# Static Analysis of 3 bars under thermal and mechanical loads, connected to a rigid beam (Method 1)

### Aims and expectations at this course

Our expectation after you study:

1- Integrated modeling of rigid and deformable wire type parts

As the Figure shows, a rigid beam, AB, hanged via 3 vertical bars with the same lengths and cross sectional areas (0.1 in2). The middle bar is made from steel while the others are from copper. The temperature of bars increases 10 oF and a load of Q=4000 lb is applied on middle of the rigid beam. We are aiming to calculate the stresses in all bars, firstly and then, compare them with the results given in reference [1]. The material properties have been presented in Table 1.

Table 1: Bars material properties

### Creating the model:

In the first step, rename the model to hanging slab. Click on icon (Create Part), then, in opened window select the items shown in Figure 2 and Continue.

Clicking on icon (Create Lines: Connected) draw a sketch same as what displayed in Figure 3. Put Vertical (V) and Horizontal (H) constraints if they would not be created automatically.

Using the constraint tool of Equal length, make the bars lengths equal. After that, utilize the icon (Add Dimension) icon and put the dimensions displayed in Figure 4. Finally, fix one point of the system by use of Fixed constraint. As we learned before, all parts appear in green which means they are fully defined.

After all, exit Sketch module.

### Material property definition:

Enter Property module. Create two materials with names of Steel and Copper and the material properties presented in Table 1. Then, create a couple of Truss sections, named section-steel and section-copper which are related to the materials of Steel and Copper, respectively. In both sections, insert 0.1 in2 as their cross sectional areas. Next, assign section-steel to the middle bar and section-copper to the bars in left-hand and right-hand sides. Here as the material of horizontal beam which is rigid and has no influence on simulation, assign the section-steel to this part, too. To find out more take a look at note 1.

### Note 1

When the rigid part is modeled in a deformable part in one integrated step, we need to assign a material section to it. In order to make this part known as rigid part for the Abaqus/CAE we will use a tool in Interaction module changing a deformable tool to a rigid one. If we do not assign the material an error will be shown, which is displayed in Figure A, when submitting the job.

The error says in addition to defining rigid body property, you are required to assign a section.

### Inserting parts in Assembly module:

Enter Assembly module, then, insert the part you created above, in this module. According to Note 2 explained in Example 1, we prefer to bring the part in assembly environment, Independently. Now, save the model in a folder with name of three-bar-method1.

### Define the static analysis:

Enter Step module and create a Static/General type step.

### Defining rigidity constraint related to the horizontal bar:

Enter Interaction module. In order to define a rigid part, a Reference Point must be created, as when rotating or translating this point, the other points of rigid part move relevantly. To create this point, you can pick every point whether laid on the rigid part or in the other areas. To ease selecting and finding the reference point, let’s choose a point below the rigid part but in line-path of the middle (steel) bar. To do this, firstly, we must define a Datum Point. So, from menu bar, select Tools, then, Datum. After this, in opened window, select the items shown in Figure 5.

Now, choose the point specified in Figure 6.

Insert the coordinate of (0,-1,0) in prompt area and press Enter key. This creates a point having a vertical distance of 1 in from mid-point of horizontal bar. After this, click on icon (Create Reference Point) and select the Datum Point you have just created. A yellow cross sign with named RP-1 emerges symbolizing that in this point, a reference point has been defined. After this, you can bond the rigid bar to the reference point clicking on icon (Create Constraint). In opened window, choose Rigid Body and click on Continue button. As displayed in Figure 7, select the item Body (elements) and hit the icon (Edit Selection).

Pick two sub-elements of horizontal bar and press Done in prompt area. To assign the reference point to this bar, click on icon (Edit) which is pointed out in Figure 8.

Then, select RP-1 in viewport and finally, press OK button, to complete the process of defining rigid part. As you can see in viewport, some yellow circles will appear on the horizontal bar. It shows that this bar has become rigid body. Take notice that this part can be controlled by the reference point of RP-1.

### Applying loads and defining boundary conditions:

Enter Load module and click on icon (Create Boundary Condition). Constrain U1 and U2 of the nodes which Figure 9 shows.

Clicking on icon (Create Load), apply a force of 4000 lb on RP-1, pointed out in Figure 10, with direction of negative Y.

To define an increase in the temperature of elements, click on icon (Create Predefined Field). Apply a temperature difference of 10 oF on vertical bars. Figure 11 shows an entire view from the model, including boundary conditions, load and temperature difference.

### Meshing the model:

Enter Mesh module and select Object: Assembly, as we chose Independent item when inserting the part into assembly environment. We learned in previous examples, in truss type structures, each member must be meshed with 1 element. Here is the same, so, use the icon (Seed Edges) and segment each bar with 1 element. After that, click on icon (Mesh Part) and mesh the part. Finally, use the icon (Assign Element Type) and specify Truss element type for the meshes. As you learned, the element type is symbolized by T2D2 showing that related elements are 2D truss, having 2 nodes. Totally, there created 5 elements in the model while 2 of them will be considered rigid when analyzing the structure.

### Analyzing the problem:

Enter Job module and clicking on icon (Create Job) create a job with name of bar3-slab, then, Submit it. The job will be solved without any warning except initial temperature definition hint, which is fine. After that, by pressing Results button enter Visualization module. Click on icon (Plot Contours on Deformed Shape) in this module, to observe deformed shape of the model. Now, go through below path in menu bar:

Report > Field Output

Extract the stress S11 produced in vertical bars with 9 decimal digits using the method you have learned through Figures 46 and 47 in Example 1. Regarding to making a comparison, the results earned from Abaqus/CAE and reference [1], have been presented in Table 2.

Table 2: Stresses in vertical bars, obtained from Abaqus/CAE and Reference [1]

### References:

[1] Timoshenko, S. P., “Strength of Materials, Part l, Elementary Theory and Problems,” 3rd Ed., D. Van Nostrand Co., Inc., l956, p. 30.