November 10, 2018 at 5:03 amasahaSubscriber
Can anyone please help me in a transient structural analysis. I am constantly getting a distortion error though I have done several times of mesh refinement.. My problem is related to ball valve friction between ball and seat ring.
November 12, 2018 at 8:36 pm
November 13, 2018 at 4:04 amasahaSubscriber
Thank you, Sir, for your kind approach.
Here I have attached the image. The left one is seat ring and the right one is a ball. The material of the ball is stainless steel and the seat ring is Teflon. The ball is rotating with respect to its centre and a pressure is acting on the seat ring in the positive y-direction.
November 13, 2018 at 1:34 pmpeteroznewmanSubscriber
Maybe you didn't know this, but you don't need Transient Structural to rotate a ball on a seat-ring, you can do the same motion in Static Structural, but a lot more easily. (I know, the word Static implies no motion, but that isn't true!).
Let's say you have a Revolute Joint Connection between the ball center and ground and you have a Joint Load that has a Displacement rotation of 90 degrees.
You have Frictional Contact between the seat-ring and the ball. Perhaps you want to plot the Torque to turn the ball 90 degrees.
The seat-ring needs more constraints than just Pressure, because if that is all there was, then it would just turn with the ball!
Add a Compression Only support to the cylidrical face of the seat-ring. That will stop it turning with the ball, but allow the pressure to push it against the ball.
In Static Structural, the default end time for the simulation is 1 seconds. That is when the ball will reach 90 degrees.
Under Analysis Settings, specify Initial Substeps as 100, Minimum Substeps as 30 and Maximum Substeps as 500.
November 13, 2018 at 3:00 pmasahaSubscriber
Many many thanks for giving your valuable time.
I have tried with static structural but I haven't given any constraints to the seat ring. For that may be the error was coming which you have correctly pointed out. I will try again with this modifications.
Another thing is that I want to plot the temperature with respect to rotational acceleration which is generated due to frictional contact. For that, I may have to further incorporate UDF which I haven't done yet. Because I am not getting that much confidence to go forward till the primary model gets solved.
Assistance from you will be a great help to me.
November 13, 2018 at 4:05 pmpeteroznewmanSubscriber
An important setting to mention under Analysis Settings.
Large Deflection must be On.
November 14, 2018 at 12:48 pmasahaSubscriber
I am very much thankful to you for your help.
I have tried as per your guidance. If the ramped pressure is applied to the seat ring and at the same time if the rotation is given as the value of angle (i.e. 90 degree) then a solution is coming.
But when I give a velocity or acceleration as an input inspite of the rotational angle, ANSYS is showing an error ''One or more joint conditions feature settings that are incompatible with the current analysis''. Also when I am giving a constant pressure throughout the rotational time, then also Ansys is showing an error ''The solver engine was unable to converge on a solution for the non linear problem as constrained''.
Can you please help me in this regard..!
November 14, 2018 at 9:33 pmpeteroznewmanSubscriber
In a Static Structural model, the Joint load is a Displacement. Though there is something called Time, it just represents progress from 0 to 1. You would not use Velocity or Acceleration on a Joint in a Static Structural model.
There are many reasons why a Static Structural model will fail to converge. I will provide some links to other Discussions that describe how to overcome convergence difficulties.
November 16, 2018 at 5:42 amasahaSubscriber
I am trying as per your suggestions. Though it has not converged yet, I am trying with every possibility.
But my question is, If I want to change the rotational speed or acceleration, what should I do in static structural..!
2nd thing is that while I am trying to give pressure input in step, one column in the tabular input is showing the time. Which is showing 2 sec But my step end time is 1 sec. Ansys is also not permitting me to give time as 0.5 sec and 1 sec. Can you please discuss the fallacy lies here... Is it time per step..! So when the step no is 2, it implies the time of rotation is 2 sec.. !!
November 16, 2018 at 4:18 pmSandeep MedikondaAnsys Employee
You will have to change it in the details of the analysis settings.
November 16, 2018 at 4:43 pm
November 16, 2018 at 5:53 pmSandeep MedikondaAnsys Employee
Are you trying to change the end time at which you are applying the load for a particular step? If so, you can select the current step number and change the end time. So, let's say you only want Step 1 to end at time 0.5 sec. Just change the Step End Time.
November 17, 2018 at 4:24 amasahaSubscriber
Thank You very much, Sir.
November 18, 2018 at 1:35 pm
November 18, 2018 at 3:37 pmSandeep MedikondaAnsys Employee
These are the recommendations from the manual for this error:
When Advanced Contact is NOT Present in the Model ...
Check for sufficient supports to prevent rigid body motion (structural) or check for thermal material curves or convection curves which rise and/or fall sharply over the temperature range (thermal).
If you encounter a convergence error during a thermal analysis that is using contact, consider modifying the Thermal Conductance property.
When Advanced Contact IS Present in the Model ...
Check for sufficient supports to prevent rigid body motion or that contact with other parts will prevent rigid motion.
Check that the loading is of a reasonable nature. Unlike linear problems whose results will scale linearly with the loading, advanced contact is nonlinear and convergence problems may arise if the loading is too big or small in a real world setting.
If the contact type is frictionless, try setting the type to rough. This may help some problems to converge if any possible sliding is not constrained.
Check that the mesh is sufficiently fine on faces that may be in contact. Too coarse a mesh may cause inaccurate answers and convergence difficulties.
Consider softening the normal contact stiffness KN to a value of .1. The default value is 1 and may be changed by setting the Normal Stiffness. Smaller KN multipliers will allow more contact penetration which may cause inaccuracies but may allow problems to converge that would not otherwise.
If symmetric contact is being used (by default the contact is symmetric), consider using asymmetric contact pairs. This may help problems that experience oscillating convergence patterns due to contact chattering. The program can be directed to automatically use asymmetric contact in the Details view of the Contact Folder.
If that doesn't help. Look at the newton-residuals, See here.
November 19, 2018 at 3:58 amasahaSubscriber
Thank You, Sir.
I want to know, when I am applying a frictional coefficient, is it acting throughout the full rotation irrespective of the pressure which is applied at the seat ring or not.
December 2, 2019 at 2:56 amalextgarnerSubscriber
Can joint velocity/acceleration not be applied in a static structural analysis?
December 2, 2019 at 4:21 ampeteroznewmanSubscriber
It cannot. If you have other questions, please open a New Discussion.
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.