September 16, 2020 at 10:50 amJasminSubscriber
I'm solving 2D axis-symmetric problem when I apply required differential pressure on inside and outside surface. I get error solver unable to converge nonlinear problem. Due to elements getting distorted at contact region which I found from newton Raphon residual force. I have tried with finer mesh and changing contact parameter. If anyone with some suggestion will be really helpful.September 16, 2020 at 5:21 pmpeteroznewmanSubscriberIt will be much easier to give a helpful suggestion if you show an image of the geometry.nSeptember 17, 2020 at 12:39 pmJasminSubscriberI want to compress the C shape structure between 2 plates in LS1 and apply temperature and differential pressure in LS2. In order to ramp load I have created 5 steps as there was convergence issue. I'm doing this in Ansys workbench. Also I was trying to set convergence criteria as mesh so that remeshing will be done to get to convergence but I was not able to do that setting.nnSeptember 18, 2020 at 12:01 pmSeptember 19, 2020 at 6:50 pmJasminSubscriberNo C shaped component is metal. I have been doing entire model in static structural in workbench and applied thermal condition by setting reference temperature of component as 'by body' which is uniform. I will try making the horizontal plane of symmetry. In error file it says too much penetration of contact element into target and also some element are getting highly distorted near contact region. Main problem arises when differential pressure load is applied on inside and outside surface of C at that point only convergence issue is coming. If you see force convergence image it's the step5 where full differential pressure load is applied solver is unable to converge.nSeptember 20, 2020 at 12:49 ampeteroznewmanSubscriberConvergence issues are often helped by taking many Initial or Minimum substeps under the Analysis Settings.nSeptember 23, 2020 at 7:08 amSeptember 23, 2020 at 3:54 pmpeteroznewmanSubscriberThe solution may be helped by softening the contact. Under the Contact Details, there is a line called Normal Contact Stiffness. Change that from Program Controlled to Factor and change the Factor from 1 to 0.1 or 0.001 and see if that helps.nAnother suggestion is the remove the sharp corner where contact is made and put a small blend radius on that corner. That way you can have many small elements around the contact point.nnSeptember 24, 2020 at 1:38 pmJasminSubscriberThanks alot for all the suggestion. Solution got converged!nOctober 26, 2020 at 6:38 amJasminSubscriberHi nWhen I ran my full Simulation I got the result with some warning and no error. In result I have equivalent stress (Von mises stress) around 3 times more than Yield and Ulimate strength but still there is no fracture seen in the model. How do I get to know the model I created in transient structural is correct.nOctober 26, 2020 at 12:00 pmpeteroznewmanSubscribernPlease read this discussion and come back with any follow up questions.nhttps://forum.ansys.com/discussion/1373/i-want-to-see-the-failure/p1nNovember 25, 2020 at 6:21 amJasminSubscriberHi PeternI have gone through the attached link. I got the point explained.nnNovember 25, 2020 at 6:34 amJasminSubscriberI have doubt when I tried to create model in the static structural I was not able to get the converge solution I used to get error solver was unable to converge the nonlinear problem . When I shifted to Transient Structural module I got the Converged solution even though my problem was static. Is it because the Transient Structural uses Full newton Raphson Method? like how do we decide the Static or Transient module to be used. Can you please give some tips/ example.nNovember 25, 2020 at 5:42 pmpeteroznewmanSubscribernOne type of problem that is difficult to solve with Static Structural analysis that is easier to solve in Transient Structural (or Explicit Dynamics) is snap-through behavior. This occurs when a structure buckles into a new shape. It is difficult for the Static solver to increment the load gradually and remain in static equilibrium to get to the buckled state. But a Transient solver can solve the dynamic equilibrium by including the inertial forces that arise from accelerating the mass to snap-through to the buckled state.nSo the key difference is what type of equilibrium is the solver trying to converge on, static equilibrium or dynamic equilibrium.nNovember 26, 2020 at 10:34 amJasminSubscriberThanks for Explanation. nNovember 26, 2020 at 11:24 amJasminSubscriberCan you please suggest what and all condition can lead to sudden drop in contact pressure as seen in attached image in 3rd step. In 3rd step differential pressure is applied on the C component between the plate. I have been changing the numerical damping value in Analysis setting to check Impact load issue while differential pressure is applied. Also tried by varying stabilization damping factor in contact controls it didn't help much.nNovember 26, 2020 at 4:14 pmpeteroznewmanSubscriberNumerical damping stabilizes the numerical integration scheme by damping out the unwanted high frequency modes. You should not need to change this value. You need Structural Damping. Structural damping refers to physical damping present in the system. For more information, see Damping in the Structural Analysis Guide. nThe contact pressure could make a sudden reduction if the deformation in the C changes from one node in contact at the tip to several nodes in contact on the side.nDecember 2, 2020 at 6:15 amJasminSubscriberThanks for the explanation.nDecember 2, 2020 at 6:27 amJasminSubscriberIn 2D Axisymmetric analysis I'm not able to define rigid-deformable contact. In geometry when I try to define stiffness behavior as flexible to C and rigid to the 2 side plates. It does'nt take. So I'm able to define only deformable-deformable contact with flexible stiffness behavior. Is there any other way to change the contact definition.nnDecember 6, 2020 at 2:28 ampeteroznewmanSubscribernYou can't define the Stiffness Behavior of the body to be Rigid in a 2D Axisymmetric model.nBut you can pick that face/body, and assign a Displacement BC to both X and Y coordinates, which makes the body behave like a rigid body.nDecember 6, 2020 at 2:32 ampeteroznewmanSubscribernDecember 7, 2020 at 5:26 amJasminSubscriberThanks , Peter!nI have done the same as you have described. Can you please explain reason why the stiffness behavior can't be rigid/ any source from where I can get information, and how can I define the rigid-flexible contact in my model is there any other way?nDecember 8, 2020 at 5:23 amJasminSubscriberThanks Peter!nI have done the same as you explain to define the body rigid. Can you please explain the reason why stiffness behavior can't be define/ any source from where I can understand the reason. Is there any other way to define the rigid-deformable contact in 2D Axisymmetric model?nDecember 9, 2020 at 1:56 ampeteroznewmanSubscribernI don't know why you can't have a body in an axisymmetric analysis be rigid for use in contact. As I suggested, if you put all the nodes of a body in a Displacement BC that sets both X and Y, that is the same as being rigid.nDecember 10, 2020 at 6:23 amJasminSubscriberYes I have done the same as you suggested. nThank you.nDecember 10, 2020 at 6:32 amJasminSubscriberI have one doubt, In Plane stress/ strain analysis I want to define revolute joint, but I see that no joint is applicable for 2D analysis. Is there any specific reason for the this. How can we define joints for plane stress/strain case.nDecember 10, 2020 at 5:12 pmpeteroznewmanSubscribernIn an axisymmetric model, a revolute joint doesn't make sense.nIn a Plane Stress/Strain 2D analysis, you can get the effect of a revolute joint to ground by fixing a vertex in X and Y, which leaves rotation about Z free. That puts a lot of stress on that vertex. If you use a Remote Displacement, you can spread the stress over the length of one or more edges, and set X and Y to 0 while leaving rotation about Z free.nJoints in Mechanical are an easy-to-use GUI that creates MPC APDL code behind the front end. I don't know why they are turned off in 2D models. Read the ANSYS Help system to learn how to construct a revolute joint using APDL code and if there are any limitations for 2D analysis.nDecember 17, 2020 at 10:09 amJasminSubscriberThanks Peter.nRemote displacement thing worked.nDecember 28, 2020 at 9:37 amJasminSubscriberHi Peter,nThe C component is sliding out of plate when 95% of simulation is done. Initial contact condition is closed. The previous discussed Boundary condition got solved in new BC I'm facing sliding issue. nnnDecember 28, 2020 at 9:49 amJasminSubscriberDecember 28, 2020 at 1:09 pmpeteroznewmanSubscribernThere is not enough information to provide guidance.nPlease attach the .wbpz Project Archive file so I can take a look.nnDecember 30, 2020 at 10:25 amJasminSubscribernDecember 30, 2020 at 2:23 pmpeteroznewmanSubscribernWhat version of ANSYS are you using?nWhy are you using Transient? Why not Static Structural?nYour material includes a Norton Creep model but your simulation time is 3 seconds. Is it important to model creep in this simulation? If so, the creep constants do not have any temperature dependency. Young's Modulus does have temperature dependency and the thermal condition is quite severe.nHave you considered using Symmetry? Do you expect a symmetric solution?nDecember 30, 2020 at 6:06 pmpeteroznewmanSubscriberHere is the results up to 1.9 out of the 3 load steps when solving as a statics problem. You can see how, at the end, the frictional interface and the two point contact makes for an unstable stick-slip motion.nIf you imposed a symmetry condition, that would make it easier to converge.nDecember 31, 2020 at 5:27 amJasminSubscriberThanks Peter.nI'm using Ansys 16.2 version.nI have tried static structural with other model it was not converging. So I shifted to Transient and got converged solution.nBut in this model there is sliding issue. nModeling creep is not important here.nI expect symmetric solution.nnDecember 31, 2020 at 6:24 pmpeteroznewmanSubscribernOkay, delete Norton from the material model. Slice the ring in half and impose a Y = 0 constraint on that cut boundary to create the symmetry condition. Now you only need one plate to push on the ring.nJanuary 7, 2021 at 11:11 amJasminSubscriberThanks Peter.nI have tried symmetry condition it worked out. nViewing 36 reply threads
Ansys Innovation Space
- 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.Trending discussions
- How to calculate the residual stress on a coating by Vickers indentation?
- Solver Pivot Warning in Beam Element Model
- Errors – Reinforced Concrete Beam
- An Unknown error occurred during solution. Check the Solver Output…..
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Saving & sharing of Working project files in .wbpz format
- Colors and Mesh Display
Top Rated Tags