Ansys Products

Ansys Products

Hyperelastic model Design Analysis for DragonSkin 10

    • Sarvesh Rathi
      Subscriber

      I have been trying to simulate a hyperelastic model made from DragonSKin 10 with the following properties being put in Ansys:

      Odgen 3rd order model with parameters taken from the research paper

      Mesh sizing of 0.001m

      Quadratic Non linear mechanical model

      1 Fixed Support from where I am inducing pressure

      2 frictional support to prevent normal movement from the sides

      Pressure of 50000Pa

      Analysis settings set as Programmed controlled autostepping with total 3 steps and minimum step size as 0.001

      Is it possible to set up a 10 minute call to debug this issue. i am trying to put this simulation in a paper with deadline November 15. I am a student at New York University studying masters in robotics. Please contact me at sr6090@nyu.edu.

    • Ashish Khemka
      Ansys Employee

      Hi Sarvesh,

      It would not be possible to set up a call through the forum. You will have to create a service request. By the way, if you can elaborate on the issues that you see while performing the analysis then it would be easier for members to comment on the queries.

      Regards,

      Ashish Khemka

       

    • Sarvesh Rathi
      Subscriber

      This is the screenshot of my present status. I am not sure what I am doing wrong in the simulation. It is not bending enough. I want to make sure if I have done everything correct in the simulation.

      Kindly refer to Nov 9 comment for the parameters I have set.

    • Sarvesh Rathi
      Subscriber

      Also, kindly tell me how to create a service request.

      I tried contacting the support already but they did not respond.

       

      Kindly request to schedule a call as soon as possible.

    • Sarvesh Rathi
      Subscriber

      Kindly clarify what would be the analysis settings for optimal hyperelastic output,

      My settings are:

    • Sarvesh Rathi
      Subscriber

      Also, what does step control mean? Does increasing the number of steps lead to more bending.

      Should I use steps as initial and minimum time step: 100 and maximum time steps 200

      or should i use time as mentioned above.

      Because I have seen that varying this setting leads to an output which leads to no bending sometimes.

      Kindly clarify. It would be a huge help if someone could contact me at sr6090@nyu.edu or 3474715977 to solve and clarify the issue.

      Thanks.

    • Ashish Khemka
      Ansys Employee

      Hi Sarvesh,

       

      For technical support, you should have TECS: Technical Enhancements and Customer Support (TECS) | Ansys

      The error is element distortion. Try using a finer linear mesh. You can start iterations with a coarser mesh and then try to refine the mesh. 

      Define substeps/ timestep size for each step. This will help you to increment the load slowly. Also, please check in which step are you experiencing this issue.

      Having more substeps help. Please refer these links for more on substeps:

      You don’t wanna step to this: Breaking down Loadsteps and Substeps in ANSYS Mechanical - PADT (padtinc.com)

      ANSYS Step Controls in Structural Analyses (mechanicalland.com)

      ">ANSYS Mechanical Tips & Tricks: Changing Multiple Load Step Settings - YouTube

       

      Also, these courses might help you:

       

      How to Perform Curve-fitting for Hyperelastic Material Models — Lesson 1 - ANSYS Innovation Courses

       

      Hyperelasticity | Ansys Innovation Courses

       

      Regards,

      Ashish Khemka

       

       

       

       

       

       

  • Sarvesh Rathi
    Subscriber

    Thank you for help Ashish.

    I already requested a support call through a same link a while back but did not get any response. Nonetheless, I have again requested the mail now. Kindly update if you got the request.

    I also tried calling the support, but there is no technical support or operator connected. Kindly suggest if there is any direct number i can connect with.

    I have defined mesh as non linear quadratic mechanical with face sizing method meshing of element size 1.e-3 m. Is this fine? or should I have a finer mesh?

    Kindly note that I have already defined the timesteps. Doesnt the settings as mentioned in the above screenshot define this properly. If not how to define timesteps for each step??

     

  • Sarvesh Rathi
    Subscriber

    I am also trying to achieve further bending of the tip. Any advice on how i can improve that? Any design considerations?

  • Sean Harvey
    Ansys Employee

    Hello Sarvesh,

    So, it does not matter if you use time or substeps.  Also, steps are to break the load conveniently for loading purposes, and substeps is used to break that step into smaller substeps. You do not need 20 steps. You just need 1 if you wish all loads to ramp up over that first step.  Do make sure your pressure is ramping from zero at time zero to max at time = 1.0 (end of load step 1)

    I would start with 200 substeps, min 10, max 2000.  

    In meshing, I would set the physics preference to nonlinear mechanical. One of the biggest issues is the elements are poorly shaped to begin with, so a little bit of deformation and they become ill-shaped  and the solver can not solve with them.

    You may wish to try a more uniform mesh, but turning off adaptive sizing.

    Have you tried just testing the stability of the material?  You can take a cube of the material and deform it in various modes of deformation to see that it is behaving numerically stable. This is helpful to debug material model issues.  

    I have seen users put values from papers into Ansys in wrong units, so please double-check this.

    Also before you run, you go to Analysis Settings> Identify Element Violations and set to 1.  After you run the model and it does not solve, under solution information, it will have some objects that indicate which elements are becoming highly distorted. You can share images of the elements and where they are located.  By improving the mesh, you can sometimes go further.

    If the deformations expected are very large, then the model may need to use nonlinear adaptive remeshing (NLAD).

    Please try these recommendations first. Thank you!

    Regards,

    Sean

  • Sarvesh Rathi
    Subscriber

    So if I understand it correctly, does number of steps equal to amount of time? Since when I apply pressure with more number of steps, I am not getting the spikes. My pressure is going from 0 to 20-50kPa.

    I have already tried min 100 substeps and maximum 200. I also tried sub-time steps minimum 0.001 to max 0.05. But I dont seem to find a good bend.

    Physics preferences are already set to nonlinear mechanical with quadratic setting. In addition I have put a face sizing method and set element sizing to 0.001 m. Is this fine?

    Uniform sizing as in Hex or tetrahedron? I have tried it but am unable to figure out how to reduce the element sizing there. Hence I am using face meshing.

    Any resource to understand how to do material stability in ansys? I will try it out and get back to you.

    I have double checked units and it is correct in my simulation.

    Yes I have already tried that using newton rafson method. Will share the results shortly. I dont understand how to deal with those.

    Yes. The deformations expected are very large. Ill try NLAD and get back to you.

     

    Thank you so much for your time.

  • Sean Harvey
    Ansys Employee

    Hello Sarvesh,

    Each step has a time associated. For example a model with 2 steps, step 1 can have a time of 1.0 sec and step 2 can have a time of 1.0 sec and the total time of the simulation will be 2.0.  But for static analyses, time is only a marker. It has no physical significance. So let's ignore time, and just stick with substeps. Since you have just 1 load, run it in one step.  At end of simulation you get to 1.0, model is has all the load applied.

    Max substeps of 200 may not be enough. When the convergence is difficult, it can need more.  Set to 1000 or 2000.

    Start with coarse mesh and avoid face sizing.  We want the best-shaped elements, not a detailed mesh. Later we can refine.

    Uniform elements means not having large elements then very tiny ones.  You may not be able to get hex, but you can try hex dominate, or multizone too.  Tets can be fine as well. The key is they are not ill shaped, or become ill shaped, so element quality in large deformation hyperelastic is critical.

    Drop the midside nodes (use linear elements, not higher order) for this hyperleastic.  Ansys will change the element formulation when you do this.  This will allow the element to be more robust in deformation and less likely to become ill shaped.  Don't drop midside notes when using test and non-hyperleastic materials (like stress analysis with linear materials such as metallics, plastics, etc.)  They will be too stiff.

    By material stability, take a block and try to deform it in some standard modes of deformation. Tension, compression, shear.  Put boundary conditions so the block is uniformly loaded.  It is like a single element test of the material.  If you can't get larger strains that you expect from the material curve fitting with simple geometry, then the material calibration (curve fitting) may be the problem.  We want to isolate if it is material related or mesh related.  My prior comments above assume that material is not the problem (meaning the curve fits produce stable material response and behaviors).

    Try all this before going to NLAD.  I may have some more tips to share later.  Thank you.

    Regards,

    Sean

     

  • Sarvesh Rathi
    Subscriber

    Thank you for your advise and time Sean.

    I used uniform meshing and number of steps to 1. Minimum substeps: 200 and maximum to 2000. 

    I am trying to understand why the front part of the finger is not bending further. Any ideas? I want a full finger like curl.

  • Sean Harvey
    Ansys Employee

    Hello Sarvesh,

    I think this is process, at least getting further than before. So with time=.94 and if end time is 1.0 you have 94% of the pressure applied. Can you highlight the loading on the model?  Where is the pressure applied?  Also, can you highlight where you have contact in the model. Also double check the material assignment is correct under the parts in geometry.  Just in case it was not.  I don't think this is the issue but just a basic check. Thanks.

     

    Btw,  does the curve fitting match the material test data? Can you share plots of the fits and which hyper elastic material model you are using.

     

    Sean

  • Sarvesh Rathi
    Subscriber

    This is the loading on the model. Kindly note that the base is not included here. All the inner faces and holes through which air passes are included in the pressure loading region.

    With base included the model is not even moving.

  • Sarvesh Rathi
    Subscriber

    Contacts are basically the inner faces which might come in contact if they expand to the limit.

  • Sarvesh Rathi
    Subscriber

    Here there are multiple materials that I was trying with but from these I used dragonskin 10 variables from the research paper.

     

  • Sarvesh Rathi
    Subscriber

    How can I simulate the jamming mechanism in ansys?

    Reference: (PDF) A Review of Jamming Actuation in Soft Robotics (researchgate.net)

  • Sean Harvey
    Ansys Employee

    Hello Sarvesh,

    Thank you for sharing.  So the material curves you provided. Do they make physical sense to you?  For example, a uniaxial tensile test that has a negative slope means that if I push to material into compression, it will stretch.  In other words, negative stress, gives a positive strain.

    It seems this material is a type of silicone right?  Would you expect this behavior?  Did the paper you get this from have the stress-strain curves to verify against?  Also, there are some hyperleastic material models that even though are the same name, the implementation is a bit different.  For example, in Ansys and Abaqus, there can be a difference in the implementation even though the coefficients seem to be the same symbols. 

    Can you share your material reference, or elaborate?  Thank you.

    Regards,

    Sean

  • Sarvesh Rathi
    Subscriber

    Link

    This is the link to the following research paper: Titled : Finite Element Modeling of Soft Fluidic Actuators: Overview and Recent Developments

  • Sarvesh Rathi
    Subscriber

    Im not entirely sure what you mean by this: 

    I push to material into compression, it will stretch.  In other words, negative stress, gives a positive strain.

    But in my understanding when air is induced in the internal compartment it should inflate. And yes, the material is silicone rubber.

    Refer to this link for the simulation output I am looking for :

    ">full strain soft-robot hyper-elastic actuator - YouTube

     

  • Sean Harvey
    Ansys Employee

    Hello Sarvesh,

    Let me clarify. 

    I modeled your material using those constants on a simple cube.  

     

    I push into the cube, so what should we see in the simulation?  You expect it would squish down right?  But look what it does.  The cube stretched.  This is non-physical for the silicone material.  

     

    Look at the paper you provided and we see the stress - stretch behavior.

    Details are in the caption following the image

    But look at the curves in the engineering data.  They show a negative relationship between stress and strain.  

    This is where your problem lies.  You have the incorrect material response.

    Now you may ask why?  Is it the units or typo?  While that is a common error, it is related to the slide below.

    The Ogden model in Ansys has a slightly different construct using the variable. That paper has the constants for Abaqus.  The equations are identical, only that what is that mu is different.  To compute mu in Ansys, set the first term ui/ai = 2ui'/ai   Let ui' be the value from Abaqus, now you solve for ui (which is mu for Ansys) and you will get ui = 2ui'/ai.

     

    I have done this and this is the modified material data

    Notice with positive stress we have positive stretch (strain).  This is physical behavior for the silicone material.

    Alternatively, you can input the material data provided from the charts, being very careful to convert to engineering stress and strain, not true stress and stretch. Then you would curve fit using the curve fit tools in engineering data. My colleague already provided lessons on how to do that.

    I suggest you try the values I have provided to see if you start to get physical behavior.  I leave it to you to double-check my inputs.

    I also suggest you take the hyperelastic free course which would have helped you identify that you have a non-physical stress-strain response.  But the mistake you have here is an easy one to make. It can be easily assumed that if Ansys and Abaqus have Ogden, then the mu and alpha are the same.  Unfortunately, the forms are slightly different.  Now you know :)

    Please circle back and let me know if you start to get the actuator to deform more as expected.

    Regards,

    Sean

  • Sarvesh Rathi
    Subscriber

    Hi Sean! It works perfectly now! I will send a screenshot shortly.

     

    I want to create a jamming mechanism on this model by creating an additional air chamber below the one I already have, and filling it with granules of coffee and creating a vaccuum is this chamber by applying a negative pressure. Any ideas how to do that without the granules first and then with the granules and putting a negative pressure.

  • Sarvesh Rathi
    Subscriber

    This is the output without jamming with 50kPa pressure. Could you please help me with the jamming negative pressure to input applied pressure ratio? How to decide how much pressure ratio to apply?

  • Sarvesh Rathi
    Subscriber

    This is the output with input pressure 25kPa and jamming negative pressure -6kPa. Would appreciate your advice with respect to the quality of my simulation and any way to improve this further.

  • Sean Harvey
    Ansys Employee

    Hello Sarvesh,

    I am glad you were able to realize the large deformations!  Introducing granules will not be an easy accomplishment.  If I understand the situation, modeling their interaction with contact in Mechanical will be time-consuming, not to mention that each granule will want to have 6 DOFs, so this simulation will typically need to be run in a transient dynamic.  There are ways to solve with Mechanical, but other methods too using LS Dyna or combining Rocky DEM to model the interactions of the granules with the mechanical, but let's take a step back to try and simplify...

    The negative pressure is the vacuum. You apply that negative pressure.  If the space can not completely close because of granules, then we can introduce offsets in the frictionless/frictional contacts that would act to prevent the space from completely collapsing.  Have a look at the offset in the contact details.  If you enter a positive offset, then the contact will take place that offset off of the surface.  This can possibly be used as a rough way to have a stop/jam as the contacts start to interact.  You would have to do some trial and error in the offsets, and which faces can touch which faces, but see if this is something you can try to incorporate.

    Regards,
    Sean

  • Sarvesh Rathi
    Subscriber

    Thanks Sean for the explaination. Is there any material i can read or video i can watch? Ill try to simulate something next before i take any more of your valuable time.

  • Sean Harvey
    Ansys Employee

    Hello Sarvesh,

    I don't have any video on lesson on that specifically.

    Can you get to this location in the help,

    Geometric Modification (ansys.com)

    If you only have student version help, then search for 

    Geometric Modification

    in the Contact settings.  There you will find an explanation on the contact offset and how it works.  Try that.

    Thank you

    Sean

  • Sarvesh Rathi
    Subscriber

    Thanks for your prompt advises. Cant appreciate enough. 
    I will look into it and get back to you with any doubts. 

  • Viewing 28 reply threads
    • You must be logged in to reply to this topic.