Project - 2 - Meshing on the suspension Assembly

OBJECTIVE :

To mesh the given rear suspension model in both 2D and 3D (according to the given quality criteria) after checking for and clearing geometrical errors. Also, to deploy appropriate connections as required between various parts of the assembly after which the model is symmetrically replicated using the reflect tool.

QUALITY CRITERIA :

FOR PARTS THAT REQUIRE TETRA MESH:

TYRE & RIM (Trias)

S.No	Quality Criteria	Value
1	Target/Average length	6.5
2	Minimum Length	5
3	Maximum Length	10
4	Skewness	45

OTHER REGIONS (Trias)

S.No	Quality Criteria	Value
1	Target/Average length	4
2	Minimum Length	2
3	Maximum Length	6
4	Skewness	45

TETRA ELEMENT QUALITY REQUIREMENTS

S.No	Quality Criteria	Value
1	Tet-collapse	0.2

FOR PARTS THAT REQUIRE 2D MIDSURFACED MESHING:

S.No	Quality Criteria	Value
1	Target/Average length	4
2	Minimum Length	2
3	Maximum Length	6
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

MODEL IMAGE

DOWNLOAD LINK

https://drive.google.com/file/d/1bFWJ5DDP-iQyvVnfzMxtyrLzX3080j9A/view?usp=sharing

PROCEDURES:

In TOPO

Geometry check:

TOPO :

• After downloading the drawing, release cons and apply TOPO.
• Proceed with Geometry check.
• If cons are generated select all then clear it fix by Right clicking. If not fix manually.
• In this case after selecting all, go for right click and fix. All errors are cleaned (If not go for individual checks and clean).

After Geometry Checks for parts other than Tyre and Rim

After Geometry Checks for Tyre and Rim

• We can go ahead and measure thicknesses of various regions in the component using the Measure tool from the top toolbar.
• This is done to decide the type of meshing we ought to carry out.
• parts with uniform thicknesses (throughout) lesser than 5mm will be 2D meshed after generating their midsurfaces and the others will undergo volumetric meshing.

Setting PID's :

Along with taking thickness measurements, it would be easier to assign PIDs to various parts of the model as well. In order to set up some connections, it is important to differentiate components with the help of PIDs.

• While assign PIDs, we can midsurface the parts that will require 2D meshing and then assign PIDs to these midsurfaces as well.
• For midsurfacing, I used the offset tool (Faces > Offset). When activated, it will ask us to select the surfaces to offset.
• We can select the surfaces on one side of the part. After that, we can assign the offset value (half the thickness).

• After this, the surfaces need to be prepared for meshing.
• This means regions that can result in minimum length failures need to be tended to.
• In such locations, cons can be suppressed at the expense of features as long as it's minimal. This is done by right-clicking the cons using the Faces > Cut tool.

The following are parameters and quality criteria for the midsurface 2D meshes:

The following are parameters and quality criteria for parts (excluding tyre and rim) that are to undergo volumetric meshing(Tria mesh):

Parameters and criteria for tria 2D meshes on the tyre and rim:

• We can then start meshing each of the parts as per the mesh requirements (2D Mixed mesh using Mesh Generation > Best from the Mesh module and 2D tria mesh using Mesh Generation > Spot).
• We can make use of the reconstruct tool (Shell Mesh > Reconstruct) to generate a better mesh if the initial mesh is not satisfactory.
• Some regions will end up having off elements anyway due to feature constraints which can be fixed manually.

• After meshing all regions, we can proceed to the next step of assigning volumes manually to each set of closed-shell elements (for volumetric meshing).
• This is done by using Volumes > Define > Manual and then selecting the regions that comprise a particular volume.
• Auto automatically detects and defines closed volumes that are selected
• The manual option lets us define properties for the volume that is to be defined.

• After the volume is defined, the list of defined volumes can be accessed from Volumes > List.
• The volumes that are unmeshed can be 3D meshed by rt. clicking the particular volume and selecting 'remesh' as shown:

• We then have the option of using either one of the Tetra rapid or Tetra FEM algorithms.
• Doing so generates the solid mesh elements within each volume.
• This process is repeated individually for every available volume in the model.

An example of 3D generated tetra elements

9. Next, we need to check the solid elements to see if any fail for the tet collapse criteria of 0.2. Before doing that, we will need to access the solids tab as well on the quality criteria window to input the tet collapse criteria.

• Now we need to switch to hidden mode to check for tet collapse errors.
• There are two ways to fix tet collapse failures.
• One is by using the Fix Quality tool from the volume mesh module (Improve > Fix Quality).

MESHING THE SPRING COMPONENT

1. For this, we shall be using 1D CBAR elements to represent the part. Firstly, we can generate a middle curve (Curves > Middle) of the topo deck.
2. We then have to convert the curves into a single one, using the Curves > Connect > Multi tool.
3. After that, we can define a COG point for the curve generated from the spring (Points > On C.O.G.).
4. Go to NASTRAN deck and go to Elements > CBAR and in the window that pops up, 'orientation with nodes' needs to be checked and the selection needs to be 'Curve (box)'.
5. The curve is then selected and we can click the middle mouse button.
6. Pick the orientation point and we can select the COG for that.
7. Specify the element length as well. We can go for 4mm.
8. After that, on clicking the middle mouse button, we are to assign a property to this curve. We can go ahead and create a new PID. In the next window, we are to input the area (A). In that selection box, we can press Shift + ? to open another window.
9. Specify the cross-sectional radius of the spring. On doing so, the algorithm automatically calcualtes and populates the other values on the PID card as per the given radius.
10. Next we need to define the CBAR element by simply naming it.
11. On proceeding, we will notice that the 1D elements have been created.
12. These can be represented as 3D solids as well. To do that, we simply need to check the 'Lines Element Cross Section' box and select 'as solids'. These options are available in the presentation parameters tab of the Quality Criteria window.

CONNECTIONS :

BOLT CONNECTION :

1. Now that all the parts have been meshed, we can move onto deploying the connections.

2. To connect regions where a bolt and nut is required, we can use the Two node RBE2 option.

• The RBE2 tool can be accessed via Elements > RBE2 in the NASTRAN deck.
• It primarily has the 'many nodes' and 'two nodes' options.
• This procedure involves connecting two sets of RBE2 spiders using a double con. Firstly, the RBE2 component is created separately for each hole using the Elements > RBE2 > Many Nodes option.
• We can select the nodes surrounding the hole and middle mouse click to form the elements.

• Through this process, we'll have two master nodes (which are to be connected).
• To connect them, use Elements > RBE2 > Two Nodes tool.
• Select the two master nodes to form the connection.
• This process is repeated for all locations where a bolt connection is to be deployed.

SEAM WELD Connection.

• In the case of seam welds, we shall be using the Curves > Cons2Curve option from the topo deck. This will let us select the edge and derive a curve from it.
• Now, we can make use of the connections manager (by accessing it from the upper toolbar).
• The seam line is selected and on proceeding, we get a set of options where we need to tell ANSA what kind of connection we intend on creating. P1 and P2 are selected - To select the PIDs for each, right-click on the option P1 or P2.
• A box pops up. There, we need to press F1. This will let us select the particular PID. (care must be taken to ensure the right component is selected as the base sheet - the layer on which the weld leg will rest). The FE Rep type here would be Overlap Shell since both layers are parallel to each other.

To Carry out Symmetry Operation.

• After we have meshed the entire model and deployed all possible connections, we can go ahead and reflect it to produce the other half of this rear suspension system. This is done using the reflect option from the Transform tool.
• To start off, we need to go to Transform from the upper toolbar. Then select 'Copy'.

LEARNING OUTCOMES :

• Thickness measurement at various parts and decided the type of the component.
• Mid surfacing by using various techniques for sheet metal components.
• Surface Meshing with provided Quality Criteria.
• Defining volumes and doing Volumetric mesh.
• Solving the failed elements by using Mesh improvement tools.
• Use of Symmetry option.

CONCLUSION :

In this project, well connectivity has been established between the surfaces. The features have been captured properly. A good mesh flow have been achieved. Hence the Model has been reflected to the other side successfully. Hence the connection has been deployed in required regions. Hence Mid Surface and Shell Mesh has been performed for the bracket and lower spring insulator component successfully.