Non linear contact

  • 111 Views
  • Last Post 11 June 2018
  • Topic Is Solved
Adisa posted this 06 June 2018

Hi,

Is there any solution of this problem.

I use non linear contact, and I get this,

i use ANSYS 18.1.

 

Does anyone have an idea, what i did wrong.

Best regards.

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 07 June 2018

You requested that the entire -127 mm of X-displacement be applied all in a single step.

This is wrong. You need to request that the -127 mm be applied in 100 small steps.

Here is the result after 5 steps:

Notice that there is no stress or strain, there is only rigid body motion because you haven't got any constraint in the Y direction.

  • Liked by
  • Adisa
Adisa posted this 07 June 2018

Thanks Peter,

I changed the BC, increase step and  reduced the displacement.

And I got fine result.

 

How to change that use all number of  CPU in workbench, to get the  fully utilization.

 

I put in theSolver Porcess Settings number of core.

 

One more, thanks Peter.

 

Best regards.

Adisa posted this 07 June 2018

Peter,

The above example was for getting knowledge about the non linear contact.

In my project I need to determine the force when the hook will fall .

I use more steps, refinemesh but the error occurs.

Which type of element is better use, hex or tetra for this contact.

Peter, thanks you so much.

peteroznewman posted this 08 June 2018

Hello Adisa,

Hex elements are better than tetra elements because they fill the volume with about half the number of elements for the same edge size and that leads to faster solve times. However, both types of elements can provide good contact force and stress results.

Hex elements require more geometry prep work to slice up the geometry into brick shaped bodies. One way to have a refined mesh in one part of the body while leaving the rest with coarse elements is the Sphere of Influence mesh control shown below.  This reduces the node count to speed up the solution, while retaining the small element edge length where you expect the high stress gradients to be.

I have answered your question, but I also read your project objective and had a few comments on that as well.

determine the force when the hook will fall

Do you mean the force when the hook falls out of the hole?  Do you want to plot the force profile as a finger pulls on the end of the part?

For a full contact problem, don't use a force if you can use a remote displacement. I made one in a new coordinate system around the face that a finger would engage, and input just one degree of freedom, leaving the others free. You can monitor the force it takes to move the point using a Force Reaction probe. This will be the good model to answer the question, "What is the force profile when I pull on the end of the part?"  That is a good question to ask, but a full contact problem is going to be challenging to converge to the point when the hook is fully deflected into the hole, and the force profile will go almost flat at the friction force of the tip sliding on the side of the hole. I noticed that you have a symmetry BC on the thin face so I applied the force on the end face edges, with the force applied at what would be the center of the full part, but is the corner of this half model geometry.

Before you get that full contact model running (I haven't run it yet), have you already done the simpler models that just flex the hook to determine the deformation and stresses in the hook for an arbitrary tip load?  You might learn that in this design, the hook is past yield at the tip deformation required to pass through the hole.  No sense doing all the work on the full contact model to determine the pull force profile, only to learn that the hook went past the yield point of the material, and the pull force results are invalid.

To estimate if the hook exceeds yield strength, I would suppress the blue part, and hold the grey part where the other contact location is and use a force to push the hook tip back. That way, there is no contact and the problem will solve quickly and easily. Apply an arbitrary load of 100 N, then solve for the tip displacement. Through CAD you know the interference of the hook tip to the side of the hole, so you can easily scale the load until the deformation equals the CAD interference.

Another load case is to push on the underside of the hook to bend it in the way it will flex when the edge of the hole is pushing on the underside of the hook.

The grey part looks like it is molded from a plastic, but in Engineering Data, I only see Structural Steel. I added a new material that I called Plastic, and set the Isotropic Elasticity to 1e10 Pa. You should set that to whatever the proper value is for your material.  I assigned that material to the grey part, but not the blue part.

I have made these changes in the attached ANSYS 18.1 archive.

Attached Files

  • Liked by
  • Adisa
Adisa posted this 08 June 2018

Peter,

Thanks you so much!!

I solved the problem, I need the max force which will occur in the hole when  the hook passes through it.

Thanks.

Adisa

 

 

 

  • Liked by
  • peteroznewman
Aniket posted this 11 June 2018

Try force reaction result in (Solution>Right Click>Insert>Probe>Force reaction) scoped to Contact region Location Method. And select the Nonlinear contact scoped to the two bodies shown in the picture.

Regards,
Aniket

-Aniket

  • Liked by
  • peteroznewman
  • Adisa
peteroznewman posted this 11 June 2018

Adisa, I read your last post and thought you were finished, but now I wonder if you had a question in there. Please let me know if you have another question.

Regards,
Peter

  • Liked by
  • Adisa
Adisa posted this 11 June 2018

Hi,

The problem of nonlinear contact is solved. Thanks Peter.

 

 

Close