General Mechanical

General Mechanical

Contact between match solid

    • mekafime
      Subscriber

      Hi,


      Please, I to try to join two parts of a solid, but I have errors. Whats is the best method?

    • Sandeep Medikonda
      Ansys Employee

      Hello, you can use either shared topology or use a bonded/no separation contact


      There are numerous posts in the forum on shared topology.


      Post 1


      Post 2


      Post 3


      This is what we have from the manual on bonded or no separation contact:



      •  Bonded: This is the default configuration and applies to all contact regions (surfaces, solids, lines, faces, edges). If contact regions are bonded, then no sliding or separation between faces or edges is allowed. Think of the region as glued. This type of contact allows for a linear solution since the contact length/area will not change during the application of the load. If contact is determined on the mathematical model, any gaps will be closed and any initial penetration will be ignored.

      •  No Separation: This contact setting is similar to the Bonded case. It only applies to regions of faces (for 3D solids) or edges (for 2D plates). Separation of the geometries in contact is not allowed.


      For more help please specify what you are doing and the errors that you are seeing?


      ~Sandeep

    • mekafime
      Subscriber

      Thanks, 


      I to try use "No separation" o "Bonded" but when I to select a face in solid don't selection in "Contact" or "Target"

    • Sandeep Medikonda
      Ansys Employee

      But aren't they already penetrated? Its hard to tell, can you hide the parts that are opposing and post a pic? Sometimes, you have to interchange contact and target surfaces.


      If you just want the geometries to remain attached, why don't you try the boolean operation on geometries that Peter suggests in this video.

    • mekafime
      Subscriber

      Hide a part


       


    • peteroznewman
      Subscriber

      Mekafime,


      Solid bodies that share a coincident face can be connected without contact definitions in DesignModeler by selecting the bodies in the Outline and RMB to Form New Part. This is the Shared Topology that Sandeep mentioned above.


      I have experienced that frustration when the face I picked is not accepted into the yellow highlighted field. I'm not sure why that is, but I have managed to get something working in the end.


      If you make a Workbench Project Archive .wbpz file, you can attach it after you reply and I will take a look at what you have.  In your reply, say if you want relative motion between bodies, such as sliding, or no relative motion, like being glued together.  I don't understand why you have all "No Separation" which allows sliding between bodies on the shared face, instead of Bonded contact which glues the faces together and allows no sliding. But your best option may be to Form New Part in DesignModeler, have no contact and use Shared Topology.


      Regards,
      Peter

    • mekafime
      Subscriber

      Hi, 


      Thanks for your answer, I have two errors:


      - The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.


      - The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information.


       


      I have the model in .wbpz, how i can attach the file?

    • peteroznewman
      Subscriber

      What version of ANSYS are you using?

    • mekafime
      Subscriber

      18.2

    • peteroznewman
      Subscriber

      In DesignModeler, you have Multibody Parts, but the bodies are not grouped in a useful way. For example Part3 has bodies that don't touch each other.



      What is the goal of your analysis?  Is it to analyze the stress in the triangular sections that look like they may represent welds?  If so, I can see why you might want the large and small rectangular tubes to be two separate parts, then the weld beads to be two separate parts and use bonded contact to obtain the force going though the weld beads.



      What is the intent of the thick plate on the bottom of the large tube?  That can be left as a separate part.


      The correction is to Explode the existing parts, and recombine them into those four meaningful parts.


      You could get a nice mesh with no slicing. I changed all extrusions (except the first) to Add Frozen.


      Now you have 5 solid bodies, each nicely sweepable, and you can use two bonded contacts to connect the two weld beads to the big and small tubes, and another contact to connect the thick plate to the bottom.


      You also have to suppress the 3 surface bodies, as they are not involved in the simulation, right?



       I see that you want to do a 1/4 model, so you do need two slices to do that, but no more!


      In Mechanical, I see you have a Frictionless contact between the large plate and the large tube, but the force is in a direction to open that up. Change the Frictionless contact to a bonded contact and the problem might solve.


      I have to move over to the other computer where I have a Full license as this geometry and mesh has exceeded the Student license limits, so I will read your replies tomorrow.


      Regards,


      Peter


       

    • mekafime
      Subscriber

      Peter,


      - The goal is calibrate a model in Ansys of a thesis to modificate dimensions and investigate others parameters.


      - The welds is to improve the stress in model


      - The thick plate represent the bank of testing, in the thesis the autor uses it


      - The model is simmetryc, for this reason only the fourth part is neccesary, I think ...

    • peteroznewman
      Subscriber

      Mekafime,


      Your model converges if you change the frictionless contact to bonded. The force applied is in a direction to separate the parts and there is no gravity, so there is no static equilibrium when you pull one part away from another part that is fixed. A different change that would allow this model to converge would be if you reversed the direction of the force and pushed the parts together.


      Under Analysis Settings, you have specified 2 steps, but there is no change in step 2, so make it 1 step.


      You have bonded contact between the small tube and the large tube, and the highest stress is in the corner. Did you intend for those faces to be bonded as well as the weld beads?



      If you click on Geometry, you can display by Material. I expect you meant to have a different material assignment than what is shown below.



      If I change all the bodies to Duplex, I see you have Multilinear Plasticity included.



      The first entry for stress is supposed to be the yield strength. Why so low a value?
      Have you entered True Stress and Plastic Strain, not Engineering Stress and Strain?
      See the spreadsheet in this article Sandeep has pointed to before.


      When you use plasticity, you must turn on Large Deflection under Analysis settings.


      After making these two additional changes (material and Large Deflection), the model still solves, but a review of the results shows a problem, the weld bead contact is not properly defined.



      I added one new Bonded Contact. Now the model looks right. The maximum strain appears on the inside of the wall, but that may move around when you refine the mesh and use smaller elements.



      Attached is the ANSYS 18.2 archive.


      Regards,


      Peter

    • mekafime
      Subscriber

      Peter,


      Thanks for your help !. 


      I think that bonded contact between small tube and the large tube is to try avoid two pieces has interferences, the welds must doing the work.


      All material is Duplex.


      I didn´t understand the spreadsheet of Sandeep, I to tried introduce manual valores seeing the chart plot


      "Initial Information" is a new method for me, I will try to learn.

    • peteroznewman
      Subscriber

      You should delete the bonded contact between the small tube and the large tube, leaving only the weld bead contacts to carry the load.


      To get accurate results, you need to take the Engineering Stress-Strain curve and use the equations to compute True Stress, Plastic Strain, Elastic Strain and True Strain.  The curve of True Stress-Strain has higher values of stress than Engineering Stress-Strain.


      Here is another reference to creating a Multilinear Plasticity Hardening Table. This is a little more complicated than the reference given above because it is using experimental data that includes an offset on the Engineering Strain zero.


      Please share the reference you have for the stress-strain curve for the Duplex material.  What is the Yield Strength of Duplex?  What is the Young's Modulus of Duplex?

    • mekafime
      Subscriber

       


       


      I took differents points from this plot (n=15) and introduce to the material table in Ansys.



       


      The material properties, I used 160x80x3


    • Sandeep Medikonda
      Ansys Employee

      Hi,


        I believe you are referring to this discussion.


      The following resources should help a little: 


      Resource 1


      Resource 2


      ~Sandeep


       

    • mekafime
      Subscriber

      Hi,


      I tried to get a better chart, but I have many negative values in Plastic Strain.


       


      The original chart : Curve is orange (n=15)



      I'm not sure if I can reduce values to 323.279 MPa ...


      I attach the file.

    • peteroznewman
      Subscriber

      The attached spreadsheet shows what to put in the material definition for multilinear isotropic hardening plasticity. The first row to use in the model is where the plastic strain begins increasing from zero.  The previous rows with negative plastic strains are not used.

    • mekafime
      Subscriber

      Dear Peter,


      I changed chart of material and the force now is compressive, trying to use the plate in the base, but the analysis state an error and I don't know what is the error ...


      Attach the model

    • peteroznewman
      Subscriber

      I will look at the model next, but first I wanted to ask about the column headings from Table 2. Are the subscripts values of strain? What does the subscript p mean?  I expect the subscript u means ultimate stress at failure.


      I didn't understand what you meant by "I'm not sure if I can reduce values to 323.279 MPa ...", please clarify.


      Also, what is the meaning of the red curve that is labeled Estandar (Standard)?


      Finally, instead of digitizing values off the curve, which results in some wobbles about the true curve, I suggest you fit the three parameters (alpha, E0 and n) for the Ramberg-Osgood model to the data, then create clean data points from the equation. That way the slope column in your spreadsheet will have a smooth decrease in slope instead of the wobble it has from the digitizing errors.

    • peteroznewman
      Subscriber

      Looking at your Solution Output, I see this:


         >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION   5
       *** LOAD STEP     1   SUBSTEP     2  COMPLETED.    CUM ITER =     29
       *** TIME =  0.145833         TIME INC =  0.625000E-01
       *** AUTO STEP TIME:  NEXT TIME INC = 0.62500E-01  UNCHANGED


       *** WARNING ***                         CP =     300.844   TIME= 23:45:57
       Plasticity algorithm did not converge for element 2156,, material 33.  
       *** LOAD STEP     1   SUBSTEP     3  NOT COMPLETED.  CUM ITER =     30
       *** BEGIN BISECTION NUMBER   1    NEW TIME INCREMENT=  0.50000E-01


       *** WARNING ***                         CP =     305.141   TIME= 23:46:02
       Plasticity algorithm did not converge for element 2851,, material 35.   




      With plasticity models, it is often required to set a large number of Minimum Substeps to ensure that plasticity occurs in small increments. I have changed the Initial and Minimum Substeps to 40 instead of 12, which allows the solver to make progress.



      Now the solution has progressed well past the point where the material failure occurs at a Total Strain of 0.4



      At 91% of the 14 kN load on the quarter model, the material has reached the elongation at break value of 40%


      Note that the total load is 4 times 14 kN or 56 kN on the full model.


      I recommend using smaller elements on the weld fillets.



      You can add frictional contact between the base of the small tube and the top of the large tube to help support the compression load. 


      You also should have more elements through the tube thickness.



      The maximum strain is where the material is in compression. You should look where the material has maximum tension since the material can tear apart in tension, while the material may be able to support higher values of strain in compression.


      Regards,


      Peter

    • mekafime
      Subscriber

      Dear Peter,


      1.


      subscript p = tensile proportional limit stress


      subscript u= statis ultimate tensile stress


      susbscript 0.1 = static 0.1% tensile proof stress


      about the author.


      2.


      About the values (323.279 MPa) is ignoring the negative values in plastic stress.


      3.


      The red curves is the standard of the material (state in the European standards), the values used in the analysis are from test.


       

    • peteroznewman
      Subscriber

      Dear mekafime,


      About that table, you say P = the proportional limit, which is typically at 0.002 strain or 0.2 % strain,  The only other value I understand is U = Ultimate stress of 766 MPa and the value of strain for that is given as 40% in the table. What is the strain at the other values of stress in that table between the two ends?


      About the idea of fitting the data to the Ramberg-Osgood formula, the benefit of using a formula for the material model is that you will be able to generate Stress values for strain up to 0.4 where failure occurs. Your current material model only goes out to a strain value of 0.011 but the solution is stretching the material beyond strains of 0.4 which means the solver is using a flat line after the last value of strain in the table.  It is a best practice to have a material model table that includes all the values of strain encountered during the solution so that it is not extrapolating past the last point.


      Since alpha and proportional stress are given in the table, I could adjust the value of n until the curve went through 766 MPa at a strain of 0.4 and that value of n is 3.48 so the curve below might be a better material model for large strain than the material model you fit to the relatively smaller strains of 0.011.



      Regards,


      Peter


       

    • mekafime
      Subscriber

      Hi Peter,


      I modificated all in mesh and connects, but in substep: 


      - Initial substeps = 40


      - Minimum substeps = 40


      - Maximum substeps = 60


      But I have the same error ..

    • peteroznewman
      Subscriber

      Okay, but how far did it get?  What was the Total Strain at the last converged substep?

    • mekafime
      Subscriber

    • peteroznewman
      Subscriber

      If you show the Force Convergence Plot, that gives an idea of how far it got. 


      Please attach an archive and I will take a look later today.

    • mekafime
      Subscriber

      Hi Peter,


      Thanks for your time.


    • peteroznewman
      Subscriber

      Hi Mekafime,


      I changed the Mesh Details to force two elements through the thickness of the large tube.




      I also added a slice in DM to make nicer elements in the corner of the small tube.



      You didn't set the Minimum Substeps to 40, I see 12.



      I am going to run that now and report the results later.

    • peteroznewman
      Subscriber

      One more change is to the table of data for the Multilinear Isotropic Hardening.


      I looked up the TBDATA command and it can only hold six points! 


      [EDIT: data is not in a TBDATA table.  More than six points can be used.]


      Here is the a table based on the Ramgood-Osgood model I wrote about above.



      In hindsight, I would have put the points closer together at low values of strain, and spaced them out at the high values of strain where the function has less curvature.


      Below is a more optimal spread of points. Note that below is Engineering Stress and Strain.



      The attached ANSYS 18.2 model solved to the end and had an interesting deflected shape. This is true size deformation.



      Probably could have run with a Minimum Substeps of 20 instead of 100.

    • peteroznewman
      Subscriber

      Dear Mekafime,


      Sorry, I didn't know that you were on a Student license. Some members on this site have unlimited Research licenses. The model I showed above has nearly ten times too many nodes.



      The way to have a small number of nodes for this problem is to create a midsurface for the two tubes and use shell elements. The weld fillets remain as solid elements. 



      The model above is computed from the shell model shown below.



      This model stays under the Student node limit of 32,000 nodes or elements.



      An example of this is attached as an ANSYS 18.2 archive.


      Regards,
      Peter

    • mekafime
      Subscriber

      Hi Peter,


      The problem with the license was because the university updated Ansys to 19.1. I made some changes:


      The radius was modified, add weld in the radius of the brace:



      I changed the restrictions for the model that is the fourth part and I changed it by symmetry region.



      The material of the weld is bilinear isotropic hardening: 



      But the model throw the following results:


      - The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information.


      - The solution failed to solve completely at all time points. Restart points are available to continue the analysis. 


      - The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.


      - Although the solution failed to solve completely at all time points, partial results at some points have been able to be solved.  Refer to Troubleshooting in the Help System for more details.


      Please, how could the model improve?


    • peteroznewman
      Subscriber

      Hello Mekafime,


      Since I see you are online, I will make a quick reply.


      See there is a + on Solution Information folder. That means you have some Newton-Raphson Force Residual Plots that will show you the last few iterations. Look at the Max value of these plot. The location is the relevant information.  It is at these locations where you add a Mesh control to make smaller elements that have been used in the solution that failed.


      Here is a relevant post, with a video!


      I will take a closer look at the model you have attached later today.


      Regards,


      Peter

    • peteroznewman
      Subscriber

      Please post a reply after trying what you saw in the video link in the previous post. You can attach a fresh archive with the mesh control and hopefully, it got further, or even better, it went all the way!

    • mekafime
      Subscriber

      Hi Peter,


      The video is very useful, I have tried to refine the mesh, but the problem persist, and the time has increased in the analysis.



      The problem is this part of the model.



      I have tried many mesh configurations, the ultimate mesh was this, but the model has errors, Could the problem be another?


      Thanks for your time.

    • Sandeep Medikonda
      Ansys Employee

      Hello Mekafime,


      What contact settings are you using?


      Have you tried scaling the contact stiffness? Increasing of FKN value will reduce the contact penetration values.


      Also, Change the Contact detection to Nodal Detection from Integration point detection.


      You can always use the normal-lagrange method to observe near zero penetration but it is often not recommended as you might run into convergence issues.


      You can also try a run changing the 'Updating Stiffness' to 'Every iteration, Aggressive' but note that this will make the simulation even slower.


      Regards,


      Sandeep

    • mekafime
      Subscriber

      Hi Sandeep,


      This is the configuration of contacts



      How I can scaling the contact stiffness and how I can change to contact nodal integration? 


       

    • peteroznewman
      Subscriber

      Here is what I see in the model, so Sandeep can see too.



      And here is the mesh.



      Here are the changes Sandeep is recommending, which I agree will help.



      The Normal Stiffness Factor is 1.0 by default. Above I increased it to 10. I also changed the Detection Method and changed the Update Stiffness setting.  I would also recommend more nodes around the radius.  I guess you are no longer limited by the Student license.

    • Sandeep Medikonda
      Ansys Employee

      Thanks Peter.


      @mekafine: Please see this section of the manual.


      Note that Frictionless (Rough & Frictional) is a nonlinear contact type and changing the settings I suggested above should help with Penetration.


      Regards,


      Sandeep


       

    • peteroznewman
      Subscriber

      I found that links to the Online help need special handling to be useful.

    • peteroznewman
      Subscriber

      Mekafime,


      Those settings prevented the penetration.



      Convergence failed after 66% of the load.  If you want to crush it further, you should use a displacement load not a force load.



       

    • mekafime
      Subscriber

      Hi Peter, 


      Why is different, I can change the Time? , in my case is Time: 1, no 0.6625



      If I change for displacement, how I can get the chart force- displacement in any node ? 

    • peteroznewman
      Subscriber

      Hi Mekefime,


      Here is the Force-Displacement plot for the above run in blue.



      I drew in the red curve by hand to illustrate what a displacement load can do that a force load cannot.
      The red curve is not data, it's just a sketch. I am running the model with an actual displacement load now.


      The force load was asked to find an equilibrium at each incremental increase in load from zero to 25 kN. The problem is there is no nearby equilibrium for a small increase in force past 16.5 kN.  You have to wait till you crush the 154 mm tall tube down to nothing and the vertical tube starts pushing on the bottom of the horizontal tube.


      A displacement load has no problem following the solution past the point of zero slope on the force-displacement curve, because there is an equilibrium past that point, it just has less force that the earlier points.


      If you request the reaction force from the displacement boundary condition that is set to Y = -150 mm, you can plot the force-displacement curve.


      Regards,


      Peter

    • peteroznewman
      Subscriber

      Using displacement reveals another contact needs to be added to the model: one between the top and bottom inside faces of the large tube, which passed through each other during this simulation.



      Here is the reaction force to go down 150 mm.



      Regards,


      Peter


       

    • mekafime
      Subscriber

      Hi Peter, 


      how I can get this plot N-s? is in any node?


       

    • peteroznewman
      Subscriber

      It is the reaction force for the Displacement boundary condition that replaced the force on the top face of the small tube.

    • mekafime
      Subscriber

      It is very interesting how the model improves from the initial situation.


      I am not sure about what is the contact between the top and bottom inside faces of the large tube. 

    • peteroznewman
      Subscriber

      Here is what I got after adding frictional contact between the top and bottom inner faces of the large tube. Note that the convergence failed when the new contact closed, but I just restarted it with 500 Initial Substeps and it completed the solution.


      Right click on the video after it starts and select Loop to make the video play over and over.



       


      Here is the reaction force plot for the 150 mm displacement.



      Once the top-bottom contact closes, the force spikes up.
      Once the vertical tube buckles, the force begins to reduce again. Awesome!

    • mekafime
      Subscriber

      Please, it is possible that you can attach the model?

    • peteroznewman
      Subscriber

      ANSYS 19.1 attached

Viewing 49 reply threads
  • You must be logged in to reply to this topic.