Learning Forum

[Harish_s]

Braid analysis.mp4

[peteroznewman]

nUse Frictional Contact between the braids and the rubber tube.nInsert a Contact Tool under the Connections folder. Generate Initial Contact Status. Reply with an image of that table.nDoes that contact show as Near Open or Far Open?nIf it is Far Open, you need to increase the Pinball Radius.n

[Harish_s]

Dear Sir,nThank you very much for your valuable advice.nI modified the pinball radius and checked the initial contact status. All the contacts were in 'closed' condition.nI ran the simulation with pressure load, I can see the interaction now. The photos and videos, I have attached with this comment.nIn my practical problem, the braid structure consists of 36 fibres. But, when I tried to simulate it, the computation time was very high, took nearly two full days to complete 25% of the simulation. So, I stopped the simulation. nThen, I reduced the number of fibres to 4 and got the above result. nSince my Workbench archive file is more than 100MB, I am sharing my drive folder with you, having the workbench file(.wbpz format). Kindly give your suggestions to reduce my computation time by changing the mesh controls and other settings.nGoogle drive location: https://drive.google.com/file/d/1__Ipz5_3h2CzPQg-ZSevQj0Hz7-13blA/view?usp=sharingn

[Harish_s]

Sir, I need one more favour. I want to simulate the inflation of rubber tube by passing air inside. I have to create rubber tube model and air volume model separately and perform system coupling on the assembly. Can you please suggest some steps or study links to perform system coupling of this. n

[peteroznewman]

nI tried your google drive but you have moved the file to the trash so I could not download it.nSome suggestions to speed up computation time.nUse Beam elements for the braidnUse Shell element for the tubenYou can use a Pressure load to inflate the rubber tube, there is no need to model the air.nn

[Harish_s]

Sorry Sir. I mistakenly moved it to trash.nNow I have restored it. please find the attached link given below:nThanks for your suggestions. I will try and give you feedback as soon as possible.n

[Harish_s]

Sir,nKindly give me some reference materials to study how the beam and shell elements are made in meshing. I have no knowledge on this.n

[Harish_s]

Dear Sir,nI first tried analysing my braid structure, by applied force from the bottom surface, to see the deformation. It came out to be successful. So, I think I have no problem with the braid model. I will attach the picture below:nPlease note that, I developed the solid model of braid in SOLIDWORKS and I combined all the individual bodies of braid fibres as one single model.n

[Harish_s]

Hello Sir. Kindly advice me on the problem. I still find no way to come out.n

[peteroznewman]

nI tried your Google Drive link above, but you have not set it to allow anyone to download it. I was going to look at your model this morning but I can't.nIn SpaceClaim, you can select the outside face of your tube solid and type Ctrl-C and Ctrl-V to copy/paste the face and create a surface. There is a similar capability in SolidWorks to extract the face of a solid.nTo create Beam elements you need a 3D curve at the center of the braid. You don't want a solid body. SpaceClaim can only convert solids to beam elements if they are perfectly extruded solids.nn

[Harish_s]

Thanks for your suggestion.nBut, I could not create the 3D curve of braid in SpaceClaim or Design modeller.n

[Harish_s]

nDear Sir,nIn SOLIDWORKS, I created the mid surface for each braid. Then, I created a surface cylinder for the rubber tube.nThen, I uploaded the model in ANSYS Static structural. I added thickness to braid surfaces as 0.2mm (symmetric) and cylindrical rubber surface as 0.5mm.nI checked the contact status and all the contacts, including frictional contact between tube and braid, are in closed condition.nWhen I applied pressure on the inner surface of the rubber tube, the simulation is ending abruptly saying that the solution is not converging at a particular time instant.nKindly help me by telling a way out of this problem. If you can spare your time, kindly create a Braid and rubber assembly and lend me a sample ANSYS simulation file.nI am uploading the rubber tube and braid models separately with this comment. Kindly perform assembly of both solids. nIn the case of a rubber tube, the top and bottom ends are fixed to a rigid support, while, in the case of braid, the top end is fixed to a rigid support and the bottom end is free along the direction of the cylinder axis. Then, apply pressure inside the rubber tube so that it touches the braid surface and brings contraction in the overall length of the system. nI referred to an article on FEA of Pneumatic braided actuator, similar to my work. I am attaching that article below. nIn that, the author has used LS-Dyna for simulation. Kindly give your view on this.nThanks for your extended support.n

[peteroznewman]

nPlease review the model in this discussion. /forum/discussion/10032/contact-step-control/p1nIt uses Beam elements to represent a coil wound around a hub to create a friction clutch. Beam elements for your braids and shell element for your rubber tube will give you the best chance of convergence with large deformations in a Static Structural model, but you may still struggle to achieve convergence.nThis model has a lot of contact, and that is where software like LS-DYNA or Explicit Dynamics has a very robust contact algorithm. You may find it beneficial to move over to that solver on this project.nI looked at your Braid assy solid files.rar, but as the filename suggests, there are only solid files. You need 3D curves to make beam elements. I have work to do this weekend, so I will not be able to do more that offer advice.nGood luck.n

[Harish_s]

Thanks for your support, Sir. I will try and give you feedback.n

[Harish_s]

nSir, I am finding it difficult to import a 3D sketch to SpaceClaim and I don't know how to create the 3D structure of braid in SpaceClaim. n

[peteroznewman]

nTry IGES formatn

[Harish_s]

n

[Harish_s]

nThanks for your suggestion.nI will explain the steps followed:nI created the intersection curve between the two surfaces and fitted the spline as a single sketch. nThen, created a plane to sweep the circular crosssection through the 3D spline sketch nThen, I converted the solid model to IGES format (as recommended by you).nThen I imported in SpaceClaim geometry for beam extraction.nnBut, when I tried to extract beams, the operation failed. nThis is my core problem.nAnd I could not create that 3D sketch in Spaceclaim due to limitations in the software, like, there is no option for creating the intersection curve.nKindly give your suggestion.n

[peteroznewman]

nI read the paper you kindly provided. They used Beam elements and Shell elements. That means you need curves and surfaces. STOP MAKING SOLIDS!nYou have Sketch4, the Path. Don't sweep a profile. Export just Sketch4 as an IGES file. Import that into SpaceClaim. In SpaceClaim, define a Circular Beam Profile and edit the profile to assign the correct radius for the braid. This is one of the tricky aspects of using SpaceClaim. Watch a YouTube video on how to do that. Use that Beam Profile and create beams using the imported path curves.nSpaceClaim can create an edge at the intersection of two surfaces. Create a cylinder and plane surface, then use Project to create the edge curve you see in the image. Use the Select tool to select that edge, then Ctrl-C and Ctrl-V to copy the edge and paste it as a Curve. If the export/import of Sketch4 fails for some reason, you can create the 3D curve from the surfaces in SpaceClaim.n

[peteroznewman]

I took the edge of one of the surfaces in the IGES file and used that as a curve.nn

[Harish_s]

Thanks for our detailed answer. I will try this method and give you feedback.n

[Harish_s]

[peteroznewman]

nEdit the beam profile and show the radius you entered for the braid.nWhen you create the beam, you must pick the curve, don't pick points.nYou can set the filter so it only picks edges.n

[Harish_s]

nSir,nThank you so much. I successfully created a beam profile.nI will perform the simulation and give you feedback.nn

[Harish_s]

Sir,nI created shell elements for rubber tube in Spaceclaim and imported in Static structural module. Then, I applied 'pipe pressure' load. I got the desired result. Video is shown below.nI created beam elements for braid model. Two separate models were created, one with single strand and other with 3 strands. I tested both the models in 'Static structural' module by applying external force from the bottom end. I got the desired result.nThen, I included rubber tube in the braid model and applied the same 'pipe pressure' load. Element type chosen were 'Beam' for braid and 'pipe' for rubber tube. n Frictional contact was created between the rubber tube and braid with pinball radius 7.2mm; type: 'adjust to touch'; small sliding:'OFF'. When the contact status was checked, all the contacts were in 'closed' condition.nBut, when i ran the simulation, the solver stopped due to 'non-convergence' of solution at a particular load step. Kindly give your suggestions to solve this problem.nI am attaching the gdrive link for the archieve file:nPlz note: I checked the gdrive link. you can surely download the file. n

[Harish_s]

nDear Sir,nKindly give suggestions on the previous comments. Sorry, I have not tagged you.n

[peteroznewman]

nDon't use Adjust to Touch. Show what the Initial Contact Status is with that turned off. What is the Gap?n

[Harish_s]

nSir,nThe gap is about 1.5mm aprrox on diameter.nI couldn't understand your point regarding in your comment contact status.nI will try the simulation by removing the option 'adjust to touch'. Whether it can be given 'program controlled'?.Thanksn

[peteroznewman]

nInsert a Contact Tool under the Connections folder and Generate Initial Contact Status.n

[Harish_s]

n

[Harish_s]

nSir,nAs you suggested, I modified the frictional contact type from 'Adjust to touch' to 'Add offset, no ramping effects'.nI added offset value of 2mm.nThen, i generated the initial contact results. Status of all the contacts were closed'.nWhen, i executed the results, I see no touching between the rubber tube and braid. I have attached video below:nPlease suggest me a solution.n

[Harish_s]

nSir,nI am sharing the drive link of my archive file: https://drive.google.com/file/d/1oWnLJgzKLVTnlIfgHklYJnzP8IXFBV4w/viewnThanksn

[peteroznewman]

nPlease explain why you added a 2 mm offset to the contact.nThere are four Static Structural models. Which one should I look at?nThe paper you provided used Shell elements, which are 2D. You have used Pipe elements which are 1D. Do not use Pipe elements. Use Shell elements.n

[Harish_s]

nn

[Harish_s]

nI added the offset based on clearance between rubber and braid. But I think I am wrong.nIn workbench, please look into the module namely ' NR with single braid'.n

[Harish_s]

nKindly refer to the Static structural model, which I have mentioned in the below picture:nI added the offset based on clearance between rubber and braid. But I think I am wrong.nKindly suggest me a better method to solve my problem.nThanks.n

[peteroznewman]

nI made changes to system F which has the Pipe elements. One change was to flip the target and contact entities. The pipe is the target. Offset is zero. You only put in an offset if the geometry you bring in does not provide a surface in the correct location. For example, if you take a tube with a wall thickness of 0.25 mm and you mesh the midsurface, then you want to offset by 0.125 because the nodes and elements are not on the outside surface, but halfway through the thickness. This is what the Shell Thickness Effect ON does automatically for you.nIt was able to converge on three iterations. then I stopped it because it obviously wasn't doing well.nHere is the third converged substep. Gravity has pulled the lower ring along the Z axis by 5.1 mm.nI recommended before that you switch this over to Explicit Dynamics, which is similar to what they used in the paper. I don't think the Pipe element with an Internal Pressure load is supported in Explicit Dynamics. You will need a Shell element version of the rubber tube, as I have been saying several times now.n

[Harish_s]

nThanks for your advice and support.nI will take the approach as you advised me.nSir, I have a query. I could not understand the meaning of 'shell element version of rubber tube'.nBecause, presently, in Spaceclaim, I am extracting the 'circular tube' beam element and in the Static structural module, I am giving the geometry type as 'pipe'.nKindly tell me how to do it.n

[Harish_s]

nSir,nWhen I checked the module file, in which you did some changes, it is observed that the contact status of 'frictional contact' bodies is ' near open'.nWil this give a right solution?nn

[peteroznewman]

nIn SpaceClaim, create a solid tube as you have done, but don't use the Beam Extract tool. Instead, use the Midsurface tool.n

[Harish_s]

nThank you sir.nKindly clear my doubt, mentioned in previous comment, on 'contact status'.n

[peteroznewman]

nAt the start of the simulation, is there a gap between the braid and the surface of the tube? If so, that is why the contact is near open. As the braid pulls inward due to the ring moving along Z and as the tube expands due to internal pressure, the contact will close.nIf there is no gap at the start of the simulation, that is when you use an offset.n

[Harish_s]

nThank you, Sir. Now I am clear.nI will try in explicit dynamics and give you feedback. Kindly advise me that what kind of load can I apply in Explicit dynamics, instead of 'pipe pressure'. n

[peteroznewman]

nPressure.nAlso, don't define Frictional Contact. Explicit Dynamics will have Body Interaction defined by default.n

[Harish_s]

Array nOk. n Today morning, I tried doing it in Explicit dynamics. It showed an error material uses hyperelastic EOS not compatible with beams ansys errornThere was no option to switch 'on' the 'Large deflection', like in Static structural.nKindly give your views on this.n

[peteroznewman]

nLarge Deflection is built-in to Explicit Dynamics.nIn Engineering Data, go to the Explicit Dynamics category and use materials you find there to get started. Please show a screen image of the error. Do you have that accurately stated?n

[Harish_s]

nThank you sir.n

[Harish_s]

ArraynSir,nI tried simulating in Explicit dynamics module.nI created beam elements for braid and shell elements for rubber tube.nWhen I tried simulating, I could see contraction in length of braided fibres, video of which is attached below:nArrayThen, I modeled with 3 braided fibres and followed the same steps in creating meshing elements. To check the model, I applied external force from bottom and the interlaced fibres were flexible, as shown in below video:nArrayUpto this, step, I got desired results.nIn next step. I added load at the bottom, bonded with braided fibres. I am interested to estimate deformation(contraction in length) in Z direction for different loads.nWhen I tried simulating it, the load was moving in opposite direction. The bonding between end of fibres and the load is not intact and gets broken in between.nDue to broken bond, the load moves down due to gravity.nI am attaching video for this:nArrayKindly suggest your correction steps to solve this issue.nI am sharing the google drive link of my ANSYS project. Please check my model steps, and let me know where I went wrong.nhttps://drive.google.com/file/d/1Z5tNYBiuWtK4TzL9qnhRdz62lVbaZDoP/view?usp=sharingnThanks.nn n

[Harish_s]

nSir, kindly give your suggestions to resolve the issue posted above.nThanksn