Learning Forum

[RoyalFlowers]

Hi Everyone

I am modelling a complex friction-less contact and facing some issues that maybe your experience could help me.

In this model as the attached picture shows, there are some contacts between load applicator as a rigid body and the main structure as a flexible body.

raised questions are as bellow:

1)     1)  Updating normal stiffness in each iteration:

When this option is active, does software increase normal stiffness value in each iteration to the default one (1 for frictional and 10 for bonded)?  what the difference between update stiffness in each iteration and never?

2)     2)  Detection Method:

The results are different between Nodal-Normal-Target method and 4 other options, and I think that it could be because of Corner-surface contact in a section. Now how could be sure that which option should be selected?

3)       3) Interface Treatment:

For this option also the results are different, if I select Adjust to Touch or Add Offset, No Ramping. Because of initial penetration and some possible errors in positioning load applicator, I selected adjust to touch option, but it was confusing that the results were remarkably different for another option. For this part also, which option are suitable?

I am grateful if someone could advise me if they have some experiences in this regards.

[peteroznewman]

In future posts, please use the Insert Image button to put your image in the post because ANSYS employees are not permitted to open attachments.

The goal of nonlinear contact (not bonded) is that the parts should not penetrate by an excessive amount. Insert a Contact Tool into the Solution branch then Insert a Penetration plot into the Contact Tool folder to evaluate the magnitude of the penetration on a contour plot.

1)   Updating normal stiffness in each iteration.

This is generally the best setting, because it allows contacts that have excessive penetration to automatically adjust the stiffness to reduce the penetration. There is a computational cost to do this, so when you don't need it, you can turn it off to get a very slight improvement in solution time. You can't just set the contact to an extremely high normal stiffness because that causes numerical problems for the solver and the solution may not converge.

2)   Detection Method:

The results are different between Nodal-Normal-Target method and 4 other options.

There are choices because there are differences in the computational cost of each option. The default option provides the fastest solution time, but if you observe excessive penetration in the results, you can change to another option to reduce the penetration and incur a slight increase in solution time.

3)  Interface Treatment:

Adjust to Touch is automatically selecting a value to put into the Offset setting, which results in the contact being closed. This is useful when the CAD geometry is perfectly tangent (and also when it is not perfect), but due to discretization in meshing, a tiny gap has been created. The solver has a very difficult task getting started when contacts are initially open, and a much easier task when the contacts are initially closed.

It's always best to have the CAD match reality as close as possible, but Offset can be a time saver to eliminate doing a very small adjustment in CAD and allow an interference to be created where none existed in the CAD geometry. For example a press fit of a shaft in a hole, where both the shaft and hole were drawn at the same nominal diameter of 10 mm, but the tolerances on the parts call out an interference fit. You can just type in the magnitude of the interference in the offset parameter in the contact definition.

[RoyalFlowers]

Hi Mr. Peterrozenewman,

Thanks  a million for your answers.

First of all of if the max. penetration in a really small point is 0,066, is it acceptable?

1) Updating Normal Stiffness:

As you said Updating Stiffness is the recommended option. But I want to know what does Ansys do exactly in this option? Because of convergence problem I selected Normal Stiffness=0,1, then by activating Updating Normal Stiffness in each iteration, how does Ansys solve problem?

And as I understood Updating Stiffness increases solution time to reduce penetrations as much as possible, but if it is inactive the model could be solved but with some penetrations (if K value is small). Then we need to check the final penetration contour to see whether penetration values are acceptable or not. am I right?

2) About contact detection method:

I checked all options to see the effect of them on the results. As you can see in the picture the left side of load applicator has edge-surface contact with the structure because of a fracture plane which slices the contact surface in two parts with an offset. So, when I selected Nodal-Normal-Target Method, displacement of loading center is close to the experimental values. However, selecting one of 4 other options results 20% error in estimating displacement of loading center. So, I do not know why should it happen, and how can I select the best contact detection method?

3) Regarding Interface Treatment:

If I select adjust to touch or add offset (no ramp), displacement of loading point is different. Adjust to touch options results in an accurate value which is close to experimental one. However, the result of add offset option is really far from the experiment. So, because of that I do not know which option could be more accurate and reasonable to select.

I really would be grateful for your advice in advance.

Best regards  

[peteroznewman]

Please say what version of ANSYS you are running because they make minor changes to terminology over time.

1) ANSYS Help has a Chapter in the Mechanical APDL, Contact Technology Guide, Chapter 3.9.4 that explains a lot about Contact Stiffness.

2) When two bodies make contact, the solver must create an equal and opposite force to prevent penetration, but what direction should that force be applied? Consider a 2D case of a flat face on one side of the contact pair and two facets on the other side of the contact pair. A single node on one element is touching the face of the element on the other side. If the blue body is defining the nodal normal, you will get the blue direction of force for both bodies, which is what you want. If the orange body is defining the nodal normal, you will get the center orange direction, which is the average of the two orange face normals. That is not what you want. You can flip between the tilted force direction and the vertical force direction for the normal component of the contact force (have not considered friction here) by flipping which body is the Target and which body is the Contact side of the pair, or by flipping the Nodal Normal selection.

Now if there was no vertex with a sharp angle, and instead a rounded body that made tangent contact, then the two arrows point in the same direction.  The lesson here is to use smooth surfaces to make contact. Your geometry seems to have a lot of facets. That is going to make the results change as you change contact definitions. I recommend you create smooth surfaces in the geometry editor.

3) Offset does a geometric offset of the surface.  Adjust to Touch translates the contact surface in X, Y and Z in a direction to close the gap. These are different. The best option is to have smooth surfaces in CAD that are initially tangent and don't use any Geometric modifications. However, after meshing, you will get facets again. The best practice is to use small elements in the contact area to minimize facet angles on what was a smooth surface.

[RoyalFlowers]

Hi Mr. Peterrozenewman,

Thanks a lot again for your illuminating answers

2) Regarding question 2, there is now way actually to make surfaces smoother and change the geometry. Because there is a fracture plane on the lefts side of tibial head. And I think that nodal-normal-target option seems logical for this model,because target body is smoother than contact surface including with facets. Contact between medial load applicator and medial parts of bone are defined as bellow.

 

 

3) Regarding interface treatment, I tried to use really small element size in the contact area. But because of some initial penetrations and errors in positioning load applicator, I selected adjust to touch to be sure that contact and target surfaces are initially in touch. However, still I can not fully understand why the result are very different when Add offset-no ramp option is selected. How could we be sure that an appropriate interface treatment method is selected? Is it enough to compare the outcomes with experimental data and select the option with closer outcomes? Is it interesting that Adjust to touch option has 6% error but by selecting Add offset no ramp options results are 20% smaller than experimental ones.  Do you think that contact refinement could be helpful, to get the same results for both interface treatment methods? 

I am grateful for all of your kind attentions in advance.

Best regards, Shabnam Samsami

[peteroznewman]

Adjust to Touch can move surfaces in unexpected ways. Look in the Solution Information folder for Solver Output, which is the listing of the Solve.out file. There should be a statement on how Adjust to Touch moved the contact surface in X,Y and Z.  Compare that with the offset distance you are using. You can move the faces both ways in CAD and see the effect. 

How are the two sides of this joint supported and loaded?  Does that support/load allow the joint to "find" the natural, lowest energy seating orientation?  In other words, if the top side is fixed, is the bottom side free in X, Y, Z and Rx, Ry and Rz to adjust so that there is only an axial load on the bottom side? If there are too many constraints on the bottom side, then unrealistic torques will be supported while the joint makes contact at high spots, rather than at the lowest point.

What is the experimental data measuring?  How is it measured? What is being measured in the model?  Is that the same measurement?

[RoyalFlowers]

Hi Mr. Peterrozenewman,

Thank a million again for your informative answers.

1) For Adjust to touch method, I am going to check output file and try to move load applicator with the same values in X,Y, and Z, and then will use add offset-no ramp option. It is worth mentioning that before when I used add offset-no ramp, offset value was 0 because I was not sure about the exact offset value to adjust contact area and also I wanted that load transfers between target and contact surfaces when they are in touch because of load.

2) In this model according to following picture, the remote point (which is our loading center) had free rotation around y axis and free displacement along z axis and this degrees of freedom were applied with defining remote displacement for remote point. The remote point is coupled to the upper surface of plate and axial load is applied on that.

In the experiments also we had the same loading conditions. To compare results with experiment, z displacement of the remote point was compared with experiment. Also we had some markers on fracture fragments and their displacements were also compared with experimental values.

Distal boundary condition is as followed. the highlighted faces were defined as a fixed support.

 

If we compare video of displacement between load applicator and main body, parts move similar to experiment when adjust to touch option is selected for contact between load applicator and bone. Hence, it seems that contact finds its realistic position with this option but with selecting add offset-no ramp (offset=0) load applicator and bone did not move as same as experiment. Because of that I thought that adjust to touch option could be accurate for this contact situation. Please correct me if it is wrong.

I am really grateful again for your advice in this discussion.

Best regards, Shabnam Samsami

 

[RoyalFlowers]

Dear Mr. Peterrozenewman,

Regarding your last comment I posted a reply in 3 days ago, and would be grateful for your reply in this regard because still I doubted that which interface treatment algorithm should be selected and what is our justification for that.

Best regards, Shabnam Samsami

[peteroznewman]

Dear Shabnam,

Sorry I missed your post 3 days ago, once the discussion has been marked Solved, I may miss a new post.

If adjust to touch gives you good results that match experimental data, that is a good reason to use that adjustment in the model. I am glad to see that the remote point has the correct degrees of freedom that match the experimental setup. That is also very important.  It looks like you have a final result you can trust.

Best regards, Peter

[RoyalFlowers]

Dear peter,

First of all thanks a million for all of your illuminating answers, they were really helpful for me to know more about Ansys theory. Also, I am so glad about finding such a useful website to have a chance for FEM discussions. This model is really complicated but I learned with that without experimental data we are not able  to select the most accurate FEM assumptions. I checked the Is Solution option. wishing you a great weekend.

Best regards, Shabnam