How to create proper contact boundaries betweent two bodies

  • 221 Views
  • Last Post 04 December 2019
  • Topic Is Solved
danilouen22 posted this 06 November 2019

I'm new into ANSYS and I'm trying to perform an analysis on a dented pipe, in order to do so I plan to use "transient structural" so I can create the dent on the depressurized pipe, and after the deformation has occurred, pressurize the pipe without the "indenter".

I used SolidWorks to create both the indenter and the pipe in question, I placed them together in an assembly and then opened it in the workbench without using neutral formats.

I used displacement on the edges of the pipe to constrict movement in the Z axis, and the same on the indenter to only allow it to move in the Y axis, I also placed a force on top of the indenter so it would push the pipe and create the dent.

Once the analysis is done, the indenter overlaps with the pipe and the two bodies fail to interact with each other, what tools am I missing? What can I do so the pipe deforms but the indenter doesn't? 

Bonus question: once that step is finished what do I need to select in order to remove the indenter for the next part of the study in which only internal pressure will interact with the dented pipe?

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 06 November 2019

I locked the duplicate post.

In the future, please Insert Image directly into the post.

You must add two things to the model.

  • Frictional Contact between the indenter and the pipe
  • Plasticity in the pipe material model so the dent remains.

You will want a a three step solution.

  • Step 1 advance the indenter into the pipe with a displacement
  • Step 2 retract the indenter back with a displacement (back to zero).
  • Step 3 add pressure to the pipe.

danilouen22 posted this 06 November 2019

Hello Peter,

Thank you very much for your answer and I'm sorry for the incorrectly posted picture.

When you say plasticity in the pipe material, do you mean the multilinear isotropic hardening stress-strain data (in engineering data)? or is it something else?

Thanks again for your help

peteroznewman posted this 07 November 2019

Either bilinear or multilinear isotropic or kinematic hardening.  The simplest model is bilinear and set the yield strength and set the tangent modulus to 0.

danilouen22 posted this 11 November 2019

Hello,

I tried adding all of your recommendations including the plasticity in the model using multilinear isotropic hardening data, I also advanced the indenter using displacement, then added the pressure, but it says a convergence can't be reached and I never get any results, always an error (When I used bonded contact by mistake it ran without any problems but when I switched it to frictional it started showing errors and never reached a solution) 

What could the problem be? 

peteroznewman posted this 11 November 2019

In Workbench, right mouse click on the Transient Structural title and Replace with Static Structural.

danilouen22 posted this 12 November 2019

I did that, and tried solving it but after a long wait an error pops up saying "The solver engine was unable to converge on a solution for the nonlinear problem as constrained."

peteroznewman posted this 12 November 2019

Under Analysis Settings, set Auto Time Stepping to On.  Set the Initial and Minimum Substeps to 100.

Set Large Deflection to On.

Under the Solution Information folder, set the Newton-Raphson Residual Plots to 3.

danilouen22 posted this 27 November 2019

I tried your last recommendations and I still get no result, the error continues to be the same, I tried different things as well but to no end. Is there any way I can upload the file so someone can take a look? 

peteroznewman posted this 28 November 2019

Use File, Archive to create a .wbpz file that can be attached after you post a reply.  The file size limit is 120 MB.

If the file is larger than that, Clear Generated Data on the Mesh/Model to delete the mesh.

I can take a look at your model, but in 19.2 not 16.2.  I think I have an old computer with 16.2 but can't get to that till next week.

I just noticed in the first post that there is only one element through the thickness. That is a problem. You want 4-8 elements through the thickness for plasticity calculations.

danilouen22 posted this 29 November 2019

Okay I will attach it to this post, thank you in advance for your help.

Attached Files

peteroznewman posted this 30 November 2019

Here is a mesh with 6 elements through the thickness. There are now 130,000 nodes.

You didn't have any plasticity on the materials. I changed the pipe to Structural Steel NL that has plasticity.

I changed the Force pushing on the sphere to a Displacement to push down the the sphere into the pipe.

I turned on Large Deflection.

I set the Auto Time Stepping to On and set the Initial and Minimum Substeps to 100.

I created a 2 step analysis. The Displacement is 100 mm in -Y direction in step 1 and back to 0 in step 2.

peteroznewman posted this 30 November 2019

Here is the pipe at the end of step 1 that compressed it by 300 mm.

Here is the result at the end of step 2 when the sphere has retracted to 0.

That solution took about 2 hours on 12 cores.

danilouen22 posted this 30 November 2019

Thank you very much for the help, in engineering data I have tabular data on multilinear isotropic hardening, isn´t that plasticity?

peteroznewman posted this 01 December 2019

In the Static Structural model, there was only Structural Steel with no multilinear plasticity.
Yes, I found that in the Transient Structural, but that analysis is not needed.

danilouen22 posted this 01 December 2019

Oh, the thing is this is the final simulation I need in order to get my paper finished. The study is aimed at finding the failure pressure for a dent of  "0.787 in" but it´s gotta be for that specific material (the one I had included in the multilinear isotropic hardening), do you have any advice? I´m trying to run it with the help you provided earlier  

peteroznewman posted this 01 December 2019

What do you mean a "failure pressure" for a dent of a certain size?

When I buckle my plastic water bottle, putting a dent in it, I can blow air into it to pop out the dent. However, buckling and unbuckling are not failures. 

If I apply sufficient pressure, I can split the side of a water bottle or pipe. That is a failure. In order to characterize the pressure to split a pipe with or without a dent, you would have to provide the elongation at break material property.  Do you have that value?

danilouen22 posted this 01 December 2019

Yeah the thing is when a pipe has a dent that makes the defect area harder due to residual stress, and I want to test the pressure (burst pressure) it can withstand with that specific dent depth. I just need the pressure in which the pipe is under a stress higher than 460 Mpa 

peteroznewman posted this 01 December 2019

When I look at the Mulitlinear Isotropic Hardening curve, 460 MPa is not near the end of the curve. Why is that defined as failure?

The last point on the plot is 12.4% plastic strain. That could be the failure point for the material, but maybe the data doesn't go all the way out to failure. There is a specific material property called Elongation at Break, or just Elongation, which is the Total Strain (elastic + plastic) when rupture occurs. That should be the definition of failure, not a stress value.

peteroznewman posted this 01 December 2019

Here is the Chart for Max. Stress vs Max. Deformation. The dense points with the positive slope is the dent being formed by the indenter going down. 460 MPa is passed early on the way down.  The sparse points going back is the indenter retracting. Again, the 460 MPa value is passed again. The last group of dense points is the pressure increasing.

 

Since the material is being plastically deformed in one direction, then the back stress is being recovered and pressure added to move the material further back, I would have chosen kinematic hardening, or maybe Chaboche kinematic hardening rather than the isotropic hardening that you have used.

danilouen22 posted this 04 December 2019

Thank you very much for the help you have provided!

peteroznewman posted this 04 December 2019

You're welcome. Please chose one post above that best answered your question and click the Is Solution link. That will mark this discussion as Solved. 

Feel free to open a New Discussion for your next question.

Good luck!

danilouen22 posted this 04 December 2019

I'm trying to run it just as you did following your advices as soon as it works I'll mark it as a solution, just in case something else pops up

Close