mesh at contact

[Anonymous]

Is it possible to reduce the amount of triangular elements at contact areas automatically?

I am using plate elements and at some parts the contact mesh looks good and at some it looks really horrible. Since these parts have the same dimensions I would like to reduce triangular elements and get rectangular ones instead.

[Anonymous]

Is there really no automatic way to realize a more homogenous mesh?

I get a max/min stiffness warning and when I look for the questionable elements, it looks like the reason is somehow connected to the bad mesh!?

[Anonymous]

Okay, since the automatic mesher did not achieve a nice result and a lot of poor-shaped elements appeared, I tried a surface mesh enhancement. Furthermore I followed AstroJohns advice:

1) Surface mesh enhancement works from the existing mesh. The new mesh is based on the surface of the existing mesh. If a model has a coarse mesh such that a hole is 10 sided, enhancing the mesh and specifying a smaller mesh size results in a finely meshed 10-sided hole; the enhancement does not know that the hole is theoretically round --- even when enhancing a CAD model. For this reason, the normal procedure when working with curved surfaces is to start with a fine mesh and use the mesh enhancement to generate either a larger mesh size or similar mesh size.

2) Note: Set the Options Feature Layer to 15 before enhancing the mesh as only one part of a CAD assembly can be enhanced at a time. Matching lines between the CAD parts will automatically be placed on Layer 15 by the CAD surface mesher (Mesh Mesh Generate 3D Mesh).

I already tried that. The mesh really looks better and it seems to work in a solid model (nevertheless I still get a stiffness warning).

Besides, unfortunately, the mesh looses contact to the adjacent parts when I use the mesh enhancer with a plate model. Does the feature layer option have problems with plate models? I can imagine that the issue occurs because the feature lines of the incoming CAD-Data are not the same lines as those where the contact actually is in the plate model.

[John_Holtz]

Oh, there are plate elements involved. That may require some additional work as shown in the series of images attached.

Technically, what happens when you enhance a surface mesh and specify a "Feature Layer" is that the position of the lines on the feature layer are kept, but the length of the lines may change. So if only one edge of the plate elements are on the feature layer (15 in my example, see image "2 - "), then the mesh enhancement can join all of the lines together (that does not change the feature!) which lets the mesh enhancement put in larger elements which no longer match the mesh on the joining part (see image "3 - ").

What needs to be done is to put more lines around the match location on the feature layer (see image "4 - "). Since the position of the features cannot be changed when making larger elements, the elements in the match zone remain the current size, and the rest of the mesh is enlarged. (see image "5 - ")

Note that this enhancement is just an example. No need to reply with how bad AstroJohn made his mesh.

[Anonymous]

Thanks John!

My Assembly has a lot of feature lines, so that it would require really a lot of time to follow your instructions for every part of the model.

However, I found another good advice: With some time investing in Model Preparation and afterwards using Plate/Shell I could achieve a much better meshing result than by using the midplane mesher. I guess the reason is that the model has a lot of edges with contact and I also define some seed-points.

Unfortunately the stiffness ratio warning is still there.

warning: max/min stiffness ratio =            1.0286E+17
               maximum stiffness =  5.112161E+18 at eqn#213093, node#38637, Rz
               minimum stiffness =  4.970171E+01 at eqn#31366, node#5228, Rx

Since I have rigid elements in the model (K=1E9), in literature one can read the advice to run the simulation with a low stiffness for these elements. Afterwards one shall use the maximum stiffness out of the report to calculate the "true" rigid elements' stiffness by k(rigid)=5k(max), but the warning did not disappear.

As one can see above, the stiffness applies to rotational degrees of freedom. Therefore my guess is that my twisting coefficient ratio is not correct.

How would you determine that? And in what range could it be?

For the moment I kept the standard 0.001.

By the way: How can I find a specific node? I know how to find an element by knowing the element and part number, but I am missing a search for nodes.

[John_Holtz]

Just to clarify, are you saying that you reduced the stiffness of the kinematic elements to something low (around 50 if you want to go as low as possible), but you still got the stiffness warning? If so, these are the things that I can think of which would cause it:

• poorly shaped plate element, either because it is warped (the 4 nodes are not in the same plane) or has a small or large angle between two sides (like 5 degrees or 180 degress). The first and last can be found from the Results environment by using "Results Contours > Other Results > Element Properties". (I think the small angles cannot be easily found.)
• If the maximum and minimum thickness of the plates is a large ratio. (One plate 1 m thick, another plate 1 mm thick.)
• Vastly different material properties for the plate elements. (Maybe use the Report environment to look at all of the properties simultaneously to confirm that something was not entered improperly.)

Node numbers can be found by using "Results Inquire > Inquire > Current Results > Specify" and type the node number. This will select the node, so it may be helpful to first change to a wireframe view "View > Appearance > Visual Style > Features".

[Anonymous]

Thank you John, this was very helpful.

I checked all of your points and the material properties are a problem in my model.

It seems like it is a mixture of the other criteria.

With your explanation I could find an element that was close to 180 and eleminate that.

Now I still have some elements that have a nodal angle of 160, but I dont get a stiffness warning if I set my rigid elements to 100 in stiffness.

Unfortunately, if I put them back to 1E8 or even higher, the stiffness warning appears again. I dont think it is economical to eliminate every angle that is around 160 and the stress result does make sense...

The only difference in stiffness that I could imagine is for example the junction between my rigid elements (DOF in all directions) and the drilling DOF of the plate elements which is characterized by the twisting coefficient ratio.

So how do I determine my rigid elements' stiffness and the twisting coefficient ratio accurately?

Of course my results change with different stiffnesses of the rigid elements and from my idealizing point of view I can make them as stiff as possible...