This chapter demonstrates the SOLIDWORKS simulation procedure for structures that primarily support axial loads. The simplest form of this type of structure is known as bars or rods. In the more complex form, they are known as plane and space trusses (which are just the two-dimensional and three-dimensional arrangements of bars, respectively). By the end of this chapter, you will be familiar with the procedure for the simulation of the aforementioned structures. Against this backdrop, the focus of this chapter is anchored on the following topics:
You will need to have access to the SOLIDWORKS software with a SOLIDWORKS Simulation license.
You can find the sample files of the models required for this chapter here: https://github.com/PacktPublishing/Practical-Finite-Element-Simulations-with-SOLIDWORKS-2022/tree/main/Chapter02
This section provides basic background information about bars and trusses. It highlights the objectives of analyzing these structures and their applications.
Let’s start with some basic definitions. A bar is a structure that is designed to support simple forces along its axis (such as tensile and compressive loads). On the other hand, a truss represents a collection of bars that are arranged as one or more units of triangulated frameworks. Discussions on the analysis of either of these types of structure (that is, a bar or a truss) often deserve separate standalone chapters. Nonetheless, since the analysis of bars is simpler than that of trusses, we shall allocate more time to the simulation of trusses with the understanding that the same knowledge carries over to the analysis of simple bars.
Note
Within the subject of mechanics, a structure broadly refers to a body or a collection of bodies designed to carry loads. Most structures are three-dimensional (3D) in nature. But for ease of analysis, engineers often leverage approximations that facilitate the use of one-dimensional (1D) members (such as a bar, a shaft, a beam, a column, and so on) or two-dimensional (2D) approximations (such as plates and shells, and so on) to reduce the computational burden of complex 3D analyses.
You will have seen the application of truss structures in various forms around you. Some of these are shown in Figure 2.1. Typically, truss structures are featured prominently in the design of cranes, truss booms, telecommunication towers, masts, electric pylons, roofs, bridges, and so on.
From an engineering performance analysis point of view, we conduct static analyses of bars and trusses with the following objectives:
In bars and trusses, the axial deformations manifest in the form of shortening (contraction) or lengthening (extension) of a member’s length. Consequently, a combination of compressive and tensile normal strains/stresses develops in these structures. Together, the stress and the deformation data that we retrieve from simulations help in determining the right geometric sizing for the members (called proportioning). But crucially, the results contribute towards our ability to design these structures to hedge against unwanted failure or excessive deformation during in-service usage. For brevity, in the rest of this chapter, we shall be using the term truss as a shorthand for axially loaded structures.
Before we get deep into analysis, it is important to be aware of the following technical points that are frequently considered for the computer analysis of trusses:
With the background information provided about trusses, let’s now take a look at strategies for their simulations in the next section.
This section describes the structural details and the modeling strategies for the simulation of truss structures. It also highlights the major features of the truss element within the SOLIDWORKS Simulation library.
Trusses can be designed to function under a wide spectrum of load-supporting applications. However, irrespective of what form they take in appearance, a consistent set of parameters is employed for their analyses. This implies that irrespective of the form of the truss you are analyzing, you will need to know the following technical information before venturing into the analysis:
Note
In practice, a chunk of time will be spent spelling out the scope of the problem relating to structures’/products’ design and analyses. Things such as what the magnitude of the load should be. In what environment will the truss be used? What materials should be used? What types of support are required? What dimensions should be assigned to each member? And so on. In short, to achieve meaningful simulation results, attention should be paid to project specifications and parameters before commencing the simulation tasks. That said, for much of this book, these details will be provided so we can focus squarely on the simulation tasks without getting bogged down by the time-consuming iterative conceptual design tasks.
When we analyze truss structures via the finite element simulation method, a basic strategy is to take a structure such as that in Figure 2.2 (a), split it into its constituent members (Figure 2.2 (b)), and then treat each member as a truss element. So, in the end, a whole structure formed from the assembly of different members is represented by the collective behavior of individual truss elements.
Figure 2.3 illustrates the other aspect of the strategy for the simulation of trusses:
In the traditional theoretical treatment of the finite element simulation method, the truss element is generally known to be a plane element with two nodes and two degrees of freedom. Within the SOLIDWORKS Simulation environment, the truss element is a 3D two-node element with three degrees of freedom per node (that is, translational displacements about the x, y, and z axes). The beauty of the 3D truss element in SOLIDWORKS is that it can be used to analyze 1D bars, 2D plane trusses, and 3D space trusses.
We will go through a case study in the next section to explore further details about the simulation of a loaded truss structure.
In this section, we will demonstrate the use of the truss element with a practical case study. Primarily, we will analyze the structural performance of a crane used in the spatial positioning of heavy objects on a mega building construction site. The example is inspired by exercise 4.11 in the textbook by Megson [1] (see the Further reading section). It is a practical problem that can only be solved satisfactorily via computer analysis.
Time for action – Conducting static analysis on a crane
Consider the 2D representation of a crane shown in Figure 2.4, which is to be analyzed based on the placement of 1500 kN and 2000kN weights at points R and W, respectively.
For convenience, we shall consider that the members of the crane are derived from tubular alloy steel. For this material, the Young’s modulus, E, is taken as 210 GPa. The members have the same cross-sectional detail characterized by external and internal diameters 200 mm and 80 mm, respectively. Using SOLIDWORKS simulation, we want to answer the following questions:
The first step in any analysis is to have a model of the structure to be analyzed. This section centers around the creation of the basic geometric lines describing the structure.
To create the skeletal sketch of the model, launch SOLIDWORKS and follow these steps:
After step 2, the New SOLIDWORKS Document screen appears. We are interested in creating the model using the Part modeling environment.
The SOLIDWORKS user interface opens up and we can start sketching right away. But before that, it is a good idea to ensure you are using the right unit of measurement.
Look at the lower-right corner of the graphical user interface (GUI) to ensure that the current unit of measurement is the MMGS (millimeter, gram, and second) system of units, as shown in Figure 2.6.
Once it is confirmed that the right unit is set up, you may save the file as Crane.
The view of the crane shown with the problem statement represents the front view. Consequently, we shall sketch the geometric model of the truss on the front plane:
After completing the sketch, it should look as in the screenshot shown in Figure 2.8. Now, the sketch we have created in this section is just a series of lines with no volume property. As such, it cannot be used for structural analyses. In the next section, we will convert the sketched line-based model into a structural model with a volume property.
This section explains how to convert the line sketches we created in the preceding section into a structural model using a special functionality in SOLIDWORKS called the weldments tool.
The weldments tool in SOLIDWORKS makes it easy to prescribe the cross-sectional details for sketched lines. In other words, it facilitates the transformation of lines with no volume properties into structural members with volume properties that are suitable for realistic engineering simulation.
The weldments tool can be used with both 2D and 3D sketches. What is more interesting about this tool is that it provides us with access to a handful of relevant structural profiles, such as those listed in Table 2.1.
The profiles highlighted in Table 2.1 are stored in the SOLIDWORKS installation folder. For instance, for laptops/PCs with a Windows operating system, the folder is located at Drive:Program FilesSOLIDWORKS CorpSOLIDWORKSlangenglishweldment profiles.
Note that Drive is a placeholder for the storage drive containing the SOLIDWORKS installation folder on your device. Scrutinizing the aforementioned directory address, you will notice that the profiles are contained in the parent folder named weldment profiles. This folder contains sub-directories, as shown in Figure 2.9 (a). Further, opening any of the sub-directories will expose relevant files with the .sldlfp extension, as shown in Figure 2.9 (b).
Now, the profiles that are bundled with the weldments tool have pre-defined dimensions, but these dimensions may differ from what we need. Consequently, it is common to have to adjust or edit these profiles to fit our needs. For instance, the external and internal diameters of the cross-section we need are 200 mm and 80 mm, respectively (from the problem statement). However, the largest tube within the weldment profiles folder differs from these values, as indicated in Figure 2.9(c). In the next sub-section, we will explore how to edit the profile for our needs, but we first need to activate the weldment profile.
Information
Our main interest is in using the weldment tool to supply the cross-sectional details of the members. However, it has many features that can be further explored. Relevant details can be found by following this SOLIDWORKS help link: https://help.solidworks.com/2022/english/SolidWorks/sldworks/c_Weldments_Overview.htm?verRedirect=1.
Check the set of items in your SOLIDWORKS’s CommandManager tab to see if the Weldments tab is present. If the CommandManager tab is missing the Weldments tab, then follow these steps (summarized in Figure 2.10):
With the Weldments tab on, the next sub-section illustrates how to convert the sketched lines to structural members.
Follow these steps to transform the sketched lines into structural members:
Once you have clicked on the Structural Member command, the Structural Member property manager window will open on the left side of the GUI. Select the options highlighted in Figure 2.12.
For ease of forming the structural members, Figure 2.13 (a-f) illustrates the series of lines to be selected for each group.
By completing steps 1-9, the Feature Manager tree will appear with some additional items. Five of these are highlighted in Figure 2.15:
The cross-section that we have employed from the weldment library is not the same as that stated in our problem statement. Thus, it is necessary to change the dimension of this cross-section to suit our needs. To do this, take the following steps:
Completing steps 1-5 wraps up the creation of the structural model with a volume property, and we shall next transition to the initiation of the simulation study.
In this section, we will activate the Simulation add-ins, specify the material for the members, indicate how to select the truss element, apply fixtures/loads, and finally, initiate the meshing process.
Follow these steps to activate the simulation tab and create a new study:
After completing steps 1-7, you will notice the changes shown in Figure 2.21. Basically, joints will be imposed at the connection points between the members of the truss. At the same time, the Simulation commands will become available:
In the next sub-section, we will specify the material property for the members.
Every single member of the crane is assumed to be made of the same material. This makes it easy to apply the material to the members at once:
Step 2 launches the material database, which is shown in Figure 2.23. For our analysis, the material that we want is alloy steel, which will be located in the sub-folder called Steel. If necessary, expand the Steel folder, then perform the following steps.
Before moving to the next sub-section, there are a few features to be observed with the material database. First, the material database is a multilevel directory. At the top layer is SOLIDWORKS Materials, then we have sub-folders that contain the same family of materials, and another sub-folder for custom materials. Second, the material property names in Figure 2.23 are either in black, blue, or red font. In general, the material property names in red font are the ones that are necessary for static analyses. Without values provided for the property names in red font, the simulation will not run. Thirdly, a material failure criterion (Max von Mises Stress) and Linear Elastic Isotropic material model are pre-defined for the selected material. Lastly, after closing the material database window, a green tick mark (ü) will appear on the study name.
By default, SOLIDWORKS Simulation treats a structural member that is created using the weldment tool as a beam element during the analysis. However, for our case study, what we need is a truss element. Therefore, in this sub-section, we will convert all the structural members from beams to trusses. To do this, in the simulation tree, do the following:
Repeat sub-steps 2-6 for every sub-folders under the Cut list to convert the beams to trusses. After completing the conversion of all members, we can now move on to the next phase, which is about the application of constraints or what we often refer to as boundary conditions.
A fixture is a constraint that we apply to structures to restrict the movement of its joint/segment when loads are applied. For this analysis, we will apply three sets of restraints to the structural model of the crane:
Let’s start with the application of the first fixture to all the nodes by following the steps highlighted next.
Applying a fixture to restrain the Z motion of all nodes:
Steps 1-7 will impose a zero translational movement on all the nodes along the z axis. This ensures that we are doing a plane analysis.
Next, we will apply the restraints at joints A and B, both of which are located at the base of the crane, by following the steps given next.
Applying fixture on nodes A and B:
Note that for joint A, we could also use the fixture named Immovable (No translation); it performs the same function as what we did using Use Reference Geometry. For joint B, we restrained the movement along the vertical direction only, which is meant to replicate the behavior of a horizontal roller support.
At this stage, we are done with the application of all fixtures that need to be applied for our analysis. In the next sub-section, we will swing our attention to the specification of loads. This will inch us closer to running the analysis.
Different types of loads can be used in SOLIDWORKS Simulation. For our analysis, we need to apply what is often referred to as payload weights represented by two vertical forces at joints R and W. We will apply the loads by using the External Loads command under the simulation study tree.
Follow these steps to apply the two forces at joints R and W, create the mesh, and then run the analysis:
After completing step 10, the appearance of the model in the graphics window will be as shown in Figure 2.31. The model is displayed in an isometric mode so that the arrows indicating the loads at joints R and W and the fixtures at all joints become apparent.
The next task is to mesh and then run the analysis, which is what happens in the next sub-section.
Meshing is an essential part of finite element simulation. There are two approaches for creating a mesh in SOLIDWORKS Simulation. The first involves creating the mesh using the command Create Mesh, while the second involves using the command Mesh and Run. For this chapter (as well as Chapter 3, Analyses of Beams and Frames, and Chapter 4, Analyses of Torsionally Loaded Components), we will be using the second approach. Principally, this approach combines the meshing and running of the analysis in a single step, and it works well whenever we use the weldment tool to create the members of a structure to be analyzed. Now, it is good to be aware that SOLIDWORKS does not provide the option for controlling the mesh quality for a structure idealized as a collection of truss elements. This means there is no point in engaging ourselves in the refinement of the mesh that we create for this problem. Further, it means if a truss is made of up 41 members, then only 41 truss elements are sufficient to analyze it accurately. Nonetheless, we will explore meshing in more detail, for instance, in Chapter 5, Analyses of Axisymmetric Bodies, and Chapter 6, Analyses of Components with Solid Elements.
Bearing the aforementioned detail in mind, we can now deal with the last steps before getting our desired results, to this end:
After completing steps 1 - 2, the study tree will appear as shown in Figure 2.32 (b).
We will examine the results folder further in the next section.
Now that we have completed the steps in the previous sections (that is, Parts A-C), we are now in a position to make sense of the results and answer the following questions:
But before answering these questions, it is worth noting that by default, when you use SOLIDWORKS for static studies, it generally computes, among others, the Displacements at the joints or nodes of the structure, the Reaction forces at the points of supports, the Strains/Stresses on an element/at the nodes, the Factor of safety, and so on.
Nevertheless, SOLIDWORKS Simulation will not always display all results. In fact, in most cases, the default results may not be what you want (you may simply right-click on them and then delete them). However, you can create custom plots of many more results and have them displayed in the Results folder. Let’s start by examining the maximum resultant deformation in the next sub-section.
To retrieve the maximum resultant deformation experienced by the structure, simply navigate to the Results folder and double-click on Displacment1 (-Res disp-), which is the result relating to the resultant displacement. After double-clicking, the graphics window with the results of the resultant displacement is shown in Figure 2.33.
The legend describing the displacement plot (on the far right of the screen) displays the range of the displacement from a very low number (in blue) to the maximum value (in red). It also displays the legend with the scientific number format. It is always better to present the result in a more readable format. Therefore, in the next set of steps, we will edit the display of the maximum resultant displacement value by following the steps given next:
Figure 2.34 indicates that with a combined load of 3500 kN applied to the crane, the maximum deformation experienced by one of the joints is 39.764 mm.
Note that since a truss element has three translational displacement degrees of freedom at its node, the resultant displacement refers to the vectorial resultant displacement.
The factor of safety (FOS) is one of those results that are not automatically displayed but need to be retrieved during the post-processing of the results. From knowledge of the mechanics of materials, we know that the calculation of the factor of safety is based on certain failure criteria. SOLIDWORKS Simulation offers four failure criteria that we shall explore further in Chapter 5, Analyses of Axisymmetric Bodies. Nonetheless, irrespective of the criterion used in calculating the FOS, the rule of thumb is that the component we are analyzing has failed if the FOS is less than 1. But if the FOS is greater than 1, then the component is considered safe to support the applied load without failing (all things being equal). To retrieve the FOS, in the simulation study tree, do the following:
Figure 2.36 reveals the distribution of the FOS for the crane upon the application of the load.
The figure indicates that the minimum FOS within the members of the crane is around 3.6, which means all is well with the crane. Note that by going with the Automatic option in step 3, SOLIDWORKS will use the failure criterion specified in the material property database, which is the Max Von-Mises failure criterion (see Figure 2.23).
The last set of results we will look at is the axial forces and stresses. To retrieve either of these results, in the simulation study tree, do the following:
Note
To retrieve the axial stresses, change to Stresses in the box labeled 1 in Figure 2.37 (b).
Immediately after we complete steps 1-4, the List Forces window will appear in the graphics window as shown in Figure 2.38. You may use the arrow (marked 2) in Figure 2.38 to navigate through the values of the axial force developed in different members of the structure. You can also click on the name of a specific member and SOLIDWORKS will instantly highlight it in the graphics window.
For instance, Beam-19 (be aware that the name of this member will likely be different in your case) is the element that corresponds to member IH. It has been highlighted within the List Forces window for convenience. As you can see, this element experiences an internal axial force of approximately 727 kN. This value is within 3% of the answer (707 kN) obtained in [1]. Note that this is the only value computed in [1], simply because it is not trivial to carry out the manual calculations of the other values (displacements, FOS, forces, and stresses) without incurring substantial errors. Indeed, the small difference between the value from SOLIDWORKS and the cited reference may be attributed to possible rounding off errors.
In many practical instances, you will want to list out all the forces/stresses for further examination. To do this, simply click on the column name Axial (N) (labeled 1) in Figure 2.39. This will give a compact display of the values of all 41 elements used in our analysis. From here, click on the Save button at the bottom of the List Forces window (labeled 3) to save all the data to an Excel file, then click Close to close the window. Afterwards, you can explore the data in Microsoft Excel.
You will notice that beyond the axial forces, the List Forces window has other columns, such as Shear1, Shear2, and so on. At the moment, they all are zeros because we are employing the truss element option. For analyses that require the use of beam elements such as frames, they will not be zero.
We have used the truss element in this chapter to study the computer analysis of a crane idealized as a 2D planar truss. However, the truss element and the procedure outlined in this chapter are also perfectly suitable to study straight bars and 3D space trusses. For conciseness, the deployment of the truss element to investigate the structural performance of components made of simple bars is demonstrated in the computer file of the first exercise question at the end of this chapter.
This chapter has covered some basic concepts in the use of SOLIDWORKS Simulation for the static analysis of trusses. We have explored how to create the skeletal lines describing a truss structure and the conversion of these line sketches into structural members with volume elements using the weldments tool. Overall, the following ideas have been addressed:
In the next chapter, Chapter 3, Analyses of Beams and Frames, we will study the use of beam elements for the analysis of transversely loaded components and study the usefulness of these elements for more complex analyses.
a. Determine the displacement of end C.
b. Evaluate the axial stresses developed in the components upon loading.
a. Determine the resultant displacement of joint B
b. Determine the minimum factor of safety of the assembly
[1] Structural and stress analysis, T. H. G. Megson, 4th, Ed, Butterworth-Heinemann, 2019.