October 21, 2020 at 12:06 pmRameez_ul_HaqSubscriber
Load and BC:October 22, 2020 at 11:23 amAniketAnsys EmployeeAnsys staff can not download files on the student portal, so if you want to reach a larger audience to get answers from, please insert the images inline. (You have done that already)nYes, you should model the plates with gap between them so that those with shell thickness effect will touch each other. Also for high stresses near support try modelling non linear material model.n-AniketnHow to access Ansys help linksnGuidelines for Posting on Ansys Learning ForumnOctober 22, 2020 at 1:43 pmRameez_ul_HaqSubscriberSo this means every time I have to input a frictionless or frictional contact, I always have to input a gap between them in the geometry? And I should also open the shell thickness effect when working with them, otherwise the frictionless or frictional contact will not work?nI actually donot want to model material non-linearity, I want to know if the stresses near those regions are actually quite higher than in the other parts of the structure, in reality (assuming these stresses donot surpass the yield strength of material), or these stresses are occuring due to constraint equations employed for fixed joint in Ansys solver, and may not actually be present in the reality. Or they are happening because of some other reason? Is that a solver error near the fixed joint, or those will happen in the reality as well?nOctober 22, 2020 at 5:47 pmpeteroznewmanSubscriberInsert a Contact Tool under the Connections folder and Evaluate Initial Contact Status. You should always do this anytime you have frictional or frictionless or rough contact.nIf the contact status shows as Open or Far Open, then the parts will pass through each other.nIf the contact status is Closed or Near Open, then the parts will not pass through each other (but will have a tiny amount of penetration).nOctober 22, 2020 at 7:05 pmAniketAnsys EmployeeTo establish contact, it is not absolutely necessary to have the gap, best way to check it at start is to insert a contact tool (https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v201/en/wb_sim/ds_Contact_Tool.html) before solving the model and check status. You can then adjust the offset so that contacts are touching.nIf you are not modelling material nonlinearity, for given increase in the strains beyond elastic limits, stresses will rise a lot, unrealistically. So if your model is bound to show unrealistic stresses in highly strained areas of your model.nnOctober 23, 2020 at 11:23 amRameez_ul_HaqSubscriberThank you for enlightening me about the contact tool.nAnd I also understand what you are trying to convey about the stresses, but I think you didn't exactly undestand my query. It is about the post processing for the stress near the hole (where deformable fixed joint is attached).nPlease observe the following figure, taken from google for stress concentration near the holes.nnNow, have a look at the stress I am getting near the hole, where deformable fixed joint is attached.nRIGHT PLATE:nnLEFT PLATE:nAs it vividly appears that there is a difference between the stress distribution and concentration between the two cases. Now I want to actually know that why is there is a difference between them? Is Ansys producing accurate results, or there is some kind of an error which is expected to be seen near the holes since there are some contraint equations involved on the nodes of these holes due to fixed joint. Is it because of bearing stress? (but there is no bearing load applied on the holes). Is the fixed joint causing any bearing load, since only half of the holes are experiencing these high stresses and the other half is not. Are the stresses artificial because of low quality mesh elements near the holes? How can we judge? n[Assume the yield strength of the material is mush greater than the stresses produced in ANSYS near these fixed joint holes on the plates].nI am actually a fresh engineer trying to make judgements on these stresses.nOctober 25, 2020 at 3:22 ampeteroznewmanSubscriberTwo thick plates that should be stacked on one another are represented as existing on the same plane in your midsurface model below. This is a significant source of error in the model.nThe improperly configured contact elements do not transfer load at the ends of the plates. This generates an erroneously large moment at the joint, which is another major source of error in the model.nFix these errors before you spend any time looking at the stress around the holes.nOctober 26, 2020 at 5:22 pmRameez_ul_HaqSubscriberI re-conducted the analysis for these two geometric environments;nGEOMTERIC CONDITION 1: Distance between the two surfaces is equal to 1 mm (with the thickness of each plate of 2 mm).nnFrictionless contact between them (with no shell thickness effect).nResults:nnnGEOMETRIC CONDITION 2: gap between the plates equal to 2 mm.nnFrictionless contact between them with shell thickness effect 'ON'.nResults:nnnIf we turn on the shell thickness effect, how does it effect my results? Will there be an affect on moment transfer between the two surfaces if shell thickness effect is turned on or off? The only difference I see is this that the target and the contact faces which are given the frictionless contact cannot cross each other, rather with the shell thickness effect on or off, doesn't matter.nSecondly, the contact side of frictionless contact is, in both cases, seen to be highlighted in gray, which says that the status is inactive. What does this mean and why does it happen? Will it affect my solutions?nIn the first geometric condition, the faces are 'NEAR', while for the second geometric condition, the faces are 'SLIDING'. How does the ANSYS decide it is far, near or sliding. How does it make a difference, i mean in the numerical calculations and the results? What does 'Number Contacting' and 'Real Constant' mean?nLastly, as you have already mentioned that if the frictionless contact works, then the forces and moments transfer occuring in the joints will be less. This is proven by the above study and shown in the figures. However, again the highly stressed area for the second geometric condition is on one side of the holes, on both the plates. This confuses me. I want to post process these results to know if it is actually going to happen in the reality or this is just a numerical glitch happening due to constraint equations applied on these holes.nI would be grateful to you if you can also briefly explain why would a big distance between the surfaces which are connected using a fixed joint, can cause a big moment transfer between them? nThank you.nnOctober 29, 2020 at 12:01 pmpeteroznewmanSubscribernI like that you ask detailed questions. I don't like it if the post is too long. I will answer questions more quickly if the post is shorter. nGEOMTERIC CONDITION 1: You should have left this out of the post. In some ways, it is more wrong that the original post with the two sheets on the same plane. This is halfway interfering which is still wrong. I have no other comments on this.nGEOMTERIC CONDITION 2: This is the correct spacing, and as you found, contact works with the shell thickness on.nDESIGN DISCUSSION: If I had to design a joint to connect two parts like this with two bolts, I would have a longer overlap and space the bolts along that overlap, not across the width. If I could use four bolts, they would be across the width and along the overlap.nNUTS AND BOLTS: The physical system has a nut and bolt. Torque on the nut and bolt creates tension in the bolt shank, which clamps the two plates together. The clamping forces are orders of magnitude larger than the forces and moments passing through this joint due to the 100 N applied load. Also, there is a washer under the nut and bolt that spreads the clamping force over a large area under the bolt head and nut.nSIMULATION DISCUSSION: Before you build a model, you have to decide what to idealize and how much simplification to do. Those decisions depend on what is important to capture in the results. nIf the area of interest is in some other location far from the joint, then the model only needs to transmit the forces and moments through the joint. Two fixed Joints do this. So would Bonded Contact of the overlap. In this case, don't look at the stress in the joint, because the joint has been idealized to such an extent as to make the stress around the holes to be irrelevant.nIf the area of interest is the nuts/bolts/holes, then don't use fixed Joints in the model. Include the nuts and bolts and use bolt pretension to clamp the overlapped pieces together. The stress pattern in the plates will be very different once the clamping force is included.nBENDING MOMENT DIAGRAM: This is simple to draw for a straight cantilever beam such as you have. The small bend at the end of your model could be left off since the force is perpendicular to the length of the beam. Draw a bending moment diagram for this model. At the point where the hole centers are, calculate the bending moment. That is what the fixed Joints have to transmit and they do so by applying forces and moments to the edges of the holes. Please reply with the bending moment diagram for this cantilevered beam problem.nOctober 29, 2020 at 2:33 pmRameez_ul_HaqSubscriberThank you answering. You mentioned this statement, ''The stress pattern in the plates will be very different once the clamping force is included''. You mean only in the vicinity of the bolt/nut and pre-tension right? Not in the all of the plates, right? When we apply a pre-tension, is the applied boundary conditions also supposed to resist these pre loads on the bolts? Since you have also pointed out that there are washers, in reality, to spread out the pre applied tension, should we model washers too with the nut and bolt inside ANSYS to analyze the spreading this pre tension, or application of only the pretension inside ANSYS with only nut and bolt is going to be enough? Like if an analysis is desired to check the region of the nut/bolt properly like it will fail or not or how the stresses are distributed in that region.nThe bending moment graph is given below for this problem.nOctober 30, 2020 at 7:40 amRameez_ul_HaqSubscriber, there is one more thing which baffles me.nSince the extreme left side of the right plate is moving upside, and this has a frictionless contact with the left plate, so this means the right plate is transferring a force (and maybe a moment) to the left plate in the +Z direction. And for the joints, they are transferring the forces and moments in the other direction. How can you say that having a frictionless contact between these two plates will actually decrease the amount of transfer of forces and moments in the fixed joints? nThe region you see, marked in black, below i think will have a local bending moment. nnAt the same time, the region on the left plate which is experiencing the upward force due to frictionless contact, is seen to be overall deforming in -Z direction. What is your opinion on this?November 4, 2020 at 5:22 pmRameez_ul_HaqSubscriberArray, waiting for your reply nNovember 17, 2020 at 11:24 amRameez_ul_HaqSubscriber,still waiting for your thoughts on this one.nNovember 23, 2020 at 2:57 ampeteroznewmanSubscribernBelow is an idealized example to help you think about this problem. It consists of two overlapped sheets, spanning a 100 mm total cantilever length. Instead of a bolt, I have used a spherical joint shown as the vertical red line on the right. The left plate has a fixed support at the left end. The red vertical line on the left can be considered the frictional contact, but is implemented as a joint. There is a 10 mm overhang between the spherical joint on the right and the joint on the left representing contact of the bottom plate to press against the top plate.nI applied a -1 N force in the Y direction at the right end of the plate so the reaction force at the fixed end on the left is +1 N in the Y direction.nBut the forces in the joints are much higher. The tension in the joint on the right is 6 N while the contact force at the tip of the overhang is 5 N.nIf the 10 mm overhang was reduced, the forces would go much higher. Imagine the distance is reduced to the diameter of a bolt head and there is no overhang. Then the forces would get very large indeed.nViewing 13 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
- 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.
- 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.
Please Login to Report Topic
Please Login to Share Feed