TAGGED: connections, line-body, multiple, release-moment, spaceclaim
February 4, 2021 at 12:09 pmMickMackSubscriber
Is there a faster way to insert end releases into a model? or a more efficient way to insert multiple releases?
Is it possible to set up the releases in SpaceClaim before i replicate the first module to form the building structure?
I want to create multiple Simple/pinned conditions at nodes (i.e. do not transmit moments) across a large modular steel model and I am wondering if there is a better way to do it than inserting individual end releases as i have done in the image below.
The internal module corners are welded where the beams join the columns at the floor and ceiling, so they transmit moments, however at the point where the above module is connected to the module below it cannot transmit any moment (also shown in 2nd image below).February 4, 2021 at 2:17 pmErik KostsonAnsys EmployeeThe object generator could potentially be used for that .nSo one can put the beams in a named selection, the vertices in another named selection, then create one end release, and finally use the object generator to create all of them in one go (using the first created end release and the named selections).nThis could be a possible way perhaps , so you would need to try and see if it could work.nnFebruary 4, 2021 at 3:33 pmAniketAnsys EmployeeThis automation should be doable using Mechanical scripting, you should also be able to record the script as well using the scripting in the automation tab.nFor more info, please visit:nhttps://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v211/en/act_script/act_script.htmlnhttps://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v211/en/act_cust_mech/act_cust_mech.html n-AniketnHow to access Ansys help linksnGuidelines for Posting on Ansys Learning ForumnFebruary 5, 2021 at 3:46 pmMickMackSubscriberThanks for the responses folks.nnI have reviewed this approach and when i went to get set up to Record the API, I don't appear to have the record button or function as shown below or indeed through the quick launch menu. Have i just missed it or is it possible i don't have this feature to record.nHow would you suggest i proceed?nFebruary 8, 2021 at 5:28 pmAniketAnsys EmployeeAh, ok, sorry about that.n First, close all the Workbench windows. Open a new one.nGo to Workbench> Tools> Options> Appearance> Turn on Beta optionsnThen go to Workbench> Tools> Options> Mechanical> Turn on RecordingnSave this file and then open your file make sure these two options above are enabled, and see if you see the record button.n-AniketnHow to access Ansys help linksnGuidelines for Posting on Ansys Learning ForumnFebruary 9, 2021 at 12:01 pmFebruary 9, 2021 at 12:12 pmErik KostsonAnsys EmployeeThat is great - thank you for your feedback, and hope others might find this useful.nnEriknFebruary 9, 2021 at 12:13 pmMickMackSubscriberThank you for your response, i have now successfully recorded the API as shown in the snippet belownnI am unsure of the best way to automate this procedure, as you can see i have inserted 96 end releases using the Object generator, but this is very labour intensive and my models are only getting bigger.nWhat is the best way to achieve the automation?nThe model is generated by duplicating the first module to create the other 29 modules. Can i set this up in spaceclaim some way to make the process more efficient?nThanks.nFebruary 10, 2021 at 10:44 amAniketAnsys EmployeeI think you should be able to use model assemblyhttps://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v211/en/wb_sim/ds_mech_model_import.htmlnwhere you can set up one model, and repeat it 29 times automatically by specifying options in the Transfer Settings with a number of copies.nOnly manual work will require to set up the first of 30 units of the model (which I am not sure about but can be automated through object generator or ACT) AND connections between subassemblies.nAlso, take a look at Limitations and Restrictions for Model Assembly https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v211/en/wb_sim/ds_mesh_model_limitations.htmlnPlease check if that would help.n-AniketnHow to access Ansys help linksnGuidelines for Posting on Ansys Learning ForumnFebruary 12, 2021 at 2:46 pmMickMackSubscriberThanks for the suggestion, I have spent the past few days reviewing this approach which certainly seems to be the best way of doing it, but i am still having trouble implementing it.nnI created a new geometry in SpaceClaim of a single module for this purpose. I was not sure how to approach this but i categorized everything into 4 separate components.nnFrom the mechanical user guide help documents 'MODEL ASSEMBLY SPECIFICATION', i set out to create model-to-model linking so that i could access the project schematic properties shown below. This did not work for me and i am not sure where i went wrong.nnI created my geometry as a stand alone component and then linked it to the static structural toolbox. Is this the issue because it is geometry-to-geometry and how do i get past it?nnI tried to overcome this my linking another static structural as shown below but i still didn't get the Project schematic properties referred toin the user guide extract abovennAny advice would be greatly appreciated. nFebruary 12, 2021 at 5:03 pmAniketAnsys EmployeeDelete system C in the last imagenDrag and drop another static structural system right side to system B. (NOT on system OR simply double click on Static structural system in Toolboxnnow drag B4 cell to C4 nFebruary 12, 2021 at 7:34 pmMickMackSubscriberThat is excellent thank you very much. nTo achieve the desired configuration i setup two copies, the first in the x direction (C4) and the second in the y direction (D4). nCorrect me if i am wrong but i don't believe the functionality allowed me to copy along both axes, like a linear pattern would, so this is why i completed it in two actions. I have included screenshots below to show the process.nnnnFebruary 12, 2021 at 7:45 pmMickMackSubscriberRegarding the end releases. The point (vertex) which i want to release is the point were the rows of modules are in contact with the row below, so i cannot insert it at an earlier stage, as the connection doesn't exist, until all the modules are in place as shown below.nnThis brings me back to what is the best way to release the 96 connections.nIs there a way to automate using the recorded API?nFebruary 15, 2021 at 5:16 pmMickMackSubscribernI have now realised that the modules are not connected in the horizontal direction, i incorrectly thought that they would generate automatic connections. I believe that this will also affect the model in the vertical direction aswell, Could you advise how to proceed?nShould i revert back to the original model generated with linear pattern in space claim?nHow can i manage and control the connections between the modules and manage the DOF at each connection.nnI look forward to hearing from younnFebruary 18, 2021 at 12:19 pmAniketAnsys EmployeeHey sorry was out. ncontacts between horizontal modules have to be created in system C while the contacts between vertical ones have to be created in the system D.n-AniketnHow to access Ansys help linksnGuidelines for Posting on Ansys Learning ForumnFebruary 19, 2021 at 1:11 pmMickMackSubscriberIs there a way to automate the installation of these connections, which correct me if i am wrong will be inserted as 'joints', using the recorded API as you previously suggested.nnSecondly given this approach seems to bring me to similar difficulties i had originally with inserting releases on 96 number connections, which one do you think is most advantageous to pursue.nnThanks,nnMichaelnMarch 2, 2021 at 10:42 amMickMackSubscriberndid you ever get a chance to review the above? thanksnMarch 2, 2021 at 8:39 pmBenjaminStarlingSubscriberHi Array,nCreate a Named Selection of all vertices where end releases are to be applied. Name it release_nnCreate Worksheet based named selection that selects the elements attached to those nodes (or manually select them). Name it release_enYou can use a command snippet in the environment to apply the endreleases. n/PREP7ncmsel,s,release_n,nodencmsel,s,release_e,elemnendrelease,-1,,ROTX,ROTY,ROTZnallseln/SOLUnThe endrelease command can also do this automatically, without prior selection of elements, but selecting just the elements and nodes you would like to release is good practice, and ensures only those are the ones that are released. nhttps://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v211/en/ans_cmd/Hlp_C_ENDRELEASE.htmlnMarch 2, 2021 at 9:04 pmBenjaminStarlingSubscriberalso just observed more closely your configuration with assembly. There is almost no advantage to building this model with assembly. As you have pointed out, some (many) connections/joints are not applicable until the structure is in its final assembled configuration. I would recommend copying components in Spaceclaim, this patterns the component, any change to bodies in one component, will affect all copies of the component.nReasons to not use assemblynSimple structure, and simple to mesh all at oncenConsistent connected mesh across whole structure, meaning the model only requires one part definition in mechanical.nno need to analyse sub componentsnReasons to use assemblynmany parts (>100) with disconnected meshnmany patterned parts that require connections (or FE objects such as distributed masses) to be patterned with the part - - - (this is what you were hoping to acheive but is not 100% applicable to this structure)ndifferent configurations of assembled parts to be analysed. i.e. assembly coordinates can be parameterised and used in studies, similar to part transform.nMarch 3, 2021 at 8:08 amMickMackSubscriberthe responses which you have provided are excellent, clear and unambigous. I am extremely grateful for you taking the time to help me.nnGiven i am hoping to build a model circa 40 stories i wanted to explore how best to do this with Ansys to have the most efficient and effective processes in place when this time comes, the answers you have provided are invaluable in this regard.nnThanks again.nMichaelnMarch 3, 2021 at 8:35 amBenjaminStarlingSubscriberNot a problem, and thank you for the comprehensive feedback.nLooking at your images more closely I noticed it is always a very short beam that you are referring to. Are these small beams the only locations you would like to apply the end releases to?nIf this is the case, you may want to consider using link elements. This can be done by assigning a duplicate cross section in SpaceClaim, giving it a name such as LINKS, then selecting those bodies in the mechanical tree (they will now be separate bodies upon import due to their different cross section) and setting the Model type the Link/Truss. This may be applicable in this instance as you are releasing all rotational degrees of freedom. If you are only releasing one or two rotations, or translations, then this will obviously not work.nAlso note for link elements, that their cross section definition is actually different in the solver, and the result output is slightly different. The are essentially uniaxial, so if you want the correct transverse stiffnessm I would not utilise this method.nA disdvantage of this method is that you will have many more bodies in the mechanical session, which slows down the application, and requires the user to have to filter through more stuff. An advantage is that this model will solve faster (probably not observable) as the endrelease command in APDL actually creates duplicate nodes and couples which will add to the matrix.nMarch 3, 2021 at 7:16 pmMickMackSubscribernThe model will be used to study the resistance to collapse when a structural element is removed, or in this case an entire module as shown in the image below. The modules are connected at the corners only to transmit the axial load down, this simplifies assembly on site by connecting only the corners and negates any load transfer through the beams, module chasis shown below. There is a gap both horizontally achieved by extending the columns below the floor and vertically by introducing a gap between adjoining modules. In the vertical gap there is a horizontal tie which will tranfer lateral forces to a core or similar and also providing a tieing resistance when the column is removed.nnI won't be releasing all the DOF, certainly in the vertical direction there will be forces being transmitted and there will be some stiffness in X and Z also. As i develop the models i may need to use springs to introduce some stiffness in these, but at the moment i am trying to replicate a previous study and progress from there. The location i am introducing the releases is where one module is in contact on the four corners with the one below, this will not be welded so it is n't fully fixed, but there will be some mechanism to fix this and may include some type of shear key, to aid alignment and resist transverse loads.nnGiven the nature of the structure i had wondered if there was a way to assemble the building similar to Solidworks, but i think the best way to proceed is using pattern in spaceclaim as you suggested and using the lists for the nodes in mechanical, as i can automatically select the columns due to their unique lenght.nnCheersnMichaelnMarch 9, 2021 at 12:39 amBenjaminStarlingSubscribernBased on what you have shown, either end releases or link elements will function just fine, so whatever you have modelled so far should be fine. Are you planning to run this as a transient? or a static analysis?nMarch 10, 2021 at 2:41 pmMickMackSubscriberI am doing both static and transient at the moment, i may have to also look at explicit dynamics later but it will be dependent on my resultsnViewing 23 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.