Nastran CBUSH Element Orientation
The Nastran CBUSH element orientation is probably one of the most confused and dreaded topics. Let us attack it head on in this post.
- We will discuss the concept of coincident versus non coincident nodes
- Nastran CBUSH element orientation definition
- FEM Model of coincident and non coincident node CBUSH elements
- Element forces when using different orientation definitions
- Element freebody loads based on nastran CBUSH element orientation
Nastran CBUSH Element Orientation – Node Locations
As you can see in the main image at the top of this post, we have two types of CBUSH elements. The first element has both of its nodes (GA and GB) at the same Cartesian Coordinates (X,Y,Z).
Non Coincident Nodes:
The second element nodes (GA and GB) are separated by a small gap (0.001 inches).
Nastran CBUSH Element Orientation – Element Orientation Definition
When a CBUSH element is defined, there are two main methods to define its orientation.
1) Using a coordinate system (CID) in the PBUSH (element property) with an ID greater than or equal to (>=) zero, or CID>=0
This method is typically used for CBUSH elements with coincident nodes. If the nodes are coincident, then there is no gap between them. Therefore it is not possible to use the element’s connectivity axis (GA-GB axis) to define the element’s X-Axis. The coordinate system defines the three primary axes of the element. Any stiffness values are also based on this coordinate system.
The PBUSH property definition dialog box below illustrates the use of the CID check box:
As we can see in the highlighted areas in the figure above, the stiffness values are dependent on the Orientation Coordinate System Axes selected by checking the box at the right.
Stiffness along DOF 1 thru 3 is translational, and stiffness along DOF 4 thru 6 is rotational, about the first three translational DOF.
2) Using a Vector
This method is typically used when the CBUSH element nodes are non coincident. For such elements, the element X-Axis is defined by the axis GA – GB (or GB – GA), in other words, the element connectivity order defines the element X-axis. Then, we are required to define the second axis (Y-axis) by defining the element orientation.
The orientation can be defined either by selecting a third node, or a vector between any two points or nodes in the model. In each of these methods, the element Y-axis is determined based on the direction going from the node A or grid point A (GA) along the selected vector direction.
As we can see from the image above, you can use a node to define the vector, the vector direction is then from grid point GA to the node.
Or, you can click on the Vector button, and then define the vector in the Vector Locate dialog box as shown above using various methods such as Global Axis, Point to Point etc. For example if you use two points (0,0,0) and (1,0,0), this vector is then moved from (0,0,0) to GA to define the second axis of the CBUSH element (Y-axis). The final axis (Z-axis) is calculated using on the cross product of the first two axes, you don’t need to worry about it.
Quick Tip: When using a vector for orientation, the element forces are automatically reported (.f06 or .out files, as well as freebody loads) in this calculated element coordinate system.
Nastran CBUSH Element Orientation – FEM Test Models
In order to demonstrate all the concepts we discussed above, let us build a test model.
A lot of stuff is happening in the model above so let us take it step by step:
- The shell or plate elements are modeled as 0.25″ thick 2024 Aluminum alloy plates (2″ wide x 5″ long), shown above with the ‘shrink’ display option turned on
- The global coordinate system is the RGB colored system at the bottom left of the image
- The model on the right has two plates in an L joint, aligned with the Global CSYS (CID=0)
- Two CBUSH elements connect the two plates together
- In the right hand model, the two plate edges are coincident, and so are the CBUSH elements (defined from bottom plate nodes to vertical plate nodes). There is a reason for this, it influences the sign of the induced load, more on this at the bottom of the post in the FEM section.
- A custom coordinate system is defined at the bottom corner of the model on the left hand side, it makes a 45 degree angle with the global CSYS
- In the left hand model, the bottom plate’s edge at the joint is at a distance of 0.001 inches from the vertical plate edge along Y in the custom coordinate system
- The CBUSH elements in this model therefore have a tiny gap of 0.001″ along Y (defined from vertical plate to bottom plate)
- Nastran CBUSH element orientation for the model on the right hand side is defined in the element property dialog box by selecting CID = 0 (see Figure 1 above)
- Similarly, the nastran CBUSH element orientation for the elements in the model on the left hand side are defined using the X axis of the custom coordinate system (vector method, see Figure 2 above, see the orange colored orientation vector display)
- All the top nodes are fixed
- All the nodes at the outer edge of the bottom plate in the model on the right are loaded with 10lbf each, along X Y Z of the global coordinate system
- The same loads are applied to the model on the left, except in the custom coordinate system
- We run this model and then look at the results
Nastran CBUSH Element Orientation -Coincident Nodes Model
The figure below shows the freebody loads of the CBUSH elements for the plates at the right in the global coordinate system:
Let us do a quick classical hand calculation here to verify these loads. We applied a total of 60lb (10lb on each node). The moment arm for this load is the width of the bottom plate, 2.0″.
Moment M = 60lb*2.0″ = 120 in-lb
Distance between the CBUSH elements L = 3.0″
CBUSH load Ry1 due this moment = M/L
Ry1 = 120 in-lb/3.0″ = 40lb (+Y tension at the bottom CBUSH, -Y compression at the top CBUSH)
Force Balance along Y:
Total Force applied Fy = 60lb
CBUSH load Ry2 due this load = Fy/2 = 60 lb/2 = 30lb (+Y tension at both CBUSH elements)
Therefore, at the bottom CBUSH:
Total Y load = Ry1+Ry2 = 40+30 = 70lb (tension along +Y)
And at the top CBUSH:
Total Y load = Ry1+Ry2 = -40+30 = -10lb (compressive along -Y)
Looking at the zoomed out view of the freebody loads, the directions of these loads may not be immediately apparent, as these are coincident node CBUSH elements.
So the best way to find out is to add them to the “Data Table” (I cover how to use the Data Table in detail in the Finite Element Analysis Course).
See the Table below.
ID 1:Bush X Force 1:Bush Y Force 1:Bush Z Force 1:Bush X Moment 1:Bush Y Moment 1:Bush Z Moment
43 -30.09294 -69.99994 -29.99999 -55.24963 5.562673e-006 7.156822e-005
44 -29.90706 9.999938 -30.00001 -64.75037 -2.459606e-005 0.0001143787
Looking at the loads in bold, we can see that the magnitudes of the loads check out with our classical hand calculation along Global Y.
But, we also see that the signs of the loads are in reverse compared to what we expected. WHY?
This highlights the tricky part of using coincident node CBUSH elements. When a CID is used to define the nastran CBUSH element orientation, the load is always computed as Ke tension based on UGB-UGA. In our case, the element was defined from the node GA on the bottom plate to the node GB on the vertical plate.
Our node 1 or GA is moving away from node 2 or GB. Therefore UGB-UGA is negative and this results in a negative load (associated with compressive load) which is not what we expected from our classical hand calculation.
So the lesson we learned here is that we need to be very careful in interpreting these loads, a simple calculation as we did above will help us understand these loads.
Nastran CBUSH Element Orientation – Non Coincident Nodes Model
In the model on the left hand side, we had a tiny gap of 0.001 inches.
The CBUSH elements were defined from the nodes at the bottom edge of the vertical plate to the corresponding nodes on the bottom plate.
The loads were applied similarly to align with the custom coordinate system. The figure below shows the property used for these elements:
Note how the CID check box is unchecked and the rotational stiffness is now moved to the DOF 5 field (this is because the DOF is is rotation about element Y, and element Y is now DOF 2 with respect to the element vector definition). Click on these links to learn more about: Spring elements in nastran and spring element forces.
See the table below:
ID 1:Bush X Force 1:Bush Y Force 1:Bush Z Force 1:Bush X Moment 1:Bush Y Moment 1:Bush Z Moment
22 70.00993 30.08381 -29.99999 -5.50368e-006 55.26286 7.899204e-005
21 -10.00994 29.91619 -30.00001 2.465597e-005 64.76714 0.0001217757
Since these are non coincident nodes, and we used the vector orientation method, now the loads look very different compared to the previous table. This is unlike using a CID to define the orientation as tension and compression loads are based on relative positive or negative nodal elongation. Perfect!
This makes a lot more sense to me. X is always along the element connectivity axis, and we can see clearly that the tension and compressive loads. Element Y is along the long shear nastran CBUSH element orientation vector direction. And we have 30lb load along Y and Z (short transverse direction) of the elements. We can also see the induced moment due to the rotational stiffness about the element Y axis.
Let us look at the freebody loads in these two CBUSH elements:
This is the key to one of my preferred joint modeling techniques in panel pin modeling, it is covered in detail in the Aircraft Structures Modeling Course.