ANSA Week 6 Challenge - Creating connections for a rear door model

OBJECTIVE
To perform suitable connections between various parts/components in the rear door FE model provided, after creating and applying different PIDs to the aforementioned components that are part of the model.


CAD MODEL IMAGE

PROCEDURE
1. Firstly, in order to set up the more complex connections for the challenge, it is important to differentiate components as the connections may require different PIDs. This entails the first step. The entire model will be separated into different PIDs. This requires creating said PIDs and that can be done via Faces > Set PID in the topo deck. The region is then selected and the middle mouse is clicked to bring up the properties window.



Here, the new property can be created and assigned as seen above. This process is repeated until PIDs have been assigned for every component/region in the model.

2. We can start off with RBE2 connections. The RBE2 tool can be accessed via Elements > RBE2 in the NASTRAN deck. It primarily has the 'many nodes' and 'two nodes' options. In the following example, we deploy the 'many nodes' option to connect two holes with a single master node. This is merely done by selecting the two sets of nodes surrounding the holes and letting the algorithm create a master node and form connections by running through the straightforward process. This is also known as a cluster node RBE2.

Then there is the two-node RBE2 process. This involves connecting two sets of RBE2 spiders using a double con. The RBE2 component is created separately for each hole using the Elements > RBE2 > Many Nodes option discussed before. Through this process, we'll have two master nodes (which are to be connected). To connect them, we shall be using the Elements > RBE2 > Two Nodes tool. Then it is just a matter of selecting the two master nodes to form the connection. This is typically used in cases where assigning properties for the bolt stem might be a requirement.



However, in this case (which is a hinge), care must be taken to assign the D.O.F.s accordingly. A hinge joint requires yaw movement and as such will have 5 D.O.F.s fixed. Meaning, when defining it during the Two Node RBE process, care must be taken to ensure the value of 'CM' is 12345 (instead of the standard 123456) to allow the aforementioned.

2. There is another way to assign bolt connections which becomes especially useful in cases where there are more than 2 layers that require connecting. This will involve using the connections manager. Before that, we need to create a COG point in one of the holes from a layer in the middle (using the Points > on COG tool from the topo deck).

Then the point needs to be converted into a bolt using the convert tool from the upper toolbar (selecting 3D points).

After converting the point into a bolt, the connection manager is accessed (from the top toolbar) and the bolt point selected. Clicking the middle mouse brings up a set of options that needs to be edited in order to develop the proper bolt connection.

In the set of options, the sections P1, P2 & P3 need to be assigned (since there are three layers). The part on the same plane as that of the bolt point would be P1 and the others can be assigned interchangeably. To select the PIDs for each, right-click on the option (P1, P2 or P3). A box pops up. There, we need to press F1. This will let us select the particular PID.

The FE Rep Type needs to be 'BOLT'. The search distance can be assigned according to the distance from the bolt point (such that the algorithm would detect the other holes in the search distance). I assigned 30mm in this case. And finally, the Zones option would be 'inner'.



As shown in the screenshot, the D.O.F.s can be assigned as well. And here's the result of this connection:

3. Now onto the door handle. In this region, we need to create a connection that applies a mass (to represent the handle). For this, we need to create RBE2 nodes in either handle holes separately (using Elements > RBE2 > Many Nodes):


Again, using the same tool, the two master nodes for either handle hole is selected and another connection is created, with the algorithm assigning a new master node at the centre of this connection.


Now, we make use of the Con Mass tool, accessible through Elements > CONMi > CONM2 > Nodes. Then the previously mentioned master node is selected. This is where the mass of the handle will be concentrated. After proceeding, the algorithm lets us assign the mass ('M' in tonnes) as shown below:


In this case, the mass of the handle is 150 grams (or 0.00015 tonnes). Hitting 'OK' forms the Con mass connection:

4. Next, we shall focus on weld connections. We shall be looking at seam and spot weld connections. In the case of seam welds, the basis is creating the weld locations from curves derived from the particular feature. Therefore, we shall be using the Perimeters > Feat2Curve option from the Mesh deck. This will let us select the edge and derive a curve from it as shown (after creation, the original component can be hidden to avoid confusion):

Then, using the same convert tool that was used earlier, the curve can be converted into a seam line as shown (this time selecting 'curves' from the dropdown menu):

Again, as before, we make use of the connections manager (by accessing it from the upper toolbar). The seam line is selected and on proceeding, we get the same set of options where we need to tell ANSA what kind of connection we intend on creating. As before, P1 and P2 are selected (this time, 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. (Otherwise, Y-Joint Shell option would be selected).

The root shell option would be 'double row'. Other properties (such as width or thickness) and PID can be assigned for the weld as well if needed. The resulting weld turns out as follows:

NOTE: Usually, a spot weld is used (instead of a seam weld) in this location but for project depiction purposes, it has been deployed here.

For spot welds, we shall be making use of the COG tool again to create 3D points. These 3D points are then converted into 'spot welds' as shown:

After conversion, it's the same process of accessing the connections manager and assigning properties. This time, since it's a spot weld, the FE Rep Type would be RBE3-HEXA-RBE3. A suitable search distance is assigned. P1 would be the same component on which the spotweld point is situated and P2 would be the layer below.

RBE3 pinflags should be constrained in all D.O.F.s. Furthermore, a PSOLID will need to be created and assigned. The following are the resulting spot weld connections:

5. The last type of connection involved in this challenge would be that of CBUSH RBE3 elements, which will be used wherever window weather strips (seals used to keep interior air in and external elements out) are involved.

To begin, the perimeter of the glass components is used to create curves. For this, Perimeters > Feat2Curve tool is used to select and create them. These created curves are then used to create a single set of offset copies. This is considering connection requires setting up on either side of the glass. We can make use of the Transform > Copy tool for this. A distance of 5 mm should be adequate:


Selecting the curves, they can be converted into Spot Lines using the Convert > Curves tool. Each curve needs to be selected separately and converted. This is to ensure they aren't grouped together when establishing the connections:


After converting them, we avail the help of the connections manager again to create these CBUSH connections (FE Model will need to be turned back on if it isn't). The process will be repeated for each curve.

For the options, we will need to select the P1, P2 (& P3 if needed) as usual. But here, spacing (S) needs to be specified (10mm). The FE Rep type would be RBE3-CBUSH-RBE3.


With the search distance entered and 'Keep All Branches' checked, we can proceed to create a Bush ID. In the PBUSH ID box, we need to press Shift+? to create a new PBUSH ID. The ID will require 6 stiffness values and they can be entered as shown:


With this, we can go ahead and Apply and Realize the connection. This is the result:

After this process is repeated for each spot line created, we need to reorient them since they use a local coordinate system which is different from the global coordinate system.

To fix this, we can go to Database > Elements > CBUSH. All the CBUSH elements are displayed. They are selected and then right-click > Modify. A modify window comes up where we can add modifications to apply to all the CBUSH connections. In the Modify Rules section, we can add the 'orient' rule and assign the 'With Cord' option to it. A second rule is then added (by clicking the '+') and for this, CID rule is created with the value being '0'. Clicking OK assigns this new modification that reorients all the CBUSH connections to that of the global coordinate system.

FINAL MODEL IMAGES

With all connections:

LEARNING OUTCOMES

1. Learned about various connections available in the NASTRAN deck.

2. Learned to convert curves and points into connection lines/points.

3. Learned to assign properties to connections and edit said connections as per requirements.

4. Learned about the concept of weather stripping and its importance, along with the concept of tailor welds.

CONCLUSION

Suitable connections were deployed between various components in the rear door model after PIDs were assigned to each component.