fbpx

Shell vs Solid Elements: are they similar?

May 27, 2021
Posted in Posts
May 27, 2021 Nikita Gurov

Regardless of whether you’re at the beginning of your Finite Element Modelling journey or have more extensive experience in the field, you probably know that meshing is one of the hottest topics.

There are many questions associated with mesh, such as mesh size and mesh convergence, but very often the first question that comes to mind is, “When should I use shell elements and when should I use solid elements?

Even though our computers and software are 10x more powerful than a decade ago, it’s still a dream to have a tool that would automatically generate mesh, removing the headache of 3D model preparation and simplification.

For many people it seems much easier to mesh a solid body with solid elements. However, meshing thin-walled bodies like sheet metal parts with solid elements isn’t always a good idea.

Let me show you when to use solid elements and when to use shell elements

When dealing with FEA there are always two important factors to consider: accuracy and time.

As we all know, accuracy is incredibly important in engineering practice, particularly when it comes to stress analysis. At the same time, engineering labour is expensive and tough deadlines push us to finish the analysis quickly.

Throughout the following test models, I will demonstrate shell and solid elements from the two opposing positions of accuracy and time.

I will detail a comparison of the results for the following six test models:

Test #1

Linear elements
Initial mesh size 5mm

Test #2

Parabolic elements
Initial mesh size 5mm

Test #3

Parabolic elements
Initial mesh size 2.5mm

Test #4

Parabolic elements
Initial mesh size 1.25mm

Test #5

Final refinement
Parabolic elements
Initial mesh size 1.25mm
0.2mm mesh fillet refinement

Test #6

Parabolic elements
Smaller fillet radius
Initial mesh size 1.25mm
0.2mm mesh fillet refinement

These results will provide general recommendations for the application of shell and solid elements. You can also see a test results summary table at the end of the article.

Solid elements and shell elements

Solid elements are designed with an assumption that their primary deformations are tension, compression and shear, while effects of bending for a single element are ignored. Therefore, solid elements have only three Translational Degrees of Freedom at each node and no Rotational Degrees of Freedom.

In practice, this means that using a single layer of solid elements to simulate bending could lead to inaccurate results. The impact on accuracy is particularly strong when thin-walled bodies meshed with solid elements using linear approximation. It produces an effect called shear locking, which makes the model rigid and leads to incorrect stress values.

Autodesk Inventor Nastran creates solid elements with parabolic approximation by default. These elements have additional mid-side nodes and to some extent are able to simulate bending.

Modelling with parabolic solid elements certainly makes situations better, but it still doesn’t guarantee high accuracy. Sometimes geometry, applied loads and constraints create conditions where deformation and force change rapidly in some areas (high gradient).

There is a risk in these areas that the parabolic approximation may limit rapidly growing change and can result in lower than actual stresses.

There is another factor that could affect accuracy – degenerated elements. Often when we mesh thin-walled bodies elements lots of solid elements have bad aspect ratios and sharp angles.

Is decreasing mesh size the answer?

The obvious method to overcome this issue is to decrease mesh size. However it leads to another problem: the finite element model becomes too heavy.

If we attempt to make the solid element size equal at least to material thickness in thin-walled models, the following is likely to occur:

It will significantly increase time to solve even a static linear analysis

Solving non-linear analysis becomes too time consuming – days, even weeks

As you can see, I’m leaning towards using shell elements for thin-walled models, but I assume that the arguments above are not enough for some readers, because meshing with solids is easier.

So, let’s compare solid and shell elements in action.

FEA Test Setup

I’m not a big fan of making experiments with basic restrained beams or plates. So, I modelled a more realistic example – a 0.5mm thick sheet metal part with three emboss features.

I then extracted a mid-surface from it to create a finite element model using shell elements. The second model is created using solid elements.

Finally, I used identical settings for both models in Autodesk Inventor Nastran:

  • Load: 10N on each emboss applied at holes
  • Constraints: one side fully fixed, other sides are fixed in vertical direction only (rotation around the edge allowed)
  • Linear static analysis. Read about different types of analysis – Static Linear, Static Nonlinear and Explicit
  • Variable parameters: elements types (shell and solid), elements approximation function (linear and parabolic) and initial mesh size

NOTE: the main purpose of this model is to demonstrate the applicability of shell and solid elements to the thin-walled bodies analysis. This finite element model does not consider effects of material thinning and residual stress from manufacturing operations. This model does not cover topic of design optimization.

Test #1

Linear solid elements vs shell elements, Initial mesh size = 5mm

I first tested linear solid elements to demonstrate the impact of shear locking.  The initial mesh size is 5mm for both models (shell and solid elements).

Displacement Results

The displacement results for solids are quite shocking:

  • Maximum displacement in the model with shell elements is 0.81mm
  • It is only 0.005mm in the model with solid elements
  • That’s 162 times the difference between shells and solids

Stress Results

Let’s look at the stress picture. As expected, the model with solid elements demonstrated a tremendous difference in stress results. The maximum stress in the solid element model (2.7MPa) is completely unrealistic and 41 times lower than in the model built using shell elements (110.5MPa).

Test #2

Parabolic solid and parabolic shell elements, Initial mesh size = 5mm

Now, let’s test the models with parabolic shell and parabolic solid elements (elements with mid-side nodes). This will help to reduce the impact of shear locking. For this test I used the same mesh size and other settings, only changing the element approximation function from linear to parabolic.

Displacement Results

As you can see, a single layer parabolic solid element can simulate bending. But the parabolic shell model and parabolic solid model still give slightly different results – displacements in the model with solid elements (0.66mm) are 23% lower than in the model with shell elements (0.81mm).

Stress Results

Using parabolic shell elements instead of linear shell elements makes the stress results 1.5% higher – 112.2MPa vs 110.5MPa respectively. However, the mesh size around the fillet remains quite large and could produce inaccurate results due to high stress gradients.

At the same time, the model with parabolic solid elements is lagging behind the shell model showing maximum stress = 105.4MPa.

Click on image to enlarge…

Test #3

Parabolic solid and parabolic shell elements, higher density mesh, Initial mesh size = 2.5mm

In the next test I increased mesh density by applying an initial mesh size of 2.5mm. It resulted in a heavier model. But the decreased mesh size minimised the difference between shell and solid models.

Displacement Results

This time the parabolic solid elements demonstrated maximum displacement 0.806mm, while the shell element model displacement demonstrated a very minor change of 0.823mm (2% higher than the solid element model).

Stress Results

The stress result in the shell elements model increased by 8.5% compared to previous analysis, demonstrating better mesh convergence.

At the same time, the higher mesh density led to a 22% increase in stress in solid elements model (128.6MPa vs 105.4MPa).

Test #4

Parabolic solid and parabolic shell elements, 2x Higher density mesh, Initial mesh size = 1.25mm

For the fourth test, I decided to continue the mesh refinement by making the initial mesh size 2x smaller than in the previous analysis.

Displacement Results

This mesh refinement made displacement results between shell and solid almost identical (0.827mm solid vs 0.815mm shell). At this point I can confidently conclude that the displacement results became stable.

Stress Results

The stress results are almost identical to the previous test. However, I observed that changes to the initial mesh size didn’t make the mesh around stress concentrators smaller. This explains the stability of the maximum stress points. A closer look at the stress picture around the stress concentrators reveals a need to continue refinement in this area.

Click on image to enlarge…

Test #5

Final refinement, Parabolic solid and parabolic shell elements, initial mesh size = 1.25mm + 0.2mm fillet refinement

When I took a close look at the stress plot around the maximum stress hot spot I realised that despite good correlation between shell and solid models there is a chance that the shell model is incapable of providing accurate results in areas like the emboss fillet.

What I mean by this is that the fillet radius measured from the mid-surface is comparable with material thickness and the shell elements are not designed to calculate the correct results in those situations. In order to confirm my assumptions, I applied 0.2mm Local Mesh control to the fillet faces.

Stress Results

The solid model returned a 9% higher result than shell elements, confirming my assumptions. As you can see the next logical step is to explore this limitation of shell elements by reducing the fillet size to 0.75mm (see test #6).

Click on image to enlarge…

Test #6

Smaller fillet radius

I created this model on the basis of the previous analysis: initial mesh size=1.25mm, local fillet refinement=0.2mm.

Stress Results

As expected, the solid elements demonstrated 49% higher stress (211.7MPa vs 140.8MPa) than shell elements. I think this is a good example which demonstrates the limitations of shell elements in situations when surface curvature or feature size is comparable to the material thickness.

Click on image to enlarge…

Recommendations

Using solid elements is an easy way of creating mesh. However it’s not possible to simulate everything using solids. Therefore, my recommendation would be: for thin-walled bodies use shell elements.

  • A single layer of linear solid elements cannot simulate bending.
  • In general, parabolic solid elements can simulate thin-walled bodies if the element size is less than 2.5x material thickness. Ideally, at least 2 layers of solid elements across the material thickness.
  • In order to obtain quality results from solid element models it is necessary to dramatically reduce mesh size. It comes at a high computational cost making this method impractical for large assemblies and nonlinear analysis.
  • Solid elements are sensitive to high stress gradients, particularly in thin-walled bodies and require fine mesh (two elements across material thickness) in critical areas.
  • Shell elements produce good results at low computational cost.
  • Shell elements are not capable of providing accurate stress results for model features comparable with material thickness. It is recommended to use shell elements to model features more than 10 times larger than the material thickness.

Test results summary table (linear static analysis)

The next steps in your FEA journey

  • Would you like to learn practical FEA and start confidently using it in your everyday work?
  • Are you looking for a highly accessible and practical FEA course where you can build finite element models from scratch?
  • Do you want to learn a range of FEA tricks and time-saving tools for your own designs?

Please get in touch

I would love to hear more about your current design challenges and help you understand how FEA could benefit your work. Feel free to contact me – fea@wordpressmu-726877-2424848.cloudwaysapps.com

, , , , , , , ,

Comments (3)

  1. Alan Missenden

    Nikita,
    Sorry to be a pain, it is always very easy to criticise, and a lot of the work you have presented is very interesting, but I am concerned about a few aspects
    You show a thin plate with quite large deflections. Have you considered the membrane effects that would be revealed by running non-linear geometry?
    You. Do comparisons between different modelling techniques and discuss accuracy. On what basis. Can you make judgement. You need to understand how these relate to reality. I do not see any attempt to generate a comparative independent analysis or test to back up the analysis. We can discuss our thought processes and logic about which we think is better, but this is speculation.
    Increasing the element density nearly always increases the stresses around local discontinuities, therefore you are not actually getting more accurate.
    The thickness discontinuity at the edge of the bosses is very difficult to represent and you need to consider how accurate you need. This is a function of how accurate your loading, your restraint structure, and your requirement. The other aspect that is critical is how the structure is actually supported and how you have represented it.

    • Hi Alan,

      Thank you for your interest in my post. I’m happy to answer your questions.

      Yes, I considered nonlinear effects in preparation of this example. As you can see form the results the maximum displacement is less than 1mm. Which is small comparing to 150mm wide part. Also, I applied sliding (1 DOF) constrain to 3 edges to avoid second order effects. At the same time, the purpose of this post is comparison of meshing techniques, and nonlinear analysis is a separate topic. Anyway, thank you for bringing this question, I will add nonlinear results to the post.
      Agree, if we dive deeper into semantics of word “accuracy”, we must compare the model with real test results. Therefore, it is correct to say that the accuracy here is relative. The reason why I published this topic in the post is that I see many examples when FEA users are not aware of the right modelling practices and get results that are far away from the reality. So, here I’m trying to review only some aspects of meshing techniques to demonstrate the difference in results when using shells or solids.

      I have also seen that the application of FEA varies in different industries. The majority of mechanical engineers and designers are not chasing the same level of accuracy that is required in the aerospace industry. Typically, mechanical engineers have no need or budget to run lots of tests to check and confirm FE modelling assumptions. But in the same time a proper application of FEA demonstrate good correlation with reality and it is much more powerful than hand calculations.
      I agree that in some cases increase in the mesh density can produce uncontrolled grows in stress. Therefore, I deliberately rounded sharp corners in the model to avoid it. So, in my model the maximum stress in growing due to increase in mesh density, but it converges to a stable value.

      Following the Saint-Venant’s principle for this model, it is clear that the Load and Boundary Conditions do not affect results in critical areas.

      Thank you again for your comment.

      Regards, Nik

Leave a Reply

Your email address will not be published.