September 5, 2020 at 12:29 pmOguzhanASubscriber
I have a buckling analysis about cylinder. I analyzed it using stabilization setting. But my result isn't what I want. Theoretically , Cylinder behavior curve should be negative slope(figure-1). But in My result ,curve is positive slope(figure-2) . Critical Buckling Load can be true,but i think behavior is failed.September 7, 2020 at 4:57 pmAshish KhemkaAnsys EmployeeHi,nnPlease refer the following steps for buckling analysis:nnnnRegards,nAshish KhemkanSeptember 8, 2020 at 7:47 amOguzhanASubscriberThank you but this does not contain the answer to my question.nSeptember 10, 2020 at 4:48 amAshish KhemkaAnsys EmployeennWhat I meant to indicate is that you might need to perform a post-buckling analysis if you have already crossed the first point (pt. A) on the force deflection curve. To have a force deflection curve with negative slope you may try prescribing displacement boundary condition rather than force to have a stabilized solution. The reaction force on displacement b.c. can be used to generate the load-deflection curve then.nnRegards,nAshish KhemkanSeptember 10, 2020 at 9:48 amOguzhanASubscriberThank you how can I use displacement for cylinder face ?nRegardsnSeptember 10, 2020 at 7:30 pmpeteroznewmanSubscriberYou can use Stabilization with a Pressure Load.nOctober 6, 2020 at 11:11 amAshish KhemkaAnsys EmployeennDid the suggestions above help you?.Regards,nAshish KhemkanOctober 7, 2020 at 4:56 pmOguzhanASubscriberI just got strain line with stabilization. Because I dont know how can I apply displacement instead of pressure. Do you have an idea? nRegardsnOguzhannOctober 8, 2020 at 4:01 pmAshish KhemkaAnsys EmployeennYou can apply the diplacement and track the force reaction to generate the force deflection curve.nnRegards,nAshish KhemkanOctober 15, 2020 at 5:11 pmOguzhanASubscriberhow can I apply displacement for cylinder face ?nRegardsnNovember 3, 2020 at 3:25 amBenjaminStarlingSubscriberHi OguzhanA,nThe answer you are looking for is the ARCLEN command.nIssue ARCLEN,ON in a static structural environment command snippet if you are in the mechanical application. Using the default settings of the command is advised and works for most cases.nThere is a related comman, ARCTRM, but you should not need to utilise this command.nFor your analysis, I believe you will need nonlinear geometry active, NLGEOM command, I am not sure if the ARCLEN command automatically turns this on or if you will have to do this separately.nNovember 3, 2020 at 6:24 pmOguzhanASubscriberNovember 9, 2020 at 9:23 pmBenjaminStarlingSubscriberIf you aren't seeing a negative curve there may be other issues with the model or the specific example. However, using the arc length method is the only way to get a negative slope on the force deflection curve. Stabilisation will not acheive this for you. I will look into the example you have provided and get back to you.nNovember 9, 2020 at 9:52 pmOguzhanASubscriberThank you, I'm waiting for your answer. nRegardsnOguzhannNovember 10, 2020 at 3:16 amBenjaminStarlingSubscriberHi Oghuzan,nI have acheived steady convergence through the negative curve of the force-deflection curve, this is shown below by the negative time increment, however I will be stopping the analysis here as disk space and time are an issue for me at the moment. Whether this analysis ultimately shows what the theory says it should, I am not sure. nTo acheive this I made the following changes to the test case you described.nfine mesh - I used 10 mm as the global size, this is pretty fine, but I found that it was critical to acheive convergence. If possible go for somewhere between 5 and 10 mm.nI utilised a small magnitude point force to introduce the assymmetry, rather than utilising the egeinvalue buckling shape. Both methods should work, but I think the buckled shape is still too symmetric in some instances. I had issues getting the solve to behave utilising the eigenvalue buckling deformed shape.nAnalsyis settings below. 10,000 maximum substeps is required. For some reason this problem is very sensitive along the negative curve. This may explain why you were getting non-convergence issues before. If you have the resources, and time is no issue for you, I would possibly even set this to 100,000. Other settings you can't see in the image below are left as default. Under Output Controls, take a look at 'Store Results At' to limit the overall size of your result file, as you will not need results through such fine time steps. You may also want to have nodal forces on in the output, this will nI have a command snippet that has ARCLEN,ON and NEQIT,100 in it. The NEQIT isn't really required but was left there from when I was troubleshooting.nnimage below of my point load to introduce assymetrynnI am using 2020R2, so you may see differences if you are using a different version, or the academic version.nMy final comment is to persist with using arclen, I have seen that you have been asking this question for a while now and have been led to use stabilisation. Stabilisation cannot model the negative curve at all, and the arc length method is 100% required.nIf I have time later on I may pick this up again and solve to completion.nNovember 10, 2020 at 4:17 pmOguzhanASubscriberHello Array thank you for answer. I will try this settings now.But I have only two questions.n1-How much pressure load did you apply?n2-For arclen command, just write arclen,on or arclen,on,max,minnRegards,nOguzhaNovember 16, 2020 at 12:01 amBenjaminStarlingSubscriberHi Oguzhan,I solved this to near completion. I ended up with non convergence at around 0.92, after reaching 0.97. The point load ended up causing further assymetry, final result shown below. The max deformation is occuring where I have applied the point load. This may not be the result you are seeking, so I would probably return to using the buckled shape.nn1 - I applied 0.02 MPa.n2 - I used arclen,on. however based on the non convergence you may need to play around with theMINARCvalue to get through to convergence.nnFor my own understanding, is it expected that this structure ever becomes stable again? if it is not, the solve will never reach convergence, however you can still plot the force deflection curve for part of the buckling process. nnnNovember 23, 2020 at 2:18 pmNovember 23, 2020 at 10:51 pmBenjaminStarlingSubscriberHi OghuzannWhat units is that graph in? is that for the same case you have provided for me to model?nTo me it appears that the structure isn't really stable, even towards the end of the loading history, this is evident in the orange curve where the gradient is consistently changing (and going backwards in terms of deflection). Also not sure what is going on with the yellow curve. the grey curve in particulary would indicate that you need an extremely small value for the MINARC value, and very small time steps, to achieve such a sharp change in gradient. The blue curve would be the most ideal to recreate, as it has smooth changes in gradient which would not require a really small value of MINARC to capture.nThat being said, I think we are expereincing non convergence before we are even close to the second change in stiffness behaviour. I will have time this weekend to investigate further. It may just be that further reductions are required in time step sizes.nDo you have any papers/references to this type of analysis or any theory that you can share with me such that I can get a better understanding of what we may be missing?nNovember 25, 2020 at 10:12 amOguzhanASubscriberOf course, I started this work because of an article. I can share the article with you. There are experimental studies and there is another program, abaqus program solution, but only for the part up to the initial torsional load. I am sharing the article link and abaqus solution link with you. But in the experimental data, we noticed that the pressure values in the article are 10 times bigger. There was probably a mistake.n" target="blank">nRegardsnOguzhannNovember 30, 2020 at 8:32 amBenjaminStarlingSubscriberHi Oghuzan,nI watched that video you linked, and found it contains everything you need to proceed with this analysis. Below are all my thoughts in no particular order.nAbaqus default shell has 5 integration points comapred to APDL 3. This can be changed using the SECDATA command, however I do not think this is consequential to your analysis.nThe method of restraining one node in direction normal to the cylinder is a clever way of introducing assymetry, for the GNA case, and I would recommend you use this method or at least try it.nDr. Wagner is not solving to completion, the fact that we are getting non-convergence is inconsequential as far as I can tell. He is specifying 300 increments to be solved maximum and ending the analysis at that point, or, the solve is ending when it reaches non-convergence (it appears to end at 224 steps). There is no need to specify this limit in Ansys, as I don't think comparing the number of substeps/iterations between solvers is anywhere close to 1:1. Some solvers are better/faster at some analysis types. He has probably determined this value from his experience with Abaqus.nDr. Wagner is using 1e-50 for the MINARC value, I would recommend you use the same value. It may not translate between solvers to be the same variable, but in either instance, it is an incredibly small value.nDr. Wagner plots pressure vs. arc-length as a result. To plot something similar, you will need nodal forces -> on, in your output controls. You may also need something else turned on to get pressure??? possibly keyopt(10)=1? but if you check the link below at table 181.1, you can see that pressure is an available output in the result file. To get the arc length you can get this value in the solver output, which can be found under solution information (shown in the image below). I don't know if there is a more direct way to get this value, or whether Ansys stores this as a variable. You will also need to filter the arc-length based on whether the iteration actually converges, as these are the only points that will have results.nThe final issue is the total displacement (GNA case). In the video 9 mm is acheived. The greatest displacement I have acheived so far is ~6 mm. I believe setting the MINARC value as I mentioned above will help the solve get further before non convergence. He acheives far greater displacement with the GNIA case, however we don't have much to compare with this case without having a similar imperfection introduced to the structure.nnnDecember 17, 2020 at 12:15 pmVenugopalbSubscriber
Hi Oghuzan,I have acheived steady convergence through the negative curve of the force-deflection curve, this is shown below by the negative time increment, however I will be stopping the analysis here as disk space and time are an issue for me at the moment. Whether this analysis ultimately shows what the theory says it should, I am not sure. https://us.v-cdn.net/6032193/uploads/PEQJQPBBF7ZO/image.pngTo acheive this I made the following changes to the test case you described.fine mesh - I used 10 mm as the global size, this is pretty fine, but I found that it was critical to acheive convergence. If possible go for somewhere between 5 and 10 mm.I utilised a small magnitude point force to introduce the assymmetry, rather than utilising the egeinvalue buckling shape. Both methods should work, but I think the buckled shape is still too symmetric in some instances. I had issues getting the solve to behave utilising the eigenvalue buckling deformed shape.Analsyis settings below. 10,000 maximum substeps is required. For some reason this problem is very sensitive along the negative curve. This may explain why you were getting non-convergence issues before. If you have the resources, and time is no issue for you, I would possibly even set this to 100,000. Other settings you can't see in the image below are left as default. Under Output Controls, take a look at 'Store Results At' to limit the overall size of your result file, as you will not need results through such fine time steps. You may also want to have nodal forces on in the output, this will I have a command snippet that has ARCLEN,ON and NEQIT,100 in it. The NEQIT isn't really required but was left there from when I was troubleshooting.https://us.v-cdn.net/6032193/uploads/0IBCP4BQF3U8/image.pngimage below of my point load to introduce assymetryhttps://us.v-cdn.net/6032193/uploads/FWTGYUMYLUOP/image.pngI am using 2020R2, so you may see differences if you are using a different version, or the academic version.My final comment is to persist with using arclen, I have seen that you have been asking this question for a while now and have been led to use stabilisation. Stabilisation cannot model the negative curve at all, and the arc length method is 100% required.If I have time later on I may pick this up again and solve to completion.https://forum.ansys.com/discussion/comment/96761#Comment_96761Hello BenjaminStarling,nThank you for your knowledge sharing. It was wonderful........nmy question is why we need to create asymmetry in the cylindrical shell to do buckling analysis? I think the intention is to create imperfection. nWhat would happen if the imperfection is not present in the cylinder for nonlinear buckling analysis?nThanking younregardsnvenugopalbnDecember 17, 2020 at 11:07 pmBenjaminStarlingSubscriberHi Venugopalb,nThe assymetry is required to allow the buckling to initialise. If you imagine a perfect cylindrical structure, with a perfectly symmetric load, the load is symmetrically reacted by it self, and the stiffness of the structure (to wherever the structure is restrained).nA good example is to consider an axisymmetric analysis, and whether this could capture the buckling. (it can not)nObviously in reality this is not an issue as no structure is perfect in any dimension. But more importantly the load is never perfectly symmetric. Even in pressure vessels, there are variations in pressure, particularly when the vessel starts to deform, the pressure local to the deformation will respond accordingly. Compare this with the FEA, where the load is as a specific value across the structure, and any change in the structure does not affect this.nViewing 22 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?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.