mesh thin body

  • Last Post 2 weeks ago
nyla posted this 3 weeks ago


My simulation involves the transmission of a force among bodies of different measure (cm and mm). In particular, in this the following figure you will see the mesh of bodies (0,7 mm element, linear, adapative mesh )


After simulation I get the following deformation

deformation of PDL

as you can observe the dark blu bodies which envelop the teeth will damage during the dormation process and holes appear on thei surface. Probably the fact is that the thickness of these bodies is 0.3 mm which is smaller than the element size used for meshing. But a reduction in the element size creates doen't provide any solution due to the elevated number of nodes. Thus, I want to create multiple elements within the wall of the bodies, but since the geometry is quite complex mesh sweeping doesn't work (if I select manually the source it keeps to be yellow, unselected) and to create a midsurface I've tried to use virtual cells (virtual topology) by merging all the external faces in one and all the internal faces in the opposite one in order to apply a sweepable mesh, but no chances to work (see image).

failure during sweeping mesh of virtual cells

Any other tips to solve this issue and get a proper deformation?

Thank you!

Order By: Standard | Newest | Votes
peteroznewman posted this 3 weeks ago

You can only create a midsurface if the wall thickness is uniform.  Is it?  Can it be assumed to be a uniform thickness?  If so, there are geometry editing techniques to create a surface to replace the thin wall bodies. I recommend you do that so you can mesh the surfaces with shell elements.

nyla posted this 3 weeks ago

Hi Peteroznewman I can say that the wall thickness is 0.3 mm, what do you mean by uniformity? the surface is a bit irregular and there is  a plenty of faces, thus I cannot select each pair of face there another way?

Thank you!

peteroznewman posted this 3 weeks ago

What do the faces look like in the Geometry editor? In SpaceClaim, you can copy the faces of a solid and paste them to create a surface.

nyla posted this 3 weeks ago

Hi Peteroznewman,

thank you for your advise. Sorry for the delay, but I've just managed to solve a problem with the Space Claim "the geometry editor was closed abnormally" and now it works well.

The object is a solid body with a lots of faces which in the DM look like in this picture.

appearance in design modeler

I've tried to do what you suggested thus in Space Claim I've selected all the faces in the exterior of the object, copied and pasted to create a surface and I've done the same for the inner part, thus two surfaces have been created, discarding the upper border of the object that is the circular faces you can observe from the top. However if I check the midsurface command I'm not able to get the result, nothing happens. Look at the picture.

midsurface attempt

Before doing this I've also tried to do the merge of all the faces but problematic geometry errors arise. 

Could you please help me?

peteroznewman posted this 3 weeks ago

You keep one surface, say the inner surface, and when you assign thickness to that surface in Mechanical, you can set it so the material is all on one side of the surface.

  • Liked by
  • nyla
nyla posted this 3 weeks ago

ok, so just to recap what I've done... I've creted the inner surface from all the faces than I uploaded the Mechanical model and I assigned a thickness of 0.3 mm (since it was the orginal wall thinckness of that ligament, should I enter a lower value?). 

During connections I've creted two contacts which share a common surface that is this thin wall surface. Honestly, contacts should be different since one is between the tooth and the inner side of the ligament and the other is between the outer side of the element and the mandible. I wasn't able to detect inner and outer wall since I had only one side. see the images of the two previous contacts respectively.

first contact -inner side of ligament and tooth

second contact- ligament and mandible

First of all, I'm not sure about this fact, secondly during the meshing process I wanted to have larger element size (0.7) for larger object and smalle element mesh size (0.007) for the element of interest such as this thin wall structure and the contacts region with other bodies. Thus, the following image show all the settings for the mesh


The automatic method allowed me to creted quad elements for the thin wall surface, but from the picture I can see that in the thickness of this thin wall structure there is just one element, thus Iìm not sure it works well. Patch Conforming was to guarantee a proper mesh within smallest regions and contact sizing was to guarantee the nodes of the interfacing bodies are overlapping at contact region.

However, the solution process is quite heavy and I don't think I did all the process correctly. What do you think?

peteroznewman posted this 3 weeks ago

A surface has two sides, a top and a bottom side.  You can create a contact of the top side to the body next to that, and you can create another contact of the bottom side to another body next to that.

  • Liked by
  • nyla
nyla posted this 3 weeks ago

You're right I'm sorry! Just to be sure.. when importing the inner surface into Mechanical I set the thickess value of 0.3 mm with top offset type because the mesh appears as it there is the real ligament (with the actual thickness) as in the figure below 

mesh of the shell with an offset to the top

 , however during connections when I choose the bottom surface to create the contact between the exterior wall of the surface and the mandible I'm not allowed to select the thickness option(figure 3). Why? I tried to use this command "keyopt,cid,11,1" to force it.

Regarding the contact between the top side of the surface and the tooth I don't select the thickness option since I chose the inner surface as shell that is actually in contact with the tooth.

inner surface import into Mechanical

contact between bottom side of inner surface and mandible

After solving I get this result for the stress distribution, as there is no transmission..

von Mises stress considering on offset of top surface

Moreover,I know that to represent the thickness of a thin object a minimum of two mesh elements should be created in the depth, but I have only one, even if I set the minimum curvature value to 0,05. While if I set the offset to middle and the shell element thickness to yes for both the contacts I get this mesh representation where it seems that there is a region of overlapping between the inner side of the surface(the top) and the tooth, thus I don't think it is correct, but there are two elements. 

mesh with offset to middle



peteroznewman posted this 3 weeks ago

I can correct one piece of your understanding when you say "to represent the thickness of a thin object a minimum of two mesh elements should be created in the depth" that is true for solid elements, but that does not apply to shell elements.  This is the benefit of shell elements, the element itself has internal equations to support bending of the element, which solid elements do not. That is why you only need a single shell element on the surface, and why you can get a good reduction in model size compared with putting solid elements on a solid body.

When looking at section views, click the button to show full elements, and not section individual elements. That makes it easier to see what is going on. When the elements get sectioned, there are extra lines drawn that are just confusing.

Read the ANSYS Help system to see what it says about the shell thickness effect. I don't know and haven't read the help myself. I don't often use offset shell elements. In Geometry, you could try to offset the inner surface by half a thickness to get a midsurface.

  • Liked by
  • nyla
nyla posted this 3 weeks ago

Hi Peteroznewman,

thank you for your tips.  I've realized the midsurface by offsetting the inner surface (even if the offset was not uniform) this allowed me to select the Middle type offset and activate the shell thickness effect, this way the contact is detected at a distance of half the midsurface's thickness away from the surface. 

The mesh I get is the following

mesh settings for midsurface, middle offset type

What do you think about this mesh? Just for information rigid bodies can be meshed?

I get this Von-Mises stress result 

equivalent stress

it is a bit curious that stress appears in spots and is not continuous, but since the tooth is moved forward and downward probably the ligament is deformed following that motion. Is there anything wrong according to your experience?

Thank you very much for your help! really appreciated!

peteroznewman posted this 3 weeks ago

I think the spots on the stress are an artifact of the coarse mesh. If you refine the mesh, do the spots move around?

Is the mesh creating Linear or Quadratic elements? 
Quadratic elements will generate less artifacts because they can represent curved surfaces.

  • Liked by
  • nyla
nyla posted this 3 weeks ago

Mesh refinement introduces a series of errors and simulation diverges. I used the settings depicted in the following images as general mesh settings to get this mesh.

mesh on PDLmeshing optionsmeshing settings

and I used a Method to create triangles quadratic elements only on the midsurface.

The final result for the von-mises stress is better as you can see. Stress spreding is more uniform. I scoped the stress to the midsurface at top/bottom position. Not only top, or only bottom, because I think this represents better the actual solid ligament. 

stress on PDL

One more thing, I've modeled the mandible (that is in contact with the ligament (midsurface) as rigid body, but I've selected a mesh option which is "dimensionally reduced" meaning that generates a surface contact mesh, however I cannot observe any stress on the mandible in the region of can it be?


To conclude I know that by creating in the Geometry "a new part" by selecting the bodies of interest together it is possible to create a uniform mesh whre the elements at the interfaces of the selected bodies share common nodes. I have to try if it improves the results.

thank you again!

peteroznewman posted this 3 weeks ago

It would be better if you used Quadratic elements on the solid body as well as the shell elements.

Rigid bodies don't have any stress because they don't deform. 

Yes, in DesignModeler, if two bodies have an identical surface (or part of surface), then you can use Form New Part to put to two bodies into a multi-body Part and during meshing, only one set of nodes will be placed on the surface in common with the two parts, and the elements will mesh each body using those nodes. That means those parts are connected without using Bonded contact.

You can do a similar thing in SpaceClaim by using the Workbench tab and clicking the Share button.

This is generically called Shared Topology.

  • Liked by
  • nyla
nyla posted this 3 weeks ago

Hi Peteroznewman,

thanks for all! Now I've tried to introduce other bodies in the simulation, but a lots of this warning "Element 296020 has a radius/thickness ratio of 2.90657952 (minimum  radius of curvature of 0.871973855 and a maximum thickness of 0.3 ) made the simulation diverge. I'm not able to identify those elements despite I activate the element violations and Newton-Raphson as it diverges at the beginning. Probably it is related to the shell.  What should I do? If I reduce the curvature min size I get this error "A software execution error occurred inside the mesher.  The process suffered an unhandled exception or ran out of usable memory." and meshing stops. 

peteroznewman posted this 3 weeks ago

You can use Named Selection with the Worksheet to find that Element ID by number.

You need to mesh with smaller elements to avoid those warnings.

The software execution error and running out of memory is usually caused by a defect in the geometry. Take the geometry into SpaceClaim and use the Repair tab to find and fix defects. DesignModeler also has an ability to check geometry for meshing.

nyla posted this 2 weeks ago

Hi Peter,

thank you again! I have a question. How can I ensure the result I get by simulating using the shell is reliable? 

This because I've run two simulations of the same bodies with the difference that one uses the shell body and another doesn't. I've got the following results about the stress on the ligament (which was a shell body on the second type of simulation). In the first image you can observe the von-Mises stress results about the ligament meshed as solid body. The second Figure is about the von-Mises stress distribution by modelling the ligament as a shell body.

solid PDL body

shell PDL

Since there is at least one order of magnitude of difference in the stress values I think this smart way of simulation is not reliable. Or I must improve it. What do you think?


peteroznewman posted this 2 weeks ago

All Finite Element models are approximations and results are not of known accuracy until validated with an experimental result.  See this post.

Some Finite Element models have mistakes so models need to be verified that all the inputs are correct. You should check your inputs carefully.

Maybe you can make two simple models that you can easily verify and obtain some experimental validation result.

  • Liked by
  • nyla