Fasteners In FEA Dynamics Simulation

How can you best simulate the dynamics response of a structure with a large number of screws or bolted connections? It is often prohibitively expensive to represent all the hardware, and at the highest level of fidelity, both in terms of set-up time, and also for the computational time. This article lays out a strategy for getting the best answer you can in the fewest compute iterations, then we delve into the tactics of accounting for the effect of each fastener.


First, lay out clearly what your goals for the FEA are. If you need to predict the stresses and strains in the fasteners, or in the parts that are fastened, that is one thing. But if you are mostly concerned instead with the product’s displacement responses – that is, the natural mode shapes, the resonance frequencies, and the peak deflections – that is a different thing entirely.

Stress and strain are local properties of particular mesh elements, and they require care that the mesh elements be small enough, have good aspect within themselves, and also in relation to their neighboring elements. Careful meshing, and equally careful application of the screwed/bolted contact conditions, mean that obtaining accurate stress and strain results will always be rather slow.

Displacement response, however, is a property of the aggregate structure. Certainly it is the summing-up of all the individual elemental responses. And it is always true that, if FEA elements are too big, then their behavior is too stiff. But local variations due to numerical truncation, element aspect, etc., tend to cancel each other out across an entire structure. The net displacements are affected by all the elements, not unduly influenced by the handful of elements that are most highly stressed.

So reporting of stresses and strains is all about singling out only the most problematic elements. And reporting of Displacements is effectively allowing every element a ‘vote’, so that the outlier elements have far less of an effect. The good news is that displacement-based FEA problems can be solved faster, with fewer mesh elements, and less effort going into the Fastener boundary conditions – and still retain good accuracy. Also, you can solve faster, and use less space on the hard-drive, by telling the solver to ONLY compute the displacements, but not to bother computing stresses or strains. Figure 1, below, shows the dialog for editing the RESULTS for both a Linear Dynamic study (left), and a Nonlinear study, (right).

Figure 1: Displacement-only studies can opt to run smaller and faster

Figure 1: Displacement-only studies can opt to run smaller and faster.


Users that have access to SOLIDWORKS Simulation Premium, have two available solvers for dynamics problems. By far, the faster of these two is the Linear Dynamics study. Certainly, any kind of dynamics study is going to be non-linear (in time), so the word linear in this study type, refers to the fact that the stiffness matrix of the problem, must be linear. That means no nonlinear materials like rubber, and also no nonlinear boundary conditions, like a sliding contact.

This second limitation is probably the greatest strategic consideration, for representing hardware. If you want to use the bolt connector at all, because you want to take into account bolt pre-load for instance, then your final study must use the nonlinear solver, mostly because the bolt connector must always be used in conjunction with a no-penetration contact set. Also, incidentally, it is because there’s a structure’s dynamics response is shifted, non-linearly, by pre-loads and other background stresses.

Figure 2: Two solver choices for Vibration problems

Figure 2: Two solver choices for vibration problems.

If you are ultimately going to be running a study using the Non-Linear solver, with fast-acting dynamics, and bolt connectors/contacts, then you will certainly want to lighten-up the study anywhere else that you can, to get answers in a reasonable time. Which is why, before I set up and run such a study, I will certainly have run perhaps a dozen or more simpler, faster test cases beforehand.


In any structural vibration problem, my first goal is to learn as much as I can, quickly and cheaply. Then I’ll add detail and pay the performance hit for finer accuracy, only in the specific regions of the model that preliminary studies have pointed to as areas of interest. As I feel my way along in the problem, I’ll discover which levels of mesh refinement, which types of boundary condition, are best suited to my goals, and all lessons learned will be gathered into the final, “for-the-numbers” study. At CAPINC we call this “spiraling in toward the bull’s eye”.

In my first prelim study, what is the cheapest possible way to fasten together plates or sheet metal?   The rigid connector, of course. In figure 3 below, we have an electrics enclosure that is configured to have all hardware removed. In their place, I have added Split Line features that occupy the same footprint that the bolt head or washer/nut would have covered. The base and the cover are sheet metal parts, and so will mesh as shells. But, the rigid connector treatment will work just as well if the fastened bodies are meshed as solid. The rigid connector will enforce that these pairs of faces will remain perfectly planar and rigid – but, unlike a “fixed” relation, they are allowed to ‘float’ in space as needed to follow the large-scale flexure of the cover and base.

Figure 3: Split-line features facilitate using rigid connectors in place of hardware.

Figure 3: Split-line features facilitate using rigid connectors in place of hardware.

What about all of the other surface area where the two main parts lap over? If we allow them to bond, then they will have much higher aggregate stiffness. If we set our Global Contact type to be “Allow Penetration”, then some flexure modes will be allowed where the two plates pass thru each other, and our net stiffness will be too low. Clearly, the most accurate way to represent this situation, ultimately, is with a no-penetration contact set. But for a preliminary study, the lesser of all evils, is to allow the plates to interfere, rather than allowing them to bond.

This will make our vibrational frequencies report lower, and our deflection predictions will be more conservative, than a bonded contact would be. In fact, most parts are machined with tolerances to permit assembly. If there is even so little as .005” clearance between the yellow cover and the gray base, pictured above, before the screws are applied, then the initial stiffness response of the structure will indeed be the lower stiffness of the individual plates, contacting only beneath the bolt/washer footprint. Even when the faces are bowed into intimate contact under extreme bending, the bending stiffness will be closer to the two walls’ stiffness, summed, rather than quadrupled (as if bonded).

Mass And Stiffness

The rigid connector is not the only short-cut to representing fasteners, but I’ll usually try these first, everywhere, and then examine the stresses and deflections to see which fasteners will be the most interesting or problematic. Even if my ultimate goal is NOT to apply a stress or strain criteria, I’ll still look at strain, and (elemental) stress, to see which of my rigid connectors are in need of more accurate treatment. And, there ARE some more tricks we can apply. So, what are the weaknesses of the rigid approach?

Without the fasteners, our mass will be too low, for one thing. But here’s a lucky break; although the software will usually NOT allow you to put two boundary conditions or loads onto a single face, it turns out, you CAN apply a distributed mass to a face, even if that face already supports a rigid connector.

The two studies pictured in Figure 4, below, are the same study, cloned, but the second study has the mass of the screw/washers/nut added to the outer face of each rigid connector pair. The added mass has the expected effect, of lowering the natural frequency and increasing displacements. But we can also see, in this example, that the gain in accuracy is only around two percent.

Figure 4: Mass of removed hardware can be added back on via a distributed mass.

Figure 4: Mass of removed hardware can be added back on via a distributed mass.

The second weakness of the rigid connector, is that it can be too…. well, rigid. It credits the contact areas under the fastener head, with being infinitely stiff. This will reinforce the elements immediately adjacent to the connector, too, resulting in slightly higher frequencies, and (usually) lower displacements. What can we do about this?

In only those fasteners that are attracting the highest strains and stresses, I would delete those rigid connectors, and replace them with a bonded contact set. The bonded contact will take longer to mesh, and slightly longer to run – especially if you need turn on mortar bonding (for higher accuracy in a non-compatible mesh). But, the bonded elements retain much more of their parent-material compliancy, meaning, a softer joint. Stresses in the immediate vicinity will likely be less singular.

Why didn’t we just use the bonded contact in the first place for every fastener? Meshing speed is certainly one reason. But there’s a deeper, tactical reason the rigid connector is preferred. A rigid connection can be applied between sets of faces, that do not touch, do not even need to be parallel, or indeed, anywhere near each other. They work reliably regardless of your part tolerances, assembly clearances, despite disparities in plate thickness, regardless of whether your SHELL definition is on an inside face, outside face, or mid-surface. I wish I could say the same for the bonded contact condition. But I’m sure you’ve already discovered, that to BOND two surfaces in the FEA, the CAD faces have to lie within certain tolerances of adjacency, or at least, of overlap. So it is not worth fighting that battle for EVERY fastener, only to find out, that only a handful of fastener locations are really of interest.

Bonded Variation

Here is a time saving trick that I see used a lot by the SOLIDWORKS support staff, and you’ll see this in most of their FEA tutorials. Where two parts are through-bolted, they will sometimes only model holes in the top or outside plate, and not bother to model the holes on the inner plate. Then the bonded contact set is applied between the EDGE of the outer hole, and the FACE of the underlying plate. In the case of solid meshing, this can save a little time, since you don’t need to mesh/resolve half the holes. And also, you don’t need to create the split line features to isolate the area under the screw head. But in the case of sheet metal and surfaces, meshed as Shells, I find that the software does not like to BOND an edge to an edge. The edge-to-face bond then becomes not just an effort-saving trick, but also a necessity. To get the edge-to-face bond to work, you actually MUST remove the holes from one of the two plates. This treatment is so prevalent among the SOLIDWORKS tutorial and training examples, I tend to believe that it is a hold over practice from an earlier time when our Mortar Bonding option did not exist. My own preference is to create the split line features for the head/nut area, in every case – perhaps that is my hold over habit?

Figure 5, below, is the setup of the part from Lesson 2, “Electronic Enclosure” of the Simulation Dynamics training class. I reference it here because you can go to the SOLIDWORKS User Portal, log in, and download this training set yourself, and look over their study set-up. It also illustrates the edge-to-face bonding approach, even though the dialog windows show a face-to-face selection. Because the faces were selected on sheet metal parts, and these will ultimately mesh as shells, not solids, and so the screw-hole face selection will become an edge of the mesh.

Figure 5


In a special case, where a screw or post or PEM stud is serving as both a fastener, and as a standoff, you have a special case that lies neatly between the two tricks I’ve outlined above. That is, a rigid connector” would work fine, no matter what the standoff distance was – but it would be too stiff. The longer a standoff is, the lower its net spring-stiffness should be. Even if you can get the bonded contact to work across the larger distance, it, too, will be too stiff. How can we de-tune this?

In most of these cases, where you have flat, parallel faces to connect, you can use a spring connector. This connector type is much like a rigid connector, except that you can then soften it by applying an axial, and transverse spring stiffness. The axial stiffness will be really high. It’s just the Young’s Modulus of the material, multiplied by the shank cross-sectional area, and then divided by the effective spring length. The shear stiffness is trickier: you can build a quick CAD model of the part, fix one end, apply a (small) unit of lateral deflection on the other end, and then measure the resulting reaction force. The transverse stiffness that you enter in the spring dialog will just be this reaction force, divided by the applied lateral deflection. Since we don’t care how much of that is shear, and how much is bending, it is quicker to do this in the CAD, than it is to try deriving this by hand with pencil and paper.

I mention this use of the spring connector, for something that is not really a spring, mostly to encourage you to think outside the box. A spring connector can sometimes be thought of as a pin connector, but with tunable stiffness. But more often, I’m working with cases where stand-offs are relatively few, and it is best to leave them represented in the assembly and mesh as solid. And in that case, you tie them into the PCB or into the sheet metal with a bonded contact, on the flat ends. Or, on the circular edges where the standoff might pass through a board, use a rigid connector.

Getting To Final Numbers

The tricks outline above will get you at least ¾ of the way to final results. If you are analyzing a structure for stiffness and not for stresses, and you don’t have any non-linear materials, elastomers, or gap/contact elements, you can stick to the linear dynamics solver and get your answers rather quickly. If you are solving instead (or also) for stress, especially, for stress within the fasteners, then you’ll need to review the stresses in the immediate area of your bonded or rigid connectors, and identify the handful of them that are of greatest concern. In only these locations, you will do one of two things:

  • Re-instate the CAD models of the fasteners, so that you can mesh them as solid elements, or;
  • Use a bolt connector in place of the rigid/bonded treatment, so that you can include contact effects, pre-load stress, and get a full report card on the fastener stresses. This method, of course, requires that you re-define the study using the nonlinear solver.

Taken together, these tricks should get you to accurate predictions, while taking up the least set-up time, putting the most detail into only those areas where you need it, for efficient meshes and faster solution times.

CAPINC was founded on one core principle: Provide the best solutions and services to assist our customers in designing and developing better products. CAPINC provides premier solutions and services in New England to assist our customers in accelerating their design and development process for better mechanical products. Our award winning technical support team is comprised of industry experts with hundreds of years of combined practical experience in mechanical design, design validation and analysis, product data management, and technical communication. We are the award winning 3D solutions partner offering SolidWorks software and training, and the entire Stratasys line of 3D printers and production systems. For more tech tips and blog tutorials check out CAPINC's blog and videos.