i am trying to model a pipe section that has an slanted S-Bend. To support the upper straight pipe i use solid bodys with contact definition because i want the pipe to be able to be lifted up. The solid bodys for vertical support and the right end the pipe have fixed support. On the lower bend i suppress the movement horizontal and vertical, axial direction is free.
I want to calculate the displacements of the pipe and the reaction foces on the supports.
As loads i use an temperature of all Parts of 200°C and gravity (9810 mm/s²) in vertical direction. I defined an initial temperature of 20°C and use the “coupled temperature-displacement” step with NLgeom = ON.
For discretizaztion of the pipe i have used shell elements and also thickened shell elements. The supports are meshed as solid bodys. The surface of the pipe is placed in the middle of the thickness, so when i use shell elemens the thickness is added on both sides. Same for thickened shells, where i use two layers (i measured the overall thickness of the mesh and it is as i expected).
In both attempts the calculations is not converging. When i calculate the displacements of the pipe without the contact supports (and also without the solid bodys of the supports) the calculation finishes with reasonable values for the pipe displacement (for both attempts: shell element and thickened shells = solid). But this model is not very realistic because the pipe is not supported against sagging through gravity (the pipe is DN900 and 30m long…)
Does anyone have an idea what i can try that my model is converging?
The resigual displacements are going down to 10^-3 but the residual forces stay quite high ~10^4 - 10^5.
I was also thinking if there is some type of constrain i can add to the support faces to allow movement in x,y and only in +z and block it in -z. I have expirienced that compression only also blocks the movement of the pipe in all other directions exept normal to the face.
Do you mean this: https://www.youtube.com/watch?v=N9F-4ZKXB7w ? Those are solid elements, just created from shells. Actually, even shell elements in CalculiX are expanded to solids but that’s just to clarify.
Non-convergence in analyses with contact is almost always caused by contact and usually by initial rigid body motions due to contact not being properly established. Load control makes it much more difficult. Tie constraints or tied contact property would most likely give you convergence but there would be no movement allowed between the touching surfaces.
Compressive-only constraint works in the direction normal to the surface (at each node) so you would need a flat surface to control movement only in one axis.
You could try e.g. establishing contact with displacement control in the first step or creating small initial overlapping between the parts so that it’s removed by contact adjustment in the analysis and contact is properly established. Otherwise, spring elements may help.
Thank you for your advice.
So to initially overlapp the parts i’d interfer them in the cad model.
Contact adjustment you mean the adjust variable in the contact definition?
Does it makes an difference in computional recources using the shell elements or extrude the shells with the thickende shell mesh?
Another question i have is: When i use shell elements and i want to set two shell faces in contact to each other. Do i have to set an initial distance between the shell surfaces that they are in contact when the thickness is taken into account or do i have to set the distance to zero of the shell surfaces (those from the CAD model)?
Regular shells are extruded to one layer of solid elements. If you create more layers manually, it will be of course more costly.
Shell thickness is taken into account in contact (after all, those elements are extruded to solids) so you should position the parts with proper gaps depending on the thicknesses (unless you use the shell section with offset).
Last question to fullfill the picture in my head :
Is the shell element extruded symmetrical with half thickness normal to the shell surface or is it extruded in one direction?
Thank you for your fast replys!
shell offset in CalculiX probably work differently with another FE, simple model of cantilever plates below will ignore additional bending due to eccentricity. However, offset variable at mid-spans may similar.
:
