Learning Forum

[alvincsl]

Hi all, I am trying to perform static structural analysis of an assembled wing under certain speed. I ran a CFX fluent to obtain the pressure distribution on the wing and transfer it to the static structural which I need to obtain the performance of the assembled structure. But it seems like the solver couldn't converge and I'm lost. I don't know what I did wrong and don't really know where to look for solution. The whole idea is to perform topology optimization on the wing rib but now I couldn't obtain the performance of the un-optimized structure.

Really appreciate if someone can point me a direction on what I did wrong. 

PS: I couldn't upload the wbpz file so I shared the google drive link. The file name is student community.wbpz

https://drive.google.com/file/d/18PxtYXDAIzd12LM9ToJF3cjaHxtATuX6/view?usp=sharing

 

[SaiD]

Hi,

Due to company policies Ansys employees cannot download any attachments. Could you use the "Insert Image" option to insert a few images that show the geometry and the boundary conditions applied?

What error message(s) do you get? Is there any contact in your model?

 

Sai

[alvincsl]

Hi, I have reduced the size of the project and attached in this post. Thank you so much. 

 

Alvin

 

[Wenlong]

Hi Alvinscl,

As Sai mentioned, Ansys employees are not permitted to download any attachment, either from this website or other links. So to get a wider help it will be nice to insert some screenshots of your model setup, such as the imported pressure, geometry, boundary conditions, unfinished results, and error messages. 

Thanks,

Regards,

Wenlong

 

[alvincsl]

Hi, apologise for not reading carefully. My analysis is currently running but the force doesn't seem to converge. 

Here's my geometry. I created a midsurface on my wing skin as well as the ribs (leading edge, mid, and trailing edge). As for the spar, I couldn't create a beam structure due to the tapered profile so I assigned it as solid. The others are shell elements. 

I applied the imported load from CFX fluent into static structural module and applied on the wing skin. The fixed supports are on the surface of the spar as well as the edge of the wing skin).

For the contact region, I've checked them and there are contact regions over the structure. The analysis is still running so I'm couldn't get the solver output messages yet. I'm not sure if I'm doing in the right direction and if the analysis is going to solve my geometry, so wish to have a discussion. 

[alvincsl]

Sorry for the long message, here'e the output message I got from the unconverged analysis. The analysis stopped at iteration 84 and it took 14 hours. 

Below are the output message. 

 

[Wenlong]

Hi alvincsl,

Thank you for the detailed response. 

It looks like you haven't assigned any substeps yet and it is trying to solve the problem with 1 substep initially. Please do this: in the analysis settings, change the time stepping to "auto", and define initial substep=50, minimum substep=20, max substep=200. Turn on the large deflection. 

Since this is a really large model, I would encourage you to start simple. For example, you can start using a very coarse mesh and suppress the imported pressure from CFX, but instead just give it a very small pressure through the "pressure" boundary condition. After your model converges, you can gradually bring in the complexities.

I am curious how the different geometry parts are connected? Are they through bonded contact or through geometry topology (which means they share common nodes).

Regards,

Wenlong

 

[alvincsl]

Hi Wenlong, thanks for your reply. 

I didn't connect them through geometry topology, they are connected through bonded contact. Is there any difference between that? My next step is to perform topology optimization on the wing ribs, and since you've mentioned about the connection, should I connect them through merged geometry topology in SpaceClaim? 

Regards, 

Alvin

[alvincsl]

I tried to assign the substeps as you mentioned but the result doesn't seem to converge. 

Here's the error messages I received: 

1. The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information. 

2. The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose. 

I wonder if that's the problem with the contact? If I set the geometry to shared topology, is it going to be better? I aimed to obtain the deflection of the geometry only. 

 

Regards, 

Alvin

[Wenlong]

Hi Alvin, 

Thanks for the reply. Both approaches (geometry shared-topology and bonded contact) should work. 

Can you please try this? Suppress all the shells, and only leave the solid ribs, run the simulation. If it works, add back some shells and run it again. The reason I'd like to do this is to isolate and find out what's causing the issue. 

Regards,

Wenlong

 

[alvincsl]

Hi Wenlong, 

I did the steps you mentioned. I applied a upward force at the bottom surface (on the bottom of solid spar and the wing skin) 

Here's the result on the solid spar with all shell elements (ribs and skin) suppressed. 

But when I unsuppressed the wing skin and apply the same force, but this time from the bottom surface of the skin. The pressure seem to only distribute across the skin and no pressure distribution on the wing spar. I thought the pressure will be distributed and transferred from the skin onto the spars and ribs but it's not. The pressure distribution on the ribs will be useful for the topology optimization of the ribs. 

Regards, 

Alvin

 

[Wenlong]

Hi Alvin,

It means the shell wing and the solid ribs are not properly connected. Check your bonded contact and you can increase the pinball radius to make sure they are bonded together. To achieve that, you can right click on connections --> insert --> Contact tool --> Initial information, if you run the initial information analysis, it will output the status of your contact and the gap between two parts, you can adjust your pinball radius based on that. 

Regards,

Wenlong

 

[alvincsl]

Hi Wen Long,

Thank you for your suggestion. I re-ran the analysis and the result still show no pressure distribution across the solid ribs. 

Here'e the initial contact region result I did before running the analysis. 

I did not assign any contact sizing between the geometry. Is it becuase of that? 

Regards, 

Alvin 

[Wenlong]

Hi Alvin,

So the contact is working fine. From the legend of the contour plot, you can see the maximum value is around 1mm, which means the ribs are deforming. It probably just deforms too little compared to the surface, so that it is hard to visualize from the plot. You can play with these three options to highlight the deformation and show the max deformation location. 

FYI, you probably don't need that small mesh, especially at the debugging stage. 

Regards,

Wenlong

 

[alvincsl]

Hi Wenlong, 

 

Thanks. I rerun the simulation with a bigger mesh but simulation stopped without an accurate results. I couldn't insert images at this time so I'd just describe it. The "Total Deformation" result and "Equivalent Stress" at the Solution have a red lightning symbol beside it. The force convergence worksheet showed no converging on the force. I ran the simulation with the shell ribs suppressed, leaving only the solid spar and shell skin active. The force is acting on the lower surface of the wing skin shell. I ran with only the solid spar and pressure acting from below, everything works fine. So I think it's on the skin but I don't know where is the error. I tried to read through the solver output but I couldn't find any problem. 

Here's the error messages I received. 

1. The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose. 

This message shown before and I've checked my contact region on the solid spar and the wing skin. Both of the contacts are closed. 

2. Althought the solution failed to solve completely at all time points, partial results at some points have been able to be solved. Refer to Troubleshooting in the Help System for more details. 

3. The solution failed to solve completely at all time points. Restart points are available to continue the analysis. 

4. The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information. 

5. The solution was executed using restart information. 

 

Regards, 

Alvin

[Wenlong]

Hi Alvin,

If the force is too big or the shell is too slender (without ribs supporting it), it is likely the shell will have nonlinear buckling and run into convergence difficulties. In this case, you can go to -> Analysis settings ->Nonlinear Controls -> Stabilization, change it to energy-based, and set the ratio as 0.01. 

FYI, (this is regarding your previous post about spar plot), when you do a displacement or stress plot of the spar, it is better if you can scope only to the spar geometry instead of "all bodies", because the shell deformation is dominant and as a result, the contour plot on the spar will be all blue. 

Regards,

Wenlong

 

[alvincsl]

Hi Wenlong, 

On the energy-based, is it constant or reduced? 

Regards, 

Alvin

[Wenlong]

Constant should be good. 

[alvincsl]

Hi Wenlong, 

I've set the stabilization to energy method as taught, then tried the with small pressure acting on the entire geometry (unsuppressed all) and everything works fine. The analysis completed successfully. But when I switch over with the imported load from CFX, the same error occurs. All 4 error messages are same as what I mentioned before. But I can see the pressure distributed across the targeted mid ribs. 

Do you t's because of the geometry? My trailing edge is pointed and maybe it is the reason that causes unconverging issue? 

Regards, 

Alvin

 

[Wenlong]

Hi Alvin,

Good to know your model is working on the artificial pressure. It means now the model is ready. I don't think the trailing edge is a problem because as you can see from the Newton-Raphson Residual plot, the value there is almost 0. 

I would try to increase the energy dissipation ratio in the stabilization and find out the smallest value that makes the model converge (The smaller the dissipation value is, the more accurate the simulation is). You can later insert a stabilization energy plot and compare it with the strain energy plot, if the stabilization energy is much smaller than the strain energy (say 5%), then you will be fine. 

Regards,

Wenlong

 

[alvincsl]

Hi Wenlong, 

Sorry I left out another image on the Newton-Raphson Residual plot. Image below was from the bottom-up view of the geometry. 

Since you've mentioned that, I went to check the plot again and it only shows at the tip of the trailing edge at the wing tip, other trailing edges are fine from what I observed. Image below was the top-down view of the geometry. 

Regards, 

Alvin

[alvincsl]

Hi WenLong, 

My analysis ran till the end (1s) yesterday. Here's the result. The mesh on the wing skin is coarse and the energy dissipation ratio used was 1 and the also included the normal stiffness factor of 0.8. But the stress distribution across the mid ribs are not very clear, and I think this is not converged either. 

Here's another simulation with the stress distribution on the mid ribs. Energy dissipation ratio was 0.05 and the normal stiffness factor is 1, the simulation stopped at 2.875e-2 s. But the stress distribution across the mid ribs are much clearer. 

My question is that does the Newton-Raphson Residual Force the problem that causes convergence difficulties and causes the simulation to stop halfway. If yes, do I decrease the normal stiffness ratio? If I decrease it, seems like the pressure distribution across the mid ribs are not defined. But I think I should decrease the normal stiffness ratio since I've got the analysis ran until 1s yesterday. 

The problem now is that I couldn't get the analysis run until 1s, it always stopped halfway. Even if it finish running, the stress distribution is not clear across my targeted geometry. 

 

Regards, 

Alvin