Preprocesing of BiW Brackets Assy for NVH Analysis using ANSA

Objective:

• For the Automobile's BiW Bracket Assy, Geometric cleanup, Meshing, mesh optimization & Connections parameters to be defined for NASTRAN-NVH simulation solving.
• In this case, connection setups like RBE2, RBE3-HEXA-RBE3, RBE3-CBUSH-RBE3, Overlap-Shells, Bolts, Seam Welds, Seam Line Joints, etc. were used for their respective applications.

Element Quality Criteria:

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

Geometry Preparation:

These CAD models were now to be checked against any geometrical errors such us normal orientation, Needle faces, etc. This can be done with the ANSA's checks manager which helps us to find the surface errors on the CAD geometry. In the checks manager, some options can be checked ON / OFF depending on the parameters required to be checked.

In the checks manager by clicking the Execute button ANSA will check for the surface errors on the visible geometry. Using several surface repairing tools provided by the ANSA these errors should be rectified. some errors can be automatically rectified using the AutoFix option in the checks manager.

The above image shows us the surface errors found on the geometry. There were 11 unchecked surface errors found by the checks manager.

After fixing the surface geometry the status icon on the checks managers shows a Green Trick Marks which resembles that the Geometry is error-free. The above images show that the part geometry is passed according to the checks manager criteria. In the beginning, the surface orientation set automatically may be in an incorrect direction as shown in the above picture.

Mid-Surface Extraction:

After clearing all the geometry errors we can generate the mid surface for the geometry. This is to be done using the Mid Surface option which creates a new surface between the upper & lower sheet surface. This is to be done to make the meshing process easier. Here the CAD geometry is a Sheet metal part that has uniform thickness all over the cross-section. So Auto Mid Surface Extract tool can be used. The thickness of the sheet metal is found to be varying with respect to the sheet metal part.

In Auto Mid-Surface Wizard we need to check for the correct color representative of the respective surfaces as top face to be Green, Bottom face as Red & Side faces to be Blue. This allows the software to generate the Mid-Surface without any issues.

After offsetting the surfaces, some surfaces will retain some unwanted holes since its a casting part, the triple cons surfaces are not captured. So these holes must be filled with the 'Fill Hole' option.

Setting up Quality Criteria:

In quality, criteria wizard the given parameters are entered so that the ANSA could check the mesh generated is under these criteria.

After the Mid Surface Extraction is processed the total assembly with its sub-assembly parts is defined with the respective property which helps for easy selection of parts to define its connection between them. The property Dialog box with the sub-assembly parts for this case is shown below.

Mesh Preparation:

Before the meshing process some of the features to be checked manually in order to generate mesh under defined quality criteria.

The length between two nodes is maintained between 3 to 7mm if not it will fail as per quality criteria since the range must be controlled. In this case, we can join the two any two surfaces which increases the length between two nodes without defeaturing the geometry.

Removal of Unnecessary perimeters:

Some of the unnecessary perimeter lines & hot points can be removed which makes the meshing to be done under defined quality criteria. Here in this model, the average length of an element is set to 5mm with tolerance the range can be within 3-7mm. So the parametric lines lesser or greater than the provided tolerance then those lines must be removed or altered without defeaturing the geometry.

Meshing Process:

Before meshing the length of a single element is provided as 5mm so that all the nodes are rearranged with an average distance of 5mm.

After meshing some elements in this component fails upon the defined quality criteria. This can be solved with the Mesh Repair Tools available in ANSA to eliminate all the errors. Make sure that the percentage of triangle element is very low in order to get accurate FEA calculation.

The above picture the model with zero error thus passing the quality criteria. For this model Total elements are 23866 consisting of 23382 quad elements & 484 triangle elements contributing only 2% of the total elements strength.

Defining Connections:

Bolt Connection:

In the above picture, The bolts are to be mounted/riveted to the brackets constraining its six degrees of freedom. So on ANSA, a 3D point is created at the center of the bolt hole. The point generated is further converted to Bolt entity where the connection parameters can be defined under the connection manager.

The above picture represents the connection manager interface where connection parameters were defined. Under Rep Type section 'Bolt' is selected. Then Part 1 & Part 2 components are selected which helps the software to understand where the bolt specification to be applied.

RBE2 Connection:

From the above picture, we can see that a bolt is mounted on the bracket connecting the whole bracket assembly with the main body. So for this NVH simulation setup, those points are considered as Rigid Body Element (RBE). On the below picture, the values for CM are inputted as 123456. Here the numbers from one to six represent the six respective degrees of freedom. 1, 2, 3 represents the degree of freedom along X, Y, Z Axises respectively in Translatory motion. 4, 5, 6 represents the degree of freedom along X, Y, Z Axises respectively in Rotational motion. For this Many Nodes RBE2 feature is used.

SpotWeld Connection:

In this assembly, For two brackets with small surface contact areas that were welded together by spot welding for structural properties. So on ANSA, 3D points are created on both brackets where the spot weld needs to be applied. The points generated are further converted to spot weld point entity where the connection parameters can be defined under the connection manager as shown above. In the connection manager, for Spot Welding Connection the FE Rep Type is set to RBE3-HEXA-RBE3 with RBE3 Pinflags as 123456 constraining all degrees of freedom.

OverLap Weld Connection:

In this assembly, For two brackets with large surface contact areas that were welded together by Seam welding for structural properties. So on ANSA, A Feature Curve is created between those brackets where the seam weld needs to be applied. The curve generated is further converted to a seam line weld entity where the connection parameters can be defined under the connection manager as shown above. In the connection manager, for Seam Welding Connection the FE Rep Type is set to OVERLAP-SHELL with base sheet selected with the bracket which has a higher thickness value.

Y-Joint Weld Connection:

In this assembly, two brackets with large surface contact areas that were not overlapping with each other can be welded together by Y Joint Seam welding for structural properties. So on ANSA, A Feature Curve is created between those brackets where the seam weld needs to be applied. The curve generated is further converted to a seam line weld entity where the connection parameters can be defined under the connection manager as shown above. In the connection manager, for Seam Welding Connection the FE Rep Type is set to Y-Joint-SHELL with base sheet selected with the bracket which has a higher thickness value.

The above picture shows the FEA Model with connection parameters completed successfully for all the parts.