Hi- I am clamping a metal disc using two clamps. They are all steel, and I am trying to understand the best surface interaction setting please for this kind of simulation. Basically, it’s a thin disc being clamped by two metal blocks. Any suggestions please ? In addition, is there please any information about the different surface interactions please ?
It would be best to model this thin part using shell elements.
When it comes to interactions, you could start with default contact settings and only add friction if needed. Then you can adjust the contact parameters as needed. They are described in the CalculiX User’s Manual. This tutorial also covers some of them: PrePoMax (CalculiX FEA) - Tutorial 33 - Leaf spring - YouTube
1 Like
Using shell element can be an improvement of analysis model since it can have multi layer by user defines, for one element trough thickness this does not make any changes. Quadratic tetrahedral may perform better than linear or quadratic shell element since it’s expanded to solid linear or quadratic wedge or hexahedral.
A uniform solutions are using solid for all parts, an extrusion based on quad dominate mesh 2D can be useful to defining number of layer. Unfortunately this is not yet implemented , but someone can still use Salome CAD/CAE instead.
Regarding to surface setting, the master or independent surface is chosen by mesh in coarser ones. Ideally for convergence faster it is not too coarser compared to slave or dependent surfaces. When the node mesh is nearly coincident, someone can select stiff part ones.
Hi Synt
¿Do you mean Quadratic tetrahedral perform better than quadratic hexahedral for thin structures?
Sorry , I don’t understand.
¿Do you suggest the master to be the stiffer or the slave to be stiifer when the node mesh is nearly coincident?
In case of one element trough thickness and excessive plastic strain and large shape deformed/distorted, it’s probably right.
In the beginning sentence of paragraph, i mention a master surfaces. So it does i mean.
In the case of Abaqus, it’s advised to use at least 4 layers of first-order reduced integration hexahedral elements (C3D8R) and avoid second-order elements for bulk metal forming problems with high mesh distortion.
This advisement are to avoid volumetric locking due to highly distorted mesh occurs When only excessive plastic strain occurs says below 10%, an incompatible linear hexahedral and quadratic tetrahedral or hexahedral element may still acceptable.
That"s benefit of CalculiX expanded shell element, a model and number of layer can easily generates. Unfortunately it’s not yet available for linear type of shell element. Another disadvantages ate in the edge boundary condition for curved and not in orthogonal axes. Although it can be solved by using transform function and avoiding use symmetry models.
Yes, reduced integration is advised to avoid volumetric and shear locking. First-order is advised due to contact. Of course, 4 layers are needed for accuracy and to avoid hourglassing.
1 Like