ccx error: shell normal in node ... is smaller than 1.e-10

swaraj

I am getting this error in the attached limil file. Can you tell me what is wrong with my mesh files?

Sergio

For some reason I can see the nodes but not the elements, can you check it and upload again the model? Regards

swaraj

Attached again, Please Check

Sergio

There is an issue with the size of the model, probably due to bad scaling during import. I took a quick measurement between two oposite nodes and is about 39400 mm. Try rescaling the model in Mecway to get the right dimention.

swaraj

Hey,
Still the same problem exist. Attaching the new project file.

Victor

If you use Mecway 12, there's a button on the solver window to select the element with the error. That shows a triangle element with an extreme aspect ratio making it look like a line, which wouldn't usually be able to solve.

With version 11, use Edit -> Select elements by number... to find it.

There are also a lot of nodes with no elements. They're usually harmless but can make rotating the view difficult. You can delete them with Mesh tools -> Delete unused nodes.

swaraj

No @Victor, I am asking what that error means?
Is the error coming because of the shell offset i did. Because some elements looks fine. How can I fix this issue overall, rather fixing element by element (I found out many bad elements detected by CCX)

Victor

Though I don't know about CCX specifically, this is how I expect that error occurs. It would calculate the normal vector of the shell's surface at each node by doing the cross product of two vectors tangent to the plane of the shell, such as those parallel to the two edges that meet at that node. If those two vectors are nearly parallel to each other (as they would be here) then the cross product is nearly zero so the normal vector is nearly zero. A near-zero vector can have a big error in its direction so CCX would stop because the direction of the normal (and thus the orientation of the expanded solid) can't be determined reliably.

In other cases where the element looks fine, the only other explanation I can think of now is that it's too small.

A general way to solve it would be to use a mesh generator which doesn't create badly shaped elements or to clean it with some mesh editing software. One free one is Meshlab which has many tools for operating on large dirty surface meshes and point clouds obtained from 3D scanning.

It's not because of the offset because the same error occurs with no offset.

disla

It is a mesh problem. You have poor quality elements. Very thin triangles.
Could you post the underlying geometry. ¿Step, iges,..?

swaraj

Hi,
So I corrected the aspect ratios of elements. On running i got a new error 'Jacobian Error'. I think it may be due to shell offset. Attaching the limil file.

I want the inner surface of shell to be in contact with the human tooth mesh. On giving thickness, shell extruded from midplane, which i don't want, so i used the shell offset option in element properties as suggested by @Victor. I don't know if that would simulate the analysis conditions that i want.

Should the shell element, on giving numerical thickness, convert to prism element ?. As its a thin shell model, it should just calculate the stresses on outer surface by an analytical formula, not by creating a 3d mesh of shell mesh using prism elements.

Please clarify these fundamentals for me.

Attached is the link to limil file:
https://we.tl/t-B6zdxJCcn3

Victor

I think there are two types of problem in this file:

1) 6 badly shaped elements. You can see these if you set offset to 0 and solve.

2) The other 72-6=66 well shaped elements that only cause errors when the offset is specified. I don't understand what's really wrong with these but they're all in the creases where there's high curvature so I suspect it may be that the offset distance plus half-thickness is greater than the radius of curvature so that the offset faces could end up intersecting each other like this:

The only solution I can think of for that is to make the mesh of the midplane or the other surface instead, or use solids. I've seen a case of Jacobian error for high curvature on offset shells before ( @prop_design ) but I'm not sure if he found a solution.

Offset shells model contact according to the offset positions of their faces. Here's a simple example (offset shell contact.liml) that shows that the offset and thickness are correctly accounted for by the contact.

CCX always converts shells to solids. It doesn't have any traditional thin or thick shells.

prop_design

i've run into the issue of having to switch midplane surface and direction of offset as well. it's a pain but you can eventually get it to work. sometimes i can use the mid-plane and go one direction but not the other. i have modeled all three at times. the inner, the midplane, and the outer. as well as experiment with the direction. what i try to do if possible is make it so the element's expand to the outside of any radius. rather than having the expand into the radius. if that makes sense. same as what victor is showing. to switch the direction of the shell expansion add a negative sign in front of the size you choose.

swaraj

hi @prop_design
Do you have a choice to give thickness to elements in only one direction. I thought, thickness is always applied symmetrically in both direction that's why i can't expand elements outside of any radius.

prop_design

no unfortunately you can only move the midplane offset. but you can move it positive or negative. so it's something you can try before creating a completely different surface. the main thing i look for now is which way the elements expand into any fillet. i use a surface that you can get the elements to expand outward. i've had some midplane models work as is though. so it's hit and miss. i think, like victor said, it's a radius of curvature to element thickness issue. so it's hard to predict for me at least. this whole mess is another unfortunate side effect of the ccx shell expansion. i don't like it. you get a 3x hit in element count. it makes creating models a pain. and there is no real benefit. a good 2d shell element formulation would be better in my opinion.

another work around would be to assign element orientations to solid orthotropic elements. but you can't do that in mecway right now. that would be the ideal option. then you wouldn't have to deal with shell models at all.

prop_design

this is a long video but i think it covers this topic. https://youtube.com/watch?v=M9YunnJhZbo&list=PLzGiietqAECXnIFl6ngHvhzgBxgTrC_qW&index=12

It looks like around the 17-20 min mark is showing this issue.

prop_design

i can't edit my previous post, however, I deleted the YouTube channel and video today. so the link provided is no longer valid.