July 12, 2020 at 4:16 amferrossiSubscriber
My simulation is failing and I can't understand why.
I am getting these errors from the ANSYS Mechanical Solution information:
This error is mentioning issues like "Contact pair is inactive", but all my contacts are shown. I am not understanding what it means.
Also, it says "Max. Penetration of -1.1545747E-04 has been detected between contact element 19914 and target element 19240".
But my mesh is only 14,169 elements (see screenshot below), so I don't understand why the Solution Information would reference elements 19914 and 19240 which are not even part of the mesh?
I am not able to do any troubleshooting here since I am not even able to visualize the problem elements.
Note: I only get this simulation fail when I create a finer mesh, which is also weird, because I would expect it to fail when the mesh is coarser.
I am very confused, is anyone able to help me figure out what is going on?
July 12, 2020 at 2:45 pmpeteroznewmanSubscriber
The Mesh Statistics are only for structural elements on the bodies that were meshed in Mechanical. The model includes contact, but the contact elements are added after you click the Solve button in the solver. That is why they have element IDs larger than the number of elements shown in Statistics.
There are many reasons a model can fail to converge. There are two plots you need to look at to diagnose what to do to resolve this problem. Click on the Solution Information folder and in the Details window, there is a row called Number of Newton-Raphson Residual Plots. The default is 0, type in a 3, then Solve.
When the solver fails to converge, under the Solution Information folder, there are now three plots. These are the Newton-Raphson Force Residual plots. They show the size of the force residual on each element. There is pass/fail criterion value on the Force Residual, and the solver has to keep iterating until it gets all the elements below the criterion. The corrective action is often to make smaller or better shaped elements in the area around this maximum N-R Force Residual location.
The other plot to look at is also under the Solution Information folder, it is the Force Residual Convergence plot. It shows the plot of the maximum value of the N-R Force Residual at each iteration. Please reply with those two plots.
July 12, 2020 at 7:22 pmferrossiSubscriber
Thank you for your support.
Together with the info you requested, see below screenshots of my model so that you can get an idea of how it is supposed to work:
*** Model Overview with Boundary Conditions: ***
*** Model Intended results: *** (this is how the model is supposed to work. I get these results only with a coarse mesh, but simulation fails with finer mesh).
*** Newton-Raphson Residual Force (plot 1) ***
*** Newton-Raphson Residual Force (plot 2) ***
*** Newton-Raphson Residual Force (plot 3) ***
*** Force Convergence Plot ***
Also, see below a new screenshot of one of the Newton-Raphson plots. This time, the top and bottom surfaces have been hidden, so you can clearly see the residual force values at the contact body (contact between top surface (target body, hidden) and triangular end cap (contact body, shown)).
NOTE: the contact type between the triangular end cap and the top surface is Bonded.
July 12, 2020 at 10:06 pmpeteroznewmanSubscriber
The last plot has shown you where the solver fails to converge. The corrective action is usually to make smaller and better shaped elements. However, this model has the additional complication of having bonded contact. That may be the cause of this issue. You need to zoom in to the Max area until you can see individual elements and determine how the contact is affecting them. In this case, it makes sense that a coarse elements might work with bonded contact better than small elements. Please show some zoomed in images or attach your project archive and let me take a closer look.
Another idea is to set the Bonded Contact Formulation to MPC so that you can see the Contact Elements after the solver has run.
July 12, 2020 at 10:31 pmferrossiSubscriber
See the archive file attached to this reply.
1) The top and bottom surfaces are currently hidden. To unhide them, you can find them under Geometry > Wing > Skin > Bot Wing Skin & Top Wing Skin.
2) The mesh is currently set at 7mm for all the assemblies in the model. I noticed that this is fine enough for the model to fail. If you set the mesh size at 8mm or 9mm, it will produce results without failing.
currently, as you can see in my model, the end cap where I am having the contact issue is a 3D body. However, every other assembly is a shell element surface. I was thinking to turn the end cap into a Beam element (this way the elements can be really high Quality and easer to handle compared to a 3D body).
However, after I turn the end cap into a Beam element, I am no longer able to connect it to the mid surface (in the middle of my assembly). For some reason the contact tool will not accept a contact of the type "surface edge to beam edge". See screenshot below.
What are your thoughts on this last point?
July 13, 2020 at 2:58 ampeteroznewmanSubscriber
I don't know about Edge to Edge bonded contact. Does surface to edge work?
Another idea is to change the End Cap Stiffness Behavior from Flexible to Rigid. ANSYS does not permit a mixture of those two types in the same component so the End Cap has to be put in one component while the surface bodies are in the other component. Unfortunately when I did this, all the Bonded Contacts broke.
I don't know if it will work, but it is another approach.
July 15, 2020 at 2:23 amferrossiSubscriber
I was able to model the End Cap with beam elements and connect the End Cap beam to the mid surface, top surface, and bottom surface.
I used a series of edge to edge contacts (this time it worked).
This way, the simulation starts running, but then it fails (this is already an improvement compared to before, where I ran a simulation with beam elements, but it failed right at the start). See below one of the Newton-Raphson plots and the unconverged Force plot.
I tried to change the beam's behavior to "Rigid", but still no luck, it failed again.
Do you have any other suggestions?
Also, the picture above is taken at the last moment of the deflection (when the trailing edge is deflected downward). It looks like the top and bottom surface are penetrating the beam. I was not experiencing this penetration with solid elements. Is this an actual issue with the simulation or it's just the rendering?
Also, when I use beam elements like in this case, it looks like the end cap remains straight (no angular deflection) while on the other hand it should point at and angle during the downward motion of the trailing edge. I suspect that since the end cap is not at an angle something must be wrong (maybe the contacts between End Cap and Top and Bottom Surfaces are not working properly).
July 17, 2020 at 1:00 ampeteroznewmanSubscriber
I have seen rendering errors in Mechanical when using Rigid Bodies.
I can tell from the graphs that the solver is trying (but failing) to accommodate the entire load in one step. Under Analysis Settings, change Auto Time Stepping to On. The set the Initial Substeps to 100, the Minimum Substeps to 10 and the Maximum Substeps to 1000.
July 27, 2020 at 12:43 amferrossiSubscriber
After following your suggestion (together with some geometry changes to the model) I was able to get the simulation to converge. Thank you for the hint!
However, now that it converged, I want to better understand what I was doing wrong, so that I have a complete understand of what I am doing.
See below the questions I have, I hope you can respond (or redirect me to other sources) so that I can clear out my doubts.
Question 1: I didn't understand your statement "I can tell from the graphs that the solver is trying (but failing) to accommodate the entire load in one step". How do you tell this is the case by looking at the Force Convergence chart?
Question 2: For what concerns the simulation results, what is the difference between "accommodating the entire load in one step" versus using substeps as you suggested? I am not familiar with the concepts that you asked me to apply (initial substeps, min substeps, max substeps). Do you have an explanation or some material that I can read to better understand the effects of using substeps in a simulation?
Question 3: The simulation converged when the values of the two forces applied to the model was +100 and -100 N. Then, I tested the same model with greater forces (200 N, 250 N, 300 N, and 400 N). See below the stress results for each simulation:
100 N --> 247 MPa (converged) 200 N --> 548 MPa (converged) 250 N --> 740 MPa (converged) 300 N --> 958 MPA (partial results, NOT converged) 400 N --> 927 MPA (partial results, NOT converged) (mesh is finer than previous meshes, so maybe this is why it's slightly lower than 300 N).
As you can see, as the force increases, the stress becomes greater (makes sense). Please consider that the material I am using is a Carbon Fiber which fails at 513 MPa (in tension) and -437 MPa (in compression). Therefore, you can see how the results for 200 N and 250 N would cause the material to fail already. My question concerns the reason why the 300 N and 400 N simulations do not converge: is it because the stress is so much above the failure limit of the material, or is it because my mesh is not fine enough (good elements quality)? I am trying to understand if the non-convergence is due to unrealistic loads (out of my control), or to the mesh which is not good enough (which would be equal to saying: ANSYS will always give a results, even if the value is extreme and clearly beyond the failure limit of the material). See here a picture of the 400 N results:
Question 4: I am not understanding how to interpret the Force Convergence chart and the Newton Raphson plots. See for example the chart and plot for the unconverged solution at 400 N force.
What does the Y axis represent? are those the errors (residuals) calculated by the solver when solving the equations? I fear they might be something else though, since the force convergence chart reaches values of 34,062.00 N (which is incredibly high) so I find it hard to believe that this is a residual error. And what does the X axis represent? It would be great if you can share some material where I can read about it.
What about the Newton Raphson plots below? The are showing units of force (N) applied to the trailing edge cap. I understand that that they are indicating some kind of error, but I can't understand why they would indicate 38 N on the trailing edge. What do these plots mean physically?
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.