## General Mechanical

#### surface contacts between components

• balsaidi
Subscriber

We need to perform shear test study. Our model consists of multiple components that have capability to slide on each other. We need to define No separation or frictional contacts type between certain surfaces. Model fails to run!

Please see the attached pdf file for clarification.

Thanks,

Bashir

• Sandeep Medikonda
Ansys Employee

Bashir,

Please try the suggestions provided in this discussion which should help with this error.

Regards,

Sandeep

• peteroznewman
Subscriber

Bashir,

Not everyone here can open attachments, so below is an image of what you attached above.

The reason the solver fails in this shear force model is that there is no resistance to the force, therefore the displacement is infinite, which causes the solver to stop.

You can have a solution if you use Frictional contact with a non-zero coefficient of friction, AND apply an X direction tension force to create a normal force on the contacting faces, so that there will be something for the coefficient of friction to be multiplied by to generate a shear force AND apply a shear displacement, not a shear force, since if the shear force is greater than the frictional force, you will again have an infinite displacement.

Regards,

Peter

• balsaidi
Subscriber

Peter,

Not sure if I did it correct, I used 0.25 coefficient of friction along with your suggested B.C. Solver still fails to run.

Thanks,

Bahir

• balsaidi
Subscriber

Thanks Sandeep!

Regards,

Bashir

• peteroznewman
Subscriber

Bashir,

Did you turn Large Deflection to On under the Analysis Settings?

You should insert a Contact Tool under the Connections folder and Generate Initial Contact Status.  If all the frictional contacts are not closed, then you have to take some corrective action.

You need to break the solution into at least two steps.

In step 1, the 10 N force is applied, while the tangential displacement is kept at 0 mm.

Then in step 2, the tangential displacement of 10 mm can be ramped on gradually.

Getting the model to converge in step 1 may require Auto Time Stepping to be changed from Program Controlled to On and the Initial Substeps to be set to 10 or higher.

I remind you of the advice I gave before to suppress all but 3 links. Make the left link fixed, let the center link have contact on either side and let the right link have the X force and Y displacement. Get this working before you try to solve with more than 3 links.

Regards,

Peter

• balsaidi
Subscriber

Peter,

Still unable to run. Do you mind check it for me please? Attached.

Thanks,

Bashir

• peteroznewman
Subscriber

Bashir,

I remind you of the advice I gave before to suppress all but 3 links. Make the left link fixed, let the center link have contact on either side and let the right link have the X force and Y displacement. Get this working before you try to solve with more than 3 links.

Get Step 1 running, the tension force along X, before worrying about step 2, the shear force.

You have to set the mesh to have more than 2 elements through the thickness. This mesh has only 1 element through the thickness, which is inadequate.

Use the Mesh Sizing setting for Proximity with 2 elements across the gap with a minimum gap of 0.5 mm.

Unfortunately, this is going to create a very big model that will take a long time to solve.

You will be better off extracting the midsurface from this solid body and meshing shell elements on a surface body.

Build a model to put a tension force on those.

Attached is an ANSYS 17.2 archive of a surface model that has an assigned wall thickness of either 1 or 2 mm.

Regards,

Peter

• balsaidi
Subscriber

Hello Peter,

I made your suggestions, 3 components of shell. Issues are, I couldn't make more than one layer of mesh elements as you did for these shells.

Also, I had to define surface contact regions manually since the system couldn't detect them automatically.

Thanks,

Bashir

• peteroznewman
Subscriber

Hello Bashir,

The solver failed because the contacts were not closed when it started.

The contacts were not closed because you didn't turn on Shell Thickness Effect.

The contacts were not closed because you didn't expand the geometry until the point where the faces are touching.

I explained previously that you can only start solving when the faces that have to push on each other are touching.

If you want to learn how to use contacts in ANSYS, you should start with a simple example and work your way up to more complicated cases. This model is complicated and I recommend you return to it after you have demonstrated success on simple examples.

Regards,

Peter

• balsaidi
Subscriber

Hello Peter,

I am confusing regarding your suggested method for running a model, do you mean I need to apply tension force only at step one till see the result of applying this force along x-axis then I rerun the model in step 2 which is by applying the shear displacement only along y-axis?

Thanks,

Bashir

• peteroznewman
Subscriber

Hello Bashir,

In the Geometry editor, you have to make the parts touch before you mesh them and apply loads and supports.

Then you apply a tension force in x direction in step 1, and a shear displacement in y direction in step 2.

Regards,

Peter

• Ashish Khemka
Ansys Employee

Hi Bashir and Peter,

I was thinking of an alternate approach - apply a known displacement, say in step 1 to close the gap and then apply the required force in second step. Also please see if adjust to touch helps.

Regards,

Ashish Khemka