

June 28, 2020 at 7:54 pmDianeSubscriber
Hello,
My model is a 2D cross section of the upper airway as shown in the image below (constrictors to the left and hard/soft palate to the right).
I am applying a negative pressure normal to the inner walls of the airway, pushing the walls to move towards each other and the airway area to decrease gradually (the model is static). An example of total deformation is shown in the image below.
The objective is to determine the pressure at which the airway collapses which means that I would want to determine the pressure at which the opposite airway walls touch or are very near (distance between walls is smaller than a specified threshold). The contact between the opposite airway walls is frictional, the pressure is ramped and the analysis is split into 15 initial substeps.
I am currently using the contact tool (status) to approximate the time at which the walls touch and then checking to which pressure this time corresponds but it is very rough and doesn't seem correct. Is there a way I can get the exact value of pressure at which the airway walls come into contact for the first time?
Best regards,
Diane

June 28, 2020 at 8:03 pmpeteroznewmanSubscriber
Hello Diane,
Thank you for a clearly explained question. You are doing exactly what I would do to get the answer you seek.
All I would add is that you can change the Initial and Minimum Substeps to 100 (or 1000) to get a very precise value of pressure at first contact. You can click on the graph where it suddenly changes slope, then use the Tabular data to identify the exact time when this happens.
Best regards,
Peter

June 28, 2020 at 8:26 pmDianeSubscriber
Hi Peter,
Thank you for your help and prompt response.
In this case I have a few more questions regarding the contact status tool. What do the values in the graph represent and how are the "near, sliding, sticking" defined? What should I exactly look at to determine the first point of contact? Below is an example of results I previously obtained.
Also, is there a way I can do this in a parametric study where i would be changing the spring stiffness in the model and looking at how it affects collapse pressure? Or I will have to do it manually, one by one?
Regarding the substeps, can I fix the number of substeps or does it always have to be a range with inital, max and min? If it can't be fixed, how can I know the number of substeps that were done after solving for one specific simulation?
Thanks again.
Diane

June 28, 2020 at 10:12 pmpeteroznewmanSubscriber
Hi Diane,
In the Solution Branch where you inserted a Contact Tool, right click on the folder and insert a Gap result. That will plot the gap, I don't know why it shows a gap as a negative number, but you will see that go toward zero as the magnitude of the negative pressure increases. That is a better result to plot.
The number of substeps are just a proxy for how many digit of precision you have in the pressure. With a small number of minimum substeps, you can only get 1 digit of precision on the pressure, with 10 or so minimum substeps, you get 2 digits of precision on the pressure, with 100 or so minimum substeps, you can get 3 digits of precision on the pressure, which is probably enough.
Okay, since you bring in a parametric study into the conversation, now it is more important to automate obtaining the pressure at first contact. In the toolbox is a category called Design Exploration and one of the components in that toolbox is Direct Optimization. It may be possible to create an optimization that searches for the value of pressure that just closes the contact. I will try to figure out how to do that and reply later if I am successful.
Best regards,
Peter

June 29, 2020 at 12:25 ampeteroznewmanSubscriber
Hi Diane,
Now that I opened your model, I find that you have setup the contact definition with "Adjust to Touch". That is wrong. The contact is clearly open at the beginning of the simulation. I changed it back to 0 offset.
I inserted a Contact tool under the Connections folder and evaluated Initial Contact Settings. It showed Far Open. That may be why you added "Adjust to Touch". The corrective action is to edit the Pinball Radius and enter a value of 10 mm. Now the Contact Tool shows Near Open, which is good.
Under Analysis Settings, I made the Minimum Substeps 100.
I see you have pressure applied in three loads. I combined those into a single load and marked the load 1000 Pa as a Parameter.
Under the Solution Tab, I added a Gap and a Penetration result into the Contact Tool. The Maximum values of each of those were added as Parameters.
Here is the Gap plot:
Here is the Penetration Plot:
Manually, we can see that the Time at which first contact is made is 0.32 s which is a pressure of 320 Pa.
In Direct Optimization, I configured a multiobjective optimization to Minimize Penetration and Maximize Gap. I don't know if this will work. I'll reply if I get a useful result.

June 29, 2020 at 10:32 ampeteroznewmanSubscriber
Hi Diane,
I figured out Direct Optimization was not a good approach.
Best regards,
Peter

June 29, 2020 at 3:13 pmDianeSubscriber
Hi Peter,
Thank you very much, your response was extremely helpful!
Just to clarify and check if I am understanding this correctly; after determining the time at which the first contact is made, we get the pressure to which this time corresponds by considering that the pressure is equally divided between the 100 substeps. If this is the case, how can we make sure that the number of substeps is 100 and not more towards the maximum substeps (200 in this case)? Also, when I am increasing the number of substeps in a more complex version of this model the solution doesn't converge anymore. Would you have any advise regarding this?
I have one last question for this model concerning the pressure. Ideally, the model should mimic the upper airway behavior in an animal model where a gradually increasing negative pressure is applied at the lower end of the upper airway. As long as the airway is open, the pressure in uniformly distributed along the walls of the entire airway. However, when the airway closes further increases in the pressure will only be transmitted from the bottom of the airway to the point of collapse and the pressure in the upper segment will not change anymore. Is there a way I can define a pressure that would behave like that in a static structural model without having to add flow?
Best regards,
Diane

June 29, 2020 at 5:26 pmpeteroznewmanSubscriber
Hi Diane,
The pressure is ramped on linearly from 0 to 1 second. If the pressure at time=1 is P, then the pressure at any time t is t*P so you don't care how many steps were needed. The reason to use a minimum number of substeps such as 100 is to avoid big time increments.
There are lots of ways to help a situation where the solver fails to converge. Please reply with more details. Show an image of the NewtonRaphson Force Residual Plot.
A twoway coupled FluidStructure Interaction model would automatically change the pressure after the airway closes.
With a lot of labor, you could manually reproduce a similar effect by breaking the curve up into many segments so the pressure can be controlled along the curve. Arrange the simulation so that the pressure in step 1 is enough to just close the airway, then in step 2, the pressure can continue to drop on one side of the closure while the pressure can increase on the other side of the closure.
Best regards,
Peter
If your questions have been answered, please mark one post with Is Solution to mark this discussion closed. You can open a New Discussion if you have a new question and can reference this discussion for background.

June 29, 2020 at 6:35 pmDianeSubscriber
Hi Peter,
I truly appreciate your help, thank you!
Best regards,
Diane

 You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
Ansys Blog
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.
 Saving & sharing of Working project files in .wbpz format
 Solver Pivot Warning in Beam Element Model
 Understanding Force Convergence Solution Output
 An Unknown error occurred during solution. Check the Solver Output…..
 What is the difference between bonded contact region and fixed joint
 whether have the difference between using contact and target bodies
 User manual
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 Colors and Mesh Display
 material damping and modal analysis

3930

2649

1865

1272

610
© 2023 Copyright ANSYS, Inc. All rights reserved.