SimScale CAE Forum

Session-2 Homework: Bending of an Airfoil Frame



Homework submission

Submitting all three homework assignments will qualify you for a free Professional Training (value of 500€) as well as a certificate of participation.

Homework 2 - Deadline 31.07 12:00pm

Submission form

The base model used in this homework session is provided by Aled J Taylor from GrabCAD


This exercise involves simulating the aircraft wing with applied bending and torsional load due to wind pressure.The task is quite interesting, to setup 6 different configurations with 3 different models and then compare the results. There is one initial model and two optimized ones. The interesting thing would be to see how the deformation and stresses change with each structural optimization of a wing. The possible load configurations with the initial model is shown below.

The structural improvements done to the wing model are shown in the figure below:

The different combinations for performing the simulations are:

Please, note that separate simulation needs to be set up for each configuration


Import the project by clicking the link below. (Ctrl + Click to open in a new tab)

Click to Import the Homework Project


  • In the ‘Mesh Creator’ tab, click on the geometry ‘Wing-with-I-beam’
  • Then, click on ‘New Mesh’ button in the options panel.

  • Select Tetrahedral Automatic mesh and select the following parameters - Second order under the desired mesh order, 3-Moderate for fineness and 8 cores. This operation will automatically create a mesh for the geometry. The cell size and refinement will be adapted automatically.

  • Click on Save button to save all settings.
  • Now click the Start button to begin the mesh operation. The meshing job will start in a few moments and all computation is done via cloud computing.

  • The mesh operation takes about 5 minutes to complete and gives a ‘Finished’ status in the lower left once it is over.

  • Follow same steps to create a mesh for other models.

Simulation Setup

  • For setting up the simulation switch to the Simulation Designer tab and select New simulation.

  • A create new project window will pop-up. Give a project suitable name (optional) e.g. Wings-with-I-beam-bending-load in this case and click Create.

  • Since our load will be static and deformation would be large. select the analysis type Static analysis - advanced under Solid mechanics, change Nonlinear analysis to true and click Save.

  • After saving, the simulation tree now looks as shown below. Here the Tree Entries in Red must be completed.

Domain selection

  • Click ‘Domain’ from the tree and select the mesh created from the previous task. Click the Save button. The mesh will then automatically load in the viewer.

  • Furthermore, change render mode to ‘Surfaces’ on viewer top to interact with the mesh more easily.

Create Topological Entity Sets

  • In this homework we are going to perform 2 different simulations with each model case, as discussed earlier. The image below shows settings for bending and torsional load condition. It is convenient to name these under ‘Topological Entity Sets’ to be used later during the setup.

  • We will create 4 sets in total, as shown below:

  • Click on the tree entry ‘Topological Entity Sets’.


  • To create the first set, click the shown surface and click on the ‘New from selection’ button to create a set named ‘fixation’.

bending load:

  • To create the second set, flip the model upside down and select the shown faces (all lower faces of wing), follow the same procedure above to create a set named ‘bending load’.

lower torsional load:

  • To create the third set, select the shown faces (all lower back half faces of wing), follow the same procedure above to create a set named ‘lower torsional load’. (ignore the warning that pops up, it just tells you that you have selected the faces which are part of some other topological entity set)

upper torsional load:

  • To create the fourth and final set, flip again the wing upside down and select the shown faces (all upper front half faces of wing), follow the same procedure above to create a set named ‘upper torsional load’.

Select Solid Material

  • Now we will define a material for our wing. Normally different Aluminum alloys are used for specific section i.e. ribs, stringers etc. But for simplicity we will assign Al 2024 to the whole material. Select ‘Material’ from the sub-tree and click New.

  • Change:
  • Name to Al 2024 (optional).
  • Young’s Modulus [N/m2] to 73100000000 (defines the stiffness of the material).
  • Poisson’s ratio to 0.33 (defines the relationship between deformation of a material along perpendicular axis).
  • Density [kg/m3] to 2780 (defines the self load of the geometry).
  • Select the volume under Topological Mapping and click Save.

Boundary Conditions

In this section, we will define the constraint (fixation) and load (bending load) for our simulation case.

  • Let’s first define fixation. Select Constraint in the tree and click New.

  • A new boundary condition with default name boundary condition 1 will be created. Rename it to fixation (optional). Under Topological Mapping, change Filter for entity types to face sets and select ‘fixation’. Then click Save.

  • Next up, we will define the boundary condition for bending load. Select Load in the tree and click New.

  • A new boundary condition will be made under Load. Rename it to bending load (optional). Click small f(x) button under Pressure and give this formula 3.75e4*t. Select bending load under Topological Mapping and click Save. (this formula will apply pressure load of 3.75e4 Pa on all lower faces of the wing linearly over time. Time is multiplied since solver can’t automatically ramp the load over time).

Simulation Control

  • Click on Simulation control and change change Initial time step length [s] to 0.25 under details of Timestep definition, Number of computing cores to 16 and Maximum runtime [s] to 7200.

Create New Run
  • Click on Simulation runs and create a new run. Give simulation run a suitable name (optional) e.g. Run-I-beam-bending in this case.

  • The new run will be created under Simulation Runs. Click Start to run the simulation.

Create Further Configurations

  • Once you have started the run with the first configuration setup, go ahead and make a duplicate of this simulation in order to perform torsional load analysis (configuration 2).

  • Rename the simulation to Wings-with-I-beam-torsional-load.

  • All you need to do is to change the pressure load in this case. Click bending load in the tree and rename it to upper torsional load. Change pressure value from 3.75e4*t to 5e4*t, deselect bending load and select upper torsional load under Topological Mapping. Then click Save

  • Next create a lower torsional load by creating a new load under Load, rename it to lower torsional load and give pressure value of 5e4*t (similar as upper torsional load). Select lower torsional load under Topological Mapping and then click Save.

  • Create a new run and click Start.

For all the other configurations with different model meshes, duplicate the already created bending and torsional load simulations, assign the desired mesh to Domain and follow all the above steps in order to setup simulation cases for all the other configurations.


  • Once the simulation is over, click on Post-processor tab to view the results.
  • Select Solution fields of the simulation run you want to view results. In this case, it is Run-I-beam-bending.

  • In order to differentiate between the deformed and undeformed geometry of the wing, make the field (at the top left corner) to Solid color and change the Opacity to 0.3. This will make the wing little transparent.

  • To see the deformed geometry, click on Add Filter and then Warp by Vector. You will see a Warp by Vector filter is added under your solution field and in the result viewer, the deformed wing will appear with the undeformed shape. You can select Toggle color bar to view the magnitude of the von Mises stress (right side of the Delete Filter button).

  • Click on Rescale and select the range from 0 to 5e8.

  • The von Mises stress would be scaled from 0 to 5e8, as shown in the figure below.

  • Click camera icon under Viewport Tools to generate a screenshot. The screenshot will appear under Screenshots section of a Result Evaluation tree item.

Follow the same guide for post processing other configurations and compare the results

Community Digest July 2016
'Aircraft wing design optimization' simulation project by ahmedhussain18



Hello everyone,

Can anyone please tell me what is the maximum displacement coming for the wing tip for configuration 1 (at 3.75e+04*t, at t=1)? In the webinar, it was said as nearby 1.8m. But for me it comes around 1.3m. So if anybody can please tell his value as well?



Hello Abhishek!

It should have to be 1.8 m. Can you please check if your mesh is made via first order or second order elements?

If you have made your mesh with first order then you have redo the case by creating second order mesh. If not, then please paste your project link so I can have a look.



Anybody here who could help me please?

Got this message in solver log after the simulation was aborted:
Run failed. Trying to recover results until last saved time step…-----------------------------------------------------------------------------Result recovery failed.


@hfoester! It might be due to use of higher core machine. Although it should not have to be the case. Can you please try changing just the Number of computing cores to 16 and rerun it. I am pretty sure it will work for you.



Hello @ahmedhussain18

Thank you so much for your reply. The mesh is second order and the link to the project file is “”. It will be really nice if you can take a look. I hope this works.

The following question is not related to the first one:
I also wonder why have we chosen non-linear analysis and then a linear elastic material. We do not define in material properties how the Al 2024 should behave in the plastic region (non-linear domain).
PS: I am not a structural expert.



Thank you very much @ahmedhussain18 . I do not understand why I cannot use more cores but now it works and I can finish the simulation


@averma! what you are getting is absolutely right. The run in the webinar was an old one with the pressure value of 5e4. That needs to be updated. Therefore, displacement for the first case has to be around 1.3 m. You are getting it right no worry! :slight_smile:

We have chosen non-linear analysis because we are having high deformations and nonlinear strains can be tracked via nonlinear solver. For the material you are right we could have used plastic but to make it simpler only elastic is used.



Hi there,
I’m finishing the hw for this session. Is it possible to compare different results from different simulations?
For this case, I would like to compare the results of the 3 simulations.



Hey Luca!

Thanks for the query. Yes you can do so. The comparison wasn’t included in this homework since it’s bit complex to do. Below you can see how to do that.

  1. First open a result. Preferably first model case.
  2. Once it’s loaded apply a WarpByVector filter. Turn off the original solution field filter i.e. one which is transparent in homework.
  3. Next right click on the solution field of the next result that needs to be loaded and then click Add result to viewer. This will load the results in the same viewer.
  4. This time before applying the WarpByVector filter, apply transform filter in order to translate the geometry to see it side by side. Give value of -3 in third box next to Translate and click apply.
  5. Now apply the WarpByVector to this filter. Turn off both previous filters.
  6. Perform above steps 3 to 5 to load the third results. In this case transform it with value of -6 rather than -3.

After following all above steps you will end up with a result tree somewhat like below:

You can click save state to save the state of your results for later use.

The results will look something like this in the viewer:

(These results are for bending load)

I hope this helps. If you have any question/s, feel free to ask.



Hi Ahmed @ahmedhussain18 ,
just done!! thank you, but my max displacement is about 1.4 m and not 1.8 m!!

however thanks :slight_smile:


Hey Luca!

Looks good! :slight_smile:

Sorry for this confusion as already discussed above:

If you change to displacement along x rather than magnitude and rescale it, you will see that the highest value is ~1.3 m for the first model case.



ok, thank you @ahmedhussain18


Just noticed also that, differently from the video workshop session, here I didn’t find mention of the creation of a point of reference for the momentum


@gned! yes it was removed from here since it was making the tutorial bit lengthy. Still I think the point data is not that important as one can have a good idea of displacement already from contour plots.



At the vacation period… I think it’s c :wink:


Hey everybody,

I’ve run into a bit of a problem regarding the boundary conditions: When selecting “fixation” with “face sets” as entity type filter, I get this error message as soon as I’m trying to save this step:

I redid the whole project twice up to this point with the same result :disappointed: Does anybody have a clue what I did wrong or how to counter it? Considering the approaching deadline, any input would be highly appreciated :wink:

My project link:


Hi Pleiades,

Just ignore this Warning message and go on. Click the OK button and continue with your simulation. Don´t worry, it will be fine :wink:

Greetings :slight_smile: