is evidently seen that the biaxial test data has a wider range and captures the non-linear behaviour of the component more accurately as compared to the uniaxial test data. The reason is, that for the biaxial test, the component is stretched from two mutually perpendicular axes, whereas with the uniaxial test, the component undergoes tension from only one axes. Hence biaxial is preferred as it captures the material behaviour more accurately, and is therefore used for the grommet material.
HyperView is used to visualize the results of the simulation. We observe the two steps of the simulation- the first one being movement of the BiW into its original position (vertical) from the horizontal position, and subsequent opening of the door. The second step is the closing of the door. The following pictures depict the movement of the various components.
Figure 27 – Analysis Step 1 – Movement of BiW to its original position
Figure 28 – Analysis step 1 – Subsequent opening of the vehicle door during BiW movement
Figure 29 – Analysis Step 2 – Closing of the door
The Following figures show the behaviour of the grommet during the two steps, and also show the areas of stress on the grommet.
Figure 30 – Behaviour of grommet during the first step
Figure 31 – Behaviour of the grommet during the second step
The following figures show the areas of stress and the variation of stress distribution between using the biaxial data and the uniaxial test data during both steps of the analysis.
Figure 32 – Comparison between Biaxial (left) and Uniaxial (right) data used as input during the first step of the analysis
Figure 33- Comparison between Biaxial (left) and Uniaxial (right) data used as input during the second step of the analysis
From the figures above, it is seen that the simulations conducted with the biaxial data turn out to be more accurate due to the capture of the non-linear material characteristics, and show a better stress distribution compared to the uniaxial test data.
From the results, the behaviour of the grommet can be seen very clearly. The movement of the grommet and the bends at the convolute portions is clearly captured during the analysis. Also, we can clearly see the areas of maximum stress on the grommet.
By understanding the behaviour of the grommet, it is easy for the designer to make the necessary design changes by altering the various parameters and performing the analysis again. This can be done in order to optimize the design of the grommet by reducing the maximum stress on the grommet. This provides an opportunity for further research and reduces the need for prototypes, hardware tests and development time for the designer.