Hi, I´m solving a model with several bolts preloadings, and when I see the deformed results (at the end of the first step, only bolt pretension) with the usual deformed variable “Displacements” with a factor of 200 I see that at some places the bolted bars looks like if they where separating (with no external load) at the contact faces (other were just TIED), the same happen with the bearing supports, they looks as if they where separating at the lower contact faces
If I choose “Disp&Def” variable for deforming the model, the model looks more realistic, with no separation on the bolted surfaces, What is the meaning/diference of “Disp&Def”??? And why even if I increase the deformation scale to 2000 or 20000 the deformed shape is the same, not as in the Displacement scaling?
This shows the sum of the displacement and mesh deformation vectors. There’s also Disp&Def&Depth which adds wear depth too - those features were added for contact wear analyses where mesh deformation can also be included.
Thanks, so the “Displ&Def” would not be correct for this situation. I have sliced the model at the first bar, and picked a node in the contact area, the Y displacement is bigger than the X and Z, could it be due to the lack of friction definition in the surface interacion? In my experience dealing with friction is a pain in CCX. What I don´t understand is why the bar are separating from the vertical walls if they are heavily pretensed.
Did you check contact outputs such as COPEN and CPRESS to see if contact is working properly there (Abaqus also has CSTATUS which is very helpful in such cases as it shows whether contact is closed and sticking/slipping or open at a given time) ? A frequency run could be helpful too if they were simply tied instead.
Friction is really bad for convergence, also in Abaqus/Standard (implicit solver). Abaqus automatically enables unsymmetric matrix storage if friction coefficient is higher than 0.2.
I would say that Disp&Def should be the same as Disp in your case, since Def (mesh deformation from the previous step) is zero. So maybe the scaling is such that it looks different. But also, the scaling should work in the same way, so something is weird.
Setting a small friction coefficient can be counterproductive. One might think a small value would help with convergence because the effect will be small but it can actually be detrimental. The smaller, the sooner it enters in the game. If, as in your case, you’re not interested in analyzing failure due to slippage of the bolt (more typical of a prestressed bolt in shear), it works better to use a friction coefficient of 1 so that friction doesn’t start acting until you have a contact value equal to the prestressing pressure. This also allows the portion of the curve where lateral movement is controlled by transverse stiffness to dominate, preventing rigid body movements in the bolt. Try μ=1 and Tangential Stiffness = E*50/100 GPa/m and see how it goes. Then check the contact clearance to see if it’s within an acceptable range.
Keep in mind this figure. transverse displacement is controll by two different mechanisms.
EDIT: Be carefull when using pretension set up by force. Your pretension section clearance could be openning for that reason if you don’t later fix it.
Abaqus also has so-called “rough” friction where it assumes that the friction coefficient is infinite and uses Lagrange multipliers to enforce zero elastic slip (infinite sticking stiffness). CalculiX doesn’t seem to offer this method for imposing frictional constraints.
Rough friction is normally used together with no separation option. In CalculiX, there is a workaround to simulate no separation contact. But to simulate “sticky” contact, I’d rather use cohesive behavior as implemented in Abaqus. Increasing the friction coefficient beyond the standard values could be risky.
I have applied pretension by force in the first step, and by displacement and fixed in the second. But is at the end of the first step where the separation appear!
Usually, it’s preload by force or displacement (to aid convergence) in the first step and then in the second step preload is fixed to apply the operational loading.
A high friction value can help to identify the source of a nonconvergent issue in the analysis. I have ear many times in the forum about convergence struggling when friction is involved but one should consider if the friction force is enough to keep the model in place once the sticky regime is finished. Specially for load driven problems. In that case the nonconvergence issue wouldn’t be a problem of the solver but an indicator that the friction force is not able to keep the parts in place.
True, but it’s very often the case that friction fails to prevent RBMs because contact it’s not firmly established (at least not yet) - too bad CalculiX doesn’t have contact stabilization.
To be more specific about the previously mentioned reason why high friction has negative impact on convergence - unsymmetric stiffness terms become more significant as μ increases. Hence the switch to unsymmetric solver (*STEP, UNSYMM=YES).
Another thing is that the mere introduction of friction (especially Lagrange friction, although in some rare cases it actually helps) hinders convergence so it’s better to use frictionless contact when possible.
I’m curious if Abaqus would behave in the same way or better/worse taking into account numerical singularities, but also possible automatic stabilization. Can you show how you apply BCs and load to the plate (via rigid body constraints, I assume) ?
If I remember correctly, it only works for wear analysis. In all other analysis types, the displacements are summed from step to step, so there is no need for mesh deformation from the previous step. The displacements contain it. In wear analysis, the displacements represent only those in the selected cycle, while displacements from previous steps are stored as mesh deformation.
