January 25, 2021 at 1:53 pmMickMackSubscriber
I have two beams in close proximity, 0.1m gap. The red beam represents the ceiling (top) beam in a steel modular unit and the yellow beam represents the floor (bottom) beam, which also carries a 100mm thick concrete slab represented by the surface.January 25, 2021 at 7:33 pmMickMackSubscriberPlease note that i have found the help section in relation to 'Surface Body Shell Offsets'.nnTo elaborate further on my original query i include the following sketch of what i want to achieve. The line in blue at the bottom is the Ansys beam elementnnFrom the explanation on the user define paramater for a shell, the centreline of the concrete slab is represented by the beam element therefore the membrane offset must be 350mm.nnI am assuming that for the PFC300 the beam element will represent the centroid of the PFC. As it is symmetrical in the y-y direction, this will be half of its height, therefore the offset must be +150mm for the floor beam and -150mm for the ceiling beam.nnPlease provide confirmation if this is correct and also if this is the best approach.nJanuary 26, 2021 at 10:37 amMickMackSubscriberHinI have noticed a further problem when i am offsetting beams, it appears that when i am offset a set of beams, the ceiling beams in the screenshot below, nn6 of the beams move in the downward y direction (red arrow) while 2 move in the positive y-direction (purple arrow), shown in the 2nd screenshot below. nnAny idea why this is happening, and also am i approaching this correctly as per previous commentsncould you offer any advice?nJanuary 26, 2021 at 3:37 pmMickMackSubscriberHinI have tried to resolve the issue with the beams in Spaceclaim. As can be seen in the first snippet the beams are indeed intersecting each other so i have simply moved them using the orientation command in space claim, as shown in the 2nd snippet.nnWhen i bring these into mechanical to mesh i could not see any gap between them, and when i meshed them individually it can be seen that they are still intersecting. Can anyone offer some advice regarding this and the above?nnJanuary 26, 2021 at 3:49 pmJanuary 28, 2021 at 11:13 amMickMackSubscriberCan anyone help me with this issue, as i am now having further problems as i try to carry out an explicit dynamics analysis. In the explicit analysis the program does not recognise the surface offset i have used.nnI think all these issues may be interrelated.nnThanksnJanuary 29, 2021 at 9:57 amMickMackSubscriberHi,nIs this thread active?nOr do i need to create a new one?.Could someone please advise thank you.nJanuary 29, 2021 at 10:01 amAshish KhemkaAnsys EmployeennThe thread is active. Please wait for someone with relevant expertise to respond.nnRegards,nAshish KhemkanJanuary 29, 2021 at 10:54 amMickMackSubscriberThanks very much.nJanuary 29, 2021 at 11:44 ampeteroznewmanSubscribernWhat is the purpose of the model, what answers do you need it to give you?nIt is much simpler if the beam and floor shell elements use the same nodes around the edge of the floor. That way, they are bonded together. Is that acceptable? Or do you require the floor to slide relative to the beam? That is more complicated.nJanuary 29, 2021 at 3:56 pmMickMackSubscriberI am working towards using the models to examine the progressive collapse resistance of a modular building. I thought i had set the beams and floors up so that they would share nodes using a rectangle in spaceclaim, i didn't realise i had changed this as i was working through the problem.Regarding Function, The function of the floor will be to act as a rigid diaphragm and transfer the floor loads into the beam, no movement is required. The beams will simply transfer the loads to the columns. The floor will be cast on top of the PFC beams in reality and the beams will then be welded to the columns. This is a simplified configuration i am using without secondary beams etc.nnUnusually compared to traditional steel frames the configuration has beams within 100mm of each other ( bottom of floor beam of upper module and top of ceiling beam of lower module).I simply want to model this accurately to reflect the above. When i reassessed what i had done originally i considered that the beams may have been intesecting and meshing each other together and then i proceeded to rectify this, whether i was correct or not i don not know, but the simulated model below (with the alterations i documented above) certainly has a better appearance. The problem is that there appears to be deformation in the top beam but that should not be the case as there is still a gap between the two beams and no force being applied to the top beam.nnI hope that i have been able to convey this issue appropriately.nnThanksnnJanuary 30, 2021 at 1:30 pmpeteroznewmanSubscribernThe problem is that there appears to be deformation in the top beam but that should not be the case as there is still a gap between the two beams and no force being applied to the top beam.nNot true. Gravity is acting on all the mass, so the Top (ceiling) beam has deformation due to its self weight, even if the Bottom (floor) beam above it still has a gap.nJanuary 30, 2021 at 3:06 pmMickMackSubscribernThe ceiling beam of the bottom module is the same ceiling beam in the top module. If it was the self weight both beams should be displaying identical deformation. The other ceiling beams in the model would also be the same, hence why i have made this assessment. nI may have missed something but that was the rationale.nnWas i correct to assume originally (at the top of this post) there was an issue with the beam elements overlapping? ndue to there section size? nJanuary 30, 2021 at 6:52 pmpeteroznewmanSubscribernThe ceiling beam of the bottom module is the same ceiling beam in the top module.nNot true. If the ceiling beams and floor beams are all welded to vertical columns, the difference between the lower ceiling beam and the upper ceiling beam is that lower ceiling beam is attached to the vertical column very near to the attachment of a floor beam just 0.1 m above it, which is carrying the extra weight of the concrete floor. The extra weight causes local deformation in the vertical column which adds some bending to the nearby ceiling beam. The upper ceiling beam doesn't have extra deformation of the column.nIf the beams were not welded, but on joints that decoupled column rotation from beam rotation, then you would see less difference between the upper and lower ceiling beams.nJanuary 31, 2021 at 2:25 pmMickMackSubscriberHi Array ,nThanks for that, i had totally forgotten the model was fixed and as you correctly pointed out the deformation in the ceiling beam is induced by the column which has caused hogging of the beam. I have verified this from the max strain results shown below.nnJanuary 31, 2021 at 2:43 pmpeteroznewmanSubscribernHi Michael,nUnfortunately, you will need a different model for Explicit Dynamics, which as you found out, does not support shell offsets.nOften, Structural Analysts will make a Trade-Study model to quickly evaluate different sizes of beam cross-sections or shell thicknesses. In this model, no offsets are used with the understanding that the results are not accurate. Once the optimum cross-section and thickness values have been found, an accurate model with the correct offsets is built to get final results.nJanuary 31, 2021 at 4:41 pmMickMackSubscriberThat's perfect thanks, i would have spent ages trying to get the explicit dynamics model to work if you hadn't pointed this out.nnI don't believe that i will need to change beams but i wanted to ensure that i was creating the model in the most effective manner, before i started getting more ambitious with the size and scale of the structure.nRegarding the beams and surfaces, can i conclude that the way i have modelled them (with offsets) is the correct way to do so for the transient and static analysis's?January 31, 2021 at 7:48 pmpeteroznewmanSubscribernYes, using offsets is a standard practice to build structural models.nFebruary 2, 2021 at 9:55 amMickMackSubscribernThanks very much for your help.nnRegarding the explicit dynamics analysis not supporting shell off sets, i could establish the line element at the slab centre and simply off set the beams down from this.nI am just wondering if i did this would it be okay and if there were any other differences that i would need to consider?nOr should i just create a separate stand alone model for the explicit dynamaics?nFebruary 2, 2021 at 7:28 pmpeteroznewmanSubscribernFor Explicit Dynamics, you can have a line body meshed at the centerline of the beam and above that, a surface body at the midsurface of the concrete, To represent the fact that these are bonded together, you can have Bonded Contact to connect the beam nodes to the nodes along the edges of the surface. I don't recall what the limitations are for bonded contact in Explicit Dynamics. I would set the type to MPC, but there may be limitations.nFebruary 4, 2021 at 10:29 amMickMackSubscriberThanks for your help.nViewing 20 reply threads
Ansys Innovation Space
- 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.
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
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- 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
- User manual
- 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
- material damping and modal analysis
- Colors and Mesh Display
Top Rated Tags
© 2023 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.