contact with shell elements on midsurfaces

[g.ceruti]

Hi everybody, I'm testing the NIC contact with shell elements on midsurfaces.
Does someone know if NIC take in account the thickness of shell during the contact solution?
or in other words, do shell elements become in contact only when their midplane intersect?

I am testing two simple alluminium cantilever beams (2mm thick, 45mm wide and 100mm long), with a 2.5mm gap between them (see attached picture).

When loaded, the upper beam should bend, cover the 2,5mm gap, touch the lower one, and then both beams should bend together.

If I solve the model with 3D tetra elements and a manual separation contact (max activation distance is set to 3mm > 2.5 gap) it works fine, even in a linear static analysis.
In a Non linear analysis I can follow up the evolution of the contact solution, the touching happens at 90% of my load, and get a final result very similar to the linear analysis.

But, when I try with midsurfaces and 2D shell elements, the separation contact does not work, and the upper beam bends trough the lower one likewise when the contact is not active!

It happens with both linear or non linear analysis, with both linear or parabolic shell elements, and even if I increase the max activation distance to 5mm > 4.5 mm gap between the midsurfaces.
I also tryed with different mesh size, or increasing the load (so the upper beam bends more than the 4.5mm midsurfaces gap) without any result.

in 3D case the contact set up is the following:

    the bottom surface of the upper beam is the slave surface
    the top surface of the lower beam is the master surface
    surface to surface
    contact type: separation
    unsymmetric penetration
    max activation distance actived and set to 3mm (>2.5mm gap bewteen solid)
    default values for all other data


in 2D case the contact set up is the following:

    the upper mid-surface is the slave surface
    the lower mid-surface is the master surface
    surface to surface
    contact type: separation
    unsymmetric penetration
    max activation distance actived and set to 5mm (>4.5mm gap between midsurfaces)
    default values for all other data

Note that if I switch the 2D contact to a bonded contatc, it does not work with max activation distance set to 3mm, but works fine with 5mm

I attach my test model in the zip file.

I'm using NIC 2018.0.1.189 (with hotfix1). I had to downgrade to this version beacuse the latest 2018.2 always crash.

[John_Holtz]

Hi @g.ceruti. Welcome to the In-CAD forum.

There is something going on with the midplane model that I do not understand, so I need to do some more tests. However, I do know the following:

1. Since your midplanes are separated by 4.5 mm and the top beam is only displacing 2.78 mm, they are not in contact ... if contact is defined as when the midplane meshes touch. 
2. The two midplane (shell) plates are definitely not passing through each other. (Because the displacement is usually small in a linear analysis, the displacements are exaggerated by some factor which can be larger or smaller than 1. By changing the exaggeration factor, you can make it look as if the parts pass through even if they have not moved far enough to some into contact yet.)
3. The normal direction of the shell elements need to be facing each other in order for the contact to be detected. I suggest that you reverse the normal direction of the bottom plate. (Right-click on Elements in the model tree and choose "Reverse Direction".)
4. The maximum activation distance is not related to how close the nodes are when contact occurs. That is controlled by the input "Penetration Offset Distance". Contact elements are created between nodes at time 0 (before there is any displacement) that are closer together than the maximum activation distance. Only those nodes can come into contact. Whether they come into contact depends on the displacements when the loads are applied.

In theory, you want to set the penetration offset distance. What confuses me is that changing the penetration offset did not work like I expected it to. I will do some more tests to see if I can understand what is going on.

[g.ceruti]

thank for your quickly replay John,

Hereafter in greeen you can find some other my considerations:

---

@John_Holtz wrote:

Hi @g.ceruti. Welcome to the In-CAD forum.

There is something going on with the midplane model that I do not understand, so I need to do some more tests. However, I do know the following:

1. Since your midplanes are separated by 4.5 mm and the top beam is only displacing 2.78 mm, they are not in contact ... if contact is defined as when the midplane meshes touch.
   • This was my dubt!!
   • the 2D shell model displaces 2.78mm, likewise the 3D solid model but with the contact disabled (2.77mm), that is close to the thoeretical solution for a cantilever beam with a tip load d=(P*L^3)/(3*E*J)=2.90mm
   • the 3D solid model works fine, the 2D shell model should lead to the same result!
     
2. The two midplane (shell) plates are definitely not passing through each other. (Because the displacement is usually small in a linear analysis, the displacements are exaggerated by some factor which can be larger or smaller than 1. By changing the exaggeration factor, you can make it look as if the parts pass through even if they have not moved far enough to some into contact yet.)
   • You are right, but I have checked my result with a true scale factor set to 1, and I have also checked the numerical values
   • if I double the load, the 2D model passes through without caring of the contact interface
3. The normal direction of the shell elements need to be facing each other in order for the contact to be detected. I suggest that you reverse the normal direction of the bottom plate. (Right-click on Elements in the model tree and choose "Reverse Direction".)
   • I tried your suggestion, but it works only if I increse the load upto 30N (corresponding to a free deflection of 4.5mm)
   • Therefore my conclusion is that NiC does not account for shell element thickness in solving contact problem. it's another big deal.
     
   • what is your suggestion if I have another beam under the lower one? Where do middle plate element normals point to?
     
   • 
     
4. The maximum activation distance is not related to how close the nodes are when contact occurs. That is controlled by the input "Penetration Offset Distance". Contact elements are created between nodes at time 0 (before there is any displacement) that are closer together than the maximum activation distance. Only those nodes can come into contact. Whether they come into contact depends on the displacements when the loads are applied.
   • I agree with you, that the maximum activation distance is useful to find the hypothetical contact interfaces at time 0, than the iterative solution deicdes which contact elements close
     
   • This article suggests, in case of manual separation contact, to increase the maximum activation distance upto the minimum nodes distance such that a "slave node" can find some "master nodes" to define the contact element.
     So, the maximum activation distance should be related to mesh size too, besides the midsurfaces distance.
     

     https://knowledge.autodesk.com/support/nastran/learn-explore/caas/sfdcarticles/sfdcarticles/Understa...

   •  I tried to increase the maximum activation distance up to 10mm (mesh size 5mm) but without reversing the lower plate shell element normals it does not work anyway

In theory, you want to set the penetration offset distance. What confuses me is that changing the penetration offset did not work like I expected it to. I will do some more tests to see if I can understand what is going on.

I think that the penetration offset distance is something related to how far nodes shall move away to consider that the contact element is opening or in contact during the iterative solution. But I am not sure, maybe I read something but I donn't remember where.

---

[John_Holtz · Accepted solution]

Hi @g.ceruti

I agree with all of your statements (in green) except for the penetration offset. The Penetration Surface Offset tells the solver where the "contact surface" is relative to the mesh. Another way to think of it is that the Penetration Surface Offset adds material to the contact face, so it reduces the gap between the parts.

For shell elements, you can enter a Penetration Surface Offset equal to (shell 1 thickness + shell 2 thickness)/2 to account for the thickness of the shells.

The attached image "solid vs shell.png" shows the same analysis setup using four different methods: two methods use solid elements, and two methods use shell elements. (The shells in my example are from a midplane, but they can be created from any method.)

• The top two methods use the defaults, so the gap is different because of the shell thickness.
• The bottom left method uses a penetration surface offset distance to reduce the gap between the parts. Of course, if the penetration surface offset is equal to the gap, then you have reduced the theoretical gap to 0.
• The bottom right method uses a penetration surface offset distance to compensate for the thickness of the shells. This method will give the same results as the top left method.

Note that the "extra material" added by the penetration surface offset in my image is not real material, so it does not change the stiffness of the part. The "material" is just my explanation of how to visualize it because it is easier than trying to explain the real mathematics.

Sorry the image is messy. There is probably a better way to make to present the idea, but this is what I could do in the time available.

For your question about a stack of 3 shells, how can you have contact from both sides since the normal direction can only face in one direction? I have not tried it, but I have heard that if you have contact on the positive normal side, the solver should detect the contact on the negative normal side. So the normal directions would look like this:

[g.ceruti]

thanks again John,

so just to resume, for midsurface shell elements:

• NiC does not automatically account for shell element thickness in solving contact problem
• max penetration distance must be set at least as the geometrical distance between midsurfaces
• penetration offset distance must be set as half of sum of the contacting thicknesses

Non linear static analisys provides at 99% the same results for both 3D and 2D midsurface models.

A simple linear static analysis provides more rough but similar results.

I also tried it with a three contacting plates, and it works fine!

[Richard_Stubbs]

Hello @John_Holtz,

I have been searching for a few days now for a solution to a problem I am facing and have not been able to find an answer. This thread is about as close as I have got so appologies if this is not the correct way to seek advice.

Can a geometric gap be modelled using separation contact between shell and solid elements?

Thanks

[John_Holtz]

Hi @Richard_Stubbs . Welcome to the Inventor Nastran forum.

Yes. You can define contact between shell and solid. This is what you need to be aware of:

• Shell elements only detect contact on the "top side" of the shell. Contact is not detected on the "bottom side" of the shell. Therefore, you need to check the normal direction of the shell and make sure the top side is facing the solid. (Display the normal direction by right-clicking on Elements in the Model Tree, then "Normal Display > Vector". The arrows must point toward the solid. Reverse the direction if necessary using "Elements > Reverse Normals".)
• The maximum activation distance needs to be large enough to account for the gap (and mesh size if using manual contact; only the gap if using solver contact). See tips 18 and 19 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum.

John