When to ignore contact in FEA?

Linear FEA calculations are the most common type of static analysis done with finite elements. So far we have discussed when it is safe to ignore material nonlinearity and when to ignore geometric nonlinearity. Ignoring those aspects allow you to use linear analysis which is a simple yet robust tool. There is another thing we should consider: contact in FEA!

A short remainder

Linear FEA is great – simple, computing is faster, far fewer problems that with nonlinear FEA, more software can do it (nowadays it is even integrated into CAD software!). A lot of benefits right?

But of course, everything has a price. It this would be a “perfect” solution this would be the only analysis type right?

The “price” in the case of the linear analysis is the “linear” part. It is fair to say that here I discuss linear static (as opposed to dynamic) and this is also a drawback – I simply won’t deal with it here.

Most notably “linear” mean that you don’t take into account various nonlinearities. I have listed below what I mean by this.

I’m well aware that different sources define what is nonlinearity differently. This is the list I personally believe in:

  • MaterialMaterial nonlinearity is a “poster boy” of nonlinear analysis. This thing alone is awesome, there are many material models available and a lot of settings needed. It is good to know when you can ignore this effect and simply use the linear material. I have already addressed this here.
  • GeometryNonlinear geometry is not as popular as material nonlinearity I think. It is more subtle and it is actually a bit harder to describe its influence. Still, it is there, and if you are doing a buckling analysis this is very important. Of course, not every analysis involves such topics, so it is good to know when to omit this nonlinearity. I have discussed this here.
  • Contact – this is a tricky one. Depending on the source you may have issues to determine if contact is always nonlinear, or can it be linear as well. I won’t take part in the discussion about definition – I hate argues about semantics! Whatever side of the fence you will take, contact in FEA can be nonlinear – so we will try to answer when ignoring it makes sense.
  • Follower forces – this is a relatively small thing. If this is a “nonlinearity” at all again is a discussion I would say. If we will “clear” geometrical nonlinearity we are certain that deformations in the model are small. In such cases, it doesn’t really matter if the loads follow the shape of the geometry or not. This would play a role in geometrical nonlinear analysis, but we are staying in the linear zone today.

We have already dealt with material and geometric nonlinearity (and follower forces on our way). It is only logical to discuss contact next.

What is contact in FEA?

This is an interesting problem. In general, contact is a situation where 2 objects touch each other… great right? A really nice definition…

I think we should divide contact in FEA into 3 categories:

  • Our model “contacts” support. This is the “easiest” case I think. Such contact would be between a book lying on the table, and the table itself (assuming we want to analyze the book). You may also have a steel column standing on the concrete floor – this is a bit more complex thing but we will get there 🙂 Contact between steel column and concrete floorNote that we are not interested in designing the concrete floor… only the steel column is of interest.
  • Two parts of out model “contact” each other. This is another possibility. Somehow I’m always drawn to steel structures, so this can easily be an end-plate bolted connection. This is a more complex case, but still doable.Contact between 2 steel beamsHere we want to analyze both beams (or beam and the column as can be seen below). This is a bit more complicated situation. Still, we will be able to avoid contact definition, at least in the simplified calculation.Contact between steel beam and steel column
  • Part of our model can touch itself. This is bad. In the case of such analysis usually, it is impossible to avoid contact… Good thing is that if you are doing something complex like that… you most likely know what do to anyway 🙂Self contact of a simple element

 Is contact with the “ground” a support?

The first case (column on a concrete floor) seems obvious right? I mean you would automatically assume this is a “normal’ pinned support.

Such reasoning is correct in many cases. However, there are several considerations you have to make:

  • I have intentionally left the screws out from that first drawing. This is not a practical case, but it should show you something. If the uplift (tensile) force appear, there is no connection. What would happen is that in reality, the column would move upward. But in the model with a support, you would get a reaction force from such action. It is then important to check if there is such reaction force for any possible loads. If so, you need to analyze that separately without the support in place… or use contact there.
  • If you add screws you can actually create rigid (or more likely semi-rigid) connection. It is easy to assume pinned joint especially when you are using a beam model. However, there is a possibility for a pair of forces between screws and the contact between column and concrete floor.Semi-rigid connection with contactThis is another consideration. You don’t control where the contact will happen. The model will choose that on its own. So if you are trying to make this a support, always consider if a connection is pinned or not.
  • In shell model, you cannot support entire outline in the vertical direction. This is an easy mistake. Even if entire column stands on concrete, this is likely that the connection won’t carry any bending moment. If you support entire outline in the vertical direction, it will. Again this will be shown as a tensile reaction force in part of the support. Be aware that you cannot carry such reaction force.
  • Contact in FEA model may be connected with friction. If there is a shear force you wish to carry you can manually check if it is ok by multiplying the compressive load with friction coefficient. If the value is higher than the shear load (which different safety factors depending on your code) you are good to go.
  • Exchanging contact to the “ground” for a support can be a complex problem. You can learn more in the series of posts about connection rigidity I have made some time ago. You can find what you need here.

To sum this up, you can ignore contact to the “ground” in following cases:

  • You are certain there is no lifting force in any possible load combination in any point of the support
  • Support rigidity was consiederd for the beam model
  • You have checked that if shear is transferred by friction, capacity there is sufficient

But what if contact is between elements that you wish to analyze?

This is a more difficult issue. Let’s say you have a beam and a column connected together and you want to calculate both accurately. You have made a shell model of the connection and now you wonder what to do with the contact. The advice above will do you no good… substituting one of the elements for the support is a stupid idea in such case.

There is hope, however, if you can predict where the contact will take place! Imagine a connection like this:

Simplified solution for contact without contact :)

If the bending moment will always be in this direction, and the flange and end plate are stiff enough you can work around this. Instead of applying contact you can simply connect the top of the end plate with the column. Just use a horizontal plate for this:

Simplified way of introducing contact without contact

What you gain is, that instead of a proper model (on the left below) you get a simplified model (on the right below). If the plates are rigid enough those should give you similar values.

How to avoid contact in a simple connection

As with everything such tricks can be done only in certain cases:

  • You need to be able to predict where the contact will take place
  • You need to have bending only in one direction
  • Planes must be rigid enough

What can go wrong?

If you are substituting contact with simplifications as this additional plate several things can go wrong. All of them are foreseeable, and also you can check some of them in post processing.

  • You have predicted wrongly where the contact takes place. This is the worst one, and hardest to check. If the model you have deforms in reality in a way you haven’t foreseen you are in trouble. The easiest way to prove it is to show it. Take a look at the end plate of the beam connected to the column:Ideal situation in contact simplification In ideal scenario end plate is so rigid that the mechanism above simply works. In such case, it is very easy to foresee where the contact point is and where to use this additional horizontal plate to connect end-plate with the column flange. But what if the end-plate is not rigid enough? Then something like that happens:Not so ideal situation in contact problemThis is serious as the force will be applied “lower” meaning that i.e. resulting tensile force in the screw will be higher. This is a tricky situation and if I would notice that in my model the end plate deforms I would use contact just in case. If the end-plate remains flat you should be ok. Just remember that the mechanism above is not the worst one… if yielding of the end-plate is a possibility using contact is unavoidable:Note how much plate is in contact… such case can’t be modeled without contact properties.
  • You have bending in 2 directions. Bending is only one of the possibilities of course… by this I mean you have a load that makes it impossible to accurately predict where contact takes place… in such case you need to use contact. If you missed it you will easily notice that in post processing, as the stress in this “additional horizontal plate” will not be constant along the width of the plate. It should be.

Summary

Wow, this is the longest post to date I think! I hope you enjoyed it!

I used steel structures and connections simply because they are easy to draw, but the principles remain the same. Everything I have written today can be summarized in 2 sentences more or less:

You can treat contact to the ground as a support. Just check if you haven’t got any tensile reaction force there… that would be bad. You can learn more about it in the video below.

If you can accurately predict where the contact takes place, you can substitute it with some additional elements that will carry compression. Adding those means you won’t have to define contact properties.

Video with a case study of contact in FEA:

Want to learn more?

This is great! I have a free nonlinear FEA course just for you! Subscribe below to get it!

If you enjoyed the post you can share it with friends – that would be a great help! If you have a spare 15 seconds write a comment with your thoughts on the matter or any questions you might have. I have a good history of replying to each and every comment 🙂

Free nonlinear FEA course!


2 Comments

  1. Ivar KJELBERG March 22, 2019 at 9:43 am - Reply

    Hi Łukasz

    Nice post, and many illustrative cases you describe here.
    One thing I did not really get, do you use “gap” elements here ? or how do you arrange these contacts, to make them reasonably low computational costly, but still representative …

    Sincxerely
    Ivar

    • Łukasz Skotny March 22, 2019 at 2:17 pm - Reply

      Hey Ivar!

      I’m not sure what do you mean by “here”… In most examples, I simply used a plate to “mimic” contact. But if you mean in the video, we used “normal” contact there.

      Gaps aren’t all that bad though. Femap has a nice button that arrange them for you if you are careful with meshing (it simply connects closes nodes) – not a bad feature, but I assume many software solutions has that ; )
      All the best
      Ł

Leave A Comment

Do NOT follow this link or you will be banned from the site!