Learning Forum

[TomPhemmy]

How can 3D line to line contact be generated between beams in ansys workbench? I have tried to do this by selecting the lines representing the centriod of the beams but it doesn't work as seen in the attached picture. The help section mentions that CONTA 176 and TARGE170 have to be mapped on the surface of the beams to established contact between them. How can I do this in the workbench environment?

[Sandeep Medikonda]

Hi Thompson,

  Did you mean CONTA177 elements? According to the manual: 

3-D line-to-line contact is represented by following the positions of lines on the contact surface, modeled by CONTA177 elements, relative to lines on the target surface, modeled by TARGE170 elements.

Can you open the solver files directory by right-clicking on the analysis type and look for what contact elements are being generated in the ds.dat file?

Regards,

Sandeep

[TomPhemmy]

Hello Sandeep,

From my understanding of the contact technology guide, the element you are referring to CONTA177is used to model line-to-surface contact. The contact i seek to model is line-to-line contact between beams where the beams geometry have been modeled in designmodeler as shown below.

Regarding your second comment, no contact elements where generated:

--- Number of total nodes = 4345
 --- Number of contact elements = 0
 --- Number of spring elements = 0
 --- Number of bearing elements = 0
 --- Number of solid elements = 2145
 --- Number of total elements = 2145

[TomPhemmy]

Also, I notice that when i use solid bodies, WB Mechanical automatically detects the contacts but when i use line bodies (beams) it does not detect the contacts.

 

[peteroznewman]

Hi JJ,

Here is a relevant post. In that example, all the beams were in a straight line arranged in a checkerboard pattern, one beam could be the target-side of the pair but only its four neighbors had to be considered contact-side beams.

The problem you have is that there is a many-to-many contact condition. This kind of contact is automatically and easily handled in Explicit Dynamics, with a Body Interaction. So the contact issue becomes simple, but getting useful results from Explicit Dynamics is more complicated than Static Structural for example.

What is you simulation goal?

Regards,

Peter

[Sandeep Medikonda]

Hi,

  According to the manual CONTA177 element handles both beam-to-beam and beam-to-surface contacts well and is recommended.

Contact between beams undergoing large displacements can be encountered in many practical applications. Some examples are hydrogen sensors, water supply lines, nuclear power plant piping, cable wires and coils, woven fabrics, and tennis racquet strings. You can model 3-D beam-to-beam contact by using the 3-D line contact element, CONTA177.

Following are alternatives to using CONTA177 elements:

• Use 2-D surface-to-surface contact elements, CONTA171 and CONTA172, to model 2-D beam-to-beam contact (see Surface-to-Surface Contact (Pair-Based)for more information).


• Use the 3-D line-to-line contact element, CONTA176, to model 3-D beam-to-beam contact. CONTA177 is the preferred element because it is more versatile and can model both beam-to-beam contact and beam-to-surface contact.

Chapter 5.3 in the Mechanical APDL Contact Technology Guide has a very similar example:

 

Regards,

Sandeep

 

[TomPhemmy]

Hello Peter,

I would like to extra the contact stresses (normal and tangential) at some of the contact interface when the cable is subjected to axial tension and bending. As you suggested, explicit dynamics generates the contact automatically for line bodies. But as you mentioned, how easy is it to access this contact information? it is easier to obtain in static structural.

I suppose the way out is to go through the APDL native interface.

 

[TomPhemmy]

Hello Sandeep,

Thank you for this. I'll look at generating the contacts using the native APDL interface.

 

[TomPhemmy]

Hello Peter,

Thank you for your previous suggestions.

I decided to try out your suggestion on using Explicit Dynamics. I applied a displacement boundary condition (1.2mm) on one end of the cable and fixed the other end putting the cable in tension. I set the end time in the Analysis settings to 0.1 and simply ran the simulation leaving other settings at their default values. After solving, deformation contours are available (as below) but stress and strain contours are not.

 

I would like to know what is wrong with the simulation settings since this is suppose to be a static analysis and not dynamic. I guess my question is how to perform a static analysis in Explicit dynamics solver.

[Sandeep Medikonda]

Thompson,

  Explicit analysis by default is a transient analysis, i.e., it solves the full equation of motion: Mu(double-dot) + Cu(dot) + Ku = F; So it by default includes the mass and subsequently the dynamic effects of the problem (short duration problems and high inertial effects). Since this equation is often hard to solve for complicated problems with the Newton-Raphson method, we solve it explicitly with a central difference method. 

  The static analysis, on the other hand, does not consider the effect of mass (inertia) or of damping, hence it only solves Ku = F and we do solve this implicitly using the Newton-Raphson method. One of the challenges here is that we invert the stiffness matrix once or even several times over the course of a load/time step. This matrix inversion is an expensive operation, especially for large models. Explicit doesn't require this step.

One of the limitations of using an explicit analysis is that the time step must be less than the Courant time step (time it takes a sound wave to travel across an element). Static and Transient implicit analysis have no inherent limit on the size of the time step. As such, implicit time steps are generally several orders of magnitude larger than explicit time steps.  

  Coming to your problem, can you show us some more details/snapshots on how you are setting up and loading the model, setting up contact etc?

Regards,

Sandeep

[TomPhemmy]

Hello Sandeep,

Thank you for your detailed explanation especially regarding time stepping in both solvers.  I have attached images below to show how I applied the fixed boundary on one end of the cable. This fixed boundary condition is applied to the nodes at the end since the elements used in this model are beam elements.

The displacement boundary condition at the other end is as below applied in the negative Z direction to create tension from 0 to -0.5mm to -1.2mm and also applied at the nodes.

The contact conditions are left at the default and not changed (see below)and the material is also left at the default structural steel because I am just trying to get a feeling of how the solver works before using my own material models and contact.

 

 

 

 

All analysis setting were left at the default value other than the end time (0.1s) which was specified as below:

 

Is there anything else I should provide?

Regards,

Thompson

 

 

 

 

 

 

 

[Sandeep Medikonda]

How about the Mesh and the elements you are using? Is this a 3-D model?

Can you try using the contact tool s discussed here and see if you are able to see initial contacts? Check the Status and the gap, adjust the pinball radius as needed?

P.S: In the future, please create a new discussion and provide a link to your old discussion. Especially when you are doing your analysis using a different solver. Solved questions and long threads tend to get less attention and slower help.

Regards,

Sandeep

[TomPhemmy]

Hello Sandeep,

Yes it is a 3-D model. The meshing is done 3D beam elements as below:

 

 As you can see also below, the model type for the line bodies are set to beam

 

From my understanding of what peteroznewman mentioned earlier about automatic contact generation in the explicit solver, i didn't bother to set up contact manually. The body interaction connections are active showing that the contacts have been detected automatically by the solver. Generating initial contact using the contact tool doesn't work for body interactions under the connection folders as shown below:

 

so I cannot check the information you requested I check.

 

Regards,

Thompson

 

 

[Sandeep Medikonda]

Thompson,

Note that the beam element used in Mechanical does not apply in Explicit Dynamics. A few comments on beam element in Explicit Dynamics:

• 2 noded Belytschko -Schwer resultant beam formulation 


• Extended to allow large axial strains


• Resultant plasticity implemented for range of cross section types


• Cross-section is a parameter (not modelled geometrically)


• Actual cross section can be rendered.


• Time step is controlled by the element length, not Time step is controlled by the element length, not by dimensions of cross-section.

In your model can you try to turn on Beam Section results to Yes and see if it works:

~Sandeep

[Sandeep Medikonda]

I also see that you are using a Trajectory contact, change that Proximity Based Contact which will account for the Edge to Edge contact of the beams. Once you make this change note that you can also change the Pinball Factor. 

Regards,

Sandeep

[TomPhemmy]

Hello Sandeep,

Many thanks for your help. I have not being able to resolve the problem even after changing the contact setting to proximity and activating edge to edge. Beam section results have also been set to yes and it still didn't work. Some questions I have:

1.

In your statement above, what do you mean by resultant plasticity? In the explicit documentation, it says the 2 noded Belytschko -Schwer beam must be used with linear elastic material properties.

2.

Also, I saw that information about contacts are not written for this element. Is this true?

3.

When using solid elements in explicit dynamics, contacts are detected by the automatic generation as body interaction and also the contact tool detects contact (i.e. contacts similar to that of the implicit solver). The explicit solver refused to work when I had both "contact" and "body interaction" active but solved when I suppressed the contact tool (see picture below). Does this mean that one can only use of one of these two contact definition methods in the explicit dynamics environment?

 

4. I have the von mises stress contour on a cable as shown below. What if i am interested in just the von mises at a section of the cable (say mid-length), how can I display this on the contour plots? Currently it shows the stress contours for all bodies.

 

Regards,

Thompson

 

 

[Sandeep Medikonda]

Thompson,

  I am not sure where you see that in the manual, can you point it to me? I ran a simple case with plasticity added and it worked.

  Yes, I don't think you can use both as it would make it redundant. Also, can you double check if you turned on edge-to-edge contact.

Lastly, you can get a section view as shown below:

Regards,

Sandeep

[TomPhemmy]

Hello Sandeep,

I am referring to page 146 of the explicit dynamics analysis guide (see below):

The statement you earlier made i have underlined in blue and the my statement in red. What does the statement resultant elasto-plastic response mean?

I am also kind of curious, the picture of the analysis you posted above, did you use beam elements? I have tried to reproduce something like that without contacts but the von mises stresses are still not visible which shows the contact setting is not the problem. Beam section results were also set to yes as shown below

 

 I basically get zero maximum and minimum which cannot be the case since deformation occurred as shown below

 

If nonlinear materials are supported, i will like to stick to using beam elements, and if not I will change to using solid elements. Also, what do you think is wrong with my settings (have a look at my project tree?) since you were able to get the stresses for the single beam model.

 

Lastly, regarding displaying section results, I can view sections as you showed above and scope results on bodies but this is not what i want. I will attach a picture of the simulation of a former student to explain what I want. The first picture below is the normal stress for the whole cable at the mid-length. How can I get the stress bar (circled in red) to display values ONLY at a given section?

 

Also, how can I get the stress bar to to do something like below, where other bodies are hidden and stresses on the stress bar indicate those of only the active bodes. 

Regards,

Thompson

 

 

 

 

 

 

 

 

 

 

 

[Sandeep Medikonda]

Hi Thompson,

  That could possibly be a defect in the documentation. Elasto-plastic response refers to the non-linear behavior of materials where plasticity can be included. To view the beam stresses, you would have to use the worksheet and use the following user-defined variable:

Note that there are limited results available to scope here that will work for beams.

You can always use the section plane and you need to select on the solid line so that it turns into a dotted line on both sides to see just the section.

You can always increase the no. of points or the limits by using the +/- on the legend or just clicking on a value and typing in the desired value

Also, to view results on only certain bodies you need to change your scoping geometries. So change it from All Bodies to only those outer bodies.

Now, I often get confused when you show the von-mises stresses on the bodies. So I am assuming those are from a different run of another student right?

There is clear variation in the through-thickness direction of these bodies, if you want to replicate this I think you would need to model these using the solid elements.

Regards,

Sandeep

[TomPhemmy]

Hello Sandeep,

Thank you so much for your time and effort! The stress results are finally visible.

Yes you are right, the results are from another student's run who used solid elements. I want to see the difference in terms of estimating the contact pressures using beam elements and solid elements. Do you have an idea how the contact forces (normal and tangential) will be influenced if I used either elements? 

 

I have some other questions:

 I am getting severe penetration at the mid-section of the cable (see below), Do you know what the cause is? My contact settings are also shown below

 

 

The selected pinball factor is too small; I am aware. The manual states 0.1-0.5 but when i used 0.1, it didn't solve the problem.

Regards,

Thompson

[Sandeep Medikonda]

Thompson,

  The manual does specify that Initial geometry/mesh must be defined such that there is a  physical gap/separation of at least the contact detection zone size between interacting nodes and faces in the model. The solver output will give error messages if this criteria is not satisfied. So this may not be practical for very complex assemblies. Having said that I would recommend you to try the following:

• Decrease the Timestep Safety Factor to 0.1 or even 0.05.


• Refine the mesh in direction of the length. I suggest this because of the way contact is detected in this algorithm:
  
  So, once a node enters the green zone (gap defined by pinball factor) a penalty based force is calculated and applied to the offending node. Since you are dealing with line bodies that are almost parallel it is very likely that contact is being missed.


• Frictional coefficient seems to be too high, is this correct?


• The manual does suggest a factor between 0.1-0.5, so what is the problem you are having when you are solving this? What is the error message?


• Try a case without the edge to edge contact and also a case using trajectory contact, just to see the effect that edge-to-edge contact is having on the results.


• Turn on Body self-contact and Element self-contact (to yes). Although I don't think this would have a big effect, you can never be sure if the twisting is high in the region in the middle especially with a refined mesh.

Regards,

Sandeep

[Connormead]

Hello sandeep, kindly assist me with detailed manual on CONTACT and PIPE for pipeline designs. .
Thanks