as notified in CalculiX documentation and previously by many comments also, quadratic tetrahedral is a general purpose element.
if i remember correctly, there’s large test of tetrahedral by Ansys for case of elastic, plastic, static, dynamic and contact problem. Report shown its reliability and robustness in element and meshing solution. Unfortunately, number of element, nodes and computational time is not clearly reported. In my experiences, it’s required almost double in times or physical memory. Another important in limitation of automatic tetrahedral mesher for thin part related to number of element layers also not been notified.
below simple example, when mesh not shown it’s hard to judge which element being used and fit better since it have similarity in results
@ osmcnkrtn using a cluster of nodes would help to average out the values but then it’s not clear quite where the boundary (or centroid?) of the area they represent is.
What’s you greater aim here? Reaction force at a point on a fixed surface (or edge) isn’t physically meaningful, or rather, it’s zero. It needs an area (or length) that it’s distributed over. Maybe what you really want is force per unit length?
In principle, you can sum the forces on each element face (or edge) individually and they’d be correct for that face (or edge). The difficulty is that the value at a node is already the sum of forces from each element using that node, so you’d have to somehow subtract the contributions from adjacent elements. Perhaps make a disconnected mesh at the boundary with several patches (even 1 per element), then you can easily sum the force in each patch.
It seems your tet mesh is way coarser than the hex one, making the comparison unfair. In the tests I’ve conducted both 2nd tetrahedrons and bricks provided good agreement against analytical results (static, hertz contact, buckling, eigenfrequency…). However, the former took more time to solve.
I believe there is some sweet point regarding mesh density for tetrahedrons because if one uses the same refinement for both types of elements (as I did in these tests), tetras will provide meshes up to 6 times more populated. It is a nice thing to investigate though .
I agree with this point. However as @vicmw remarked, forces along an edge are not a physically meaningful quantity in continuum mechanics, surface tractions are; especially because in FEM boundary conditions are imposed in a weak form (variational formulation of the differential equations and boundary conditions).
This has a distinct effect in contact calculations since contact is discretized into nonlinear springs and their spring forces.
I have crashed headlong into this concept recently. Especially when translating my hand calculation of the springs that were necessary needed to support my model into the nodes. In linear elements the loads are distributed “approximately” proportional to the contributing areas of each node but in quadratic elements they have no correspondence with physical reality at all. This leads to the extreme of having to introduce negative stiffnesses in the springs of some nodes in order to support the element uniformly.
Thanks @vicmw ! My primary goal is to acknowledge the presence of an area near varying forces on a fixed edge and to distribute these force values across this area. In this scenario, I’m assuming that the nodal forces don’t vary significantly over this area(area very is small). One edge of the area can be considered as the arc swept by a circle (or the edge formed by the nodes I’ve chosen), while the other edge will be a length that I can change parametrically. Therefore, I plan to perform a regional stress estimation based on the area and nodal force values. I believe this method can provide a reasonable estimate of the stress value in the scanned region, even if it’s not perfectly accurate.
I’m considering an approach where I divide fixed nodes into groups and sum up the nodal forces within each group to make an estimation. I believe that this method might not lead to significantly incorrect results. What are your thoughts on this?
It seems to hinge on how the “regional stress estimation” works which I don’t understand but here’s an idea to approximate force on each element edge -
Sum forces over each edge, but halving the values shared by two edges since they contribute to the force on both edges.
It’s not quite accurate because the edges aren’t equal length but might be close enough and the overall sum will be correct. Also, you’ll be able to divide these values by the edge lengths to get a more physically meaningful force per unit length (or force resultant?), the 1D equivalent of surface traction that @JuanP74 referred to.
I thought they had aproximately the same number of elements. But I just disovered that the element number doesn’t start at 1 when using te10 elements with cgx. Probably because of the use of tetgen internally. So, I learned something today!
However, when I correct that and give the tet mesh approximately the same number of elements as the hex mesh, the tet mesh is still much more visible in the results.
I would say that if you manage to build a nice structured hexa linear mesh on that edge you can get what you need. The linear hexa benefit from the fact that each node has the same weight. If the shape is not distorted one could assume the weight corresponds to the contributive area. That provides a nice and smooth reaction all around the corner.
Another thing is what Victor says. Has a point value physical sense? .I don’t think so.
Be careful if you load your body with a distributed load like gravity as the RF value may contain part of that load.
.
Probably because of the use of 
