Topic: Mesh dependend results

Dear all,

I have some problems understanding the results / finding the error in the modelling for a simply supported RC-beam.
Structure: Simply supported beam with one load (modelled as displacement) in mid span (3-Point-Bending-Test). The beam has one reinforcement bar.

Element types: The Concrete is modelled as CCIsoBrick<xxxxxxxx> and the reinforcement bar as CCBarWithBond (as CCDiscreteReinforcementME defined/generated through nodes and embedded in the brick elements)

Load: The structure is analysed until the first two/three cracks due to bending appear (load equals then approx. 1.3-1.4 x Load_crack and is less than half of the ultimate limit load).

Depending on the mesh size, I get different crack patterns. The load-displacement-relation as well as the total crack width (sum of crack widths in longitudinal direction for the vertical position) follow the same trend (of course with jumps at different positions since cracks appear not at the same time). If I have a uniform mesh size in vertical direction and only one element in transverse direction, I get the expected crack pattern with the expected distance between the cracks. If I discretize the transverse direction with more elements or/and change the vertical coordinates to a non-uniform grid, the crack pattern changes in an unexpected way. Instead of a new second crack (at some distance from the first one in the mid span), the crack in the middle will “continue” cracking (increasing of its width and neighbour elements start cracking, even though the stress at the expected crack position is significantly higher).

The “problem” of the transverse discretisation can sometimes be solved by performing the analysis with more load steps. However, not in all cases: for the “initial” model, 10 load steps after the first crack are sufficient to achieve the expected crack pattern. For some transverse discretisations lead to the same crack pattern using 50-100 load steps, others do not start a new crack even if up to 1000 load steps are used (This depends also on the general size of one element, i.e. number of elements in vertical and longitudinal direction). However, due to having only one reinforcement bar, increasing the number of load steps seems reasonable.

For the problem of the vertical coordinates (e.g. changing [0 0.02 0.04 0.06 0.08 0.12 0.16 0.2] to [0 0.016 0.032 0.05 0.075 0.1 0.125 0.15 0.175 0.2] in the *.inp) I was not able to find a way of obtaining somehow the expected crack pattern. The ELEMENT INCIDENCES are still grouped in one ELEMENT GROUP.

Maybe someone of you saw up to here already the problem. According to previous threads in the forum, my mesh causes - obviously - some trouble, since the results vary a lot. In the documentation (troubleshooting etc.) I couldn’t find a solution, that’s why I have the following questions:
1. Do I have to take something additional into account when discretising the transverse direction?
2. Can elements in one ELEMENT GROUP have different sizes or do different sizes cause problems? (e.g. because of only one Jacobian per group is calculated when IsoBrick elements are used, …)
3. Sometimes I got also different results when the reinforcement bar is going through the element / is at the position where element edges are / is at the position where element vertices are. Can this also cause some problems or is this just some side effects from the problems above?

I am glad for any kind of hint what I can try next.

Best regards,

Re: Mesh dependend results

Dear Marcel,
I. without seeing your model, we can only blindly guess what is happening...

II. As you mention a single element in transverse direction, I don't understand why you prefer a 3D model over a 2D one?

III. Please keep in mind the max. recommended edge aspect ratio is about 3:1 for volume elements.

IV. Moreover, please do not forget mesh sizes smaller than the max. aggregate size clearly violate the assumptions of concrete as a [homogeneous] continuum. See also the relatively new option"crack spacing min", which can reduce the problems at least to some extent.

Ad 1.: Please see points II. + III. above.

Ad 2.: I do not see any way how varying elements size throughout an Element Group should cause problems (except for indirect - loosely related effects discussed above).

Ad 3.: This can have some influence (see also Troubleshooting, 2.1.21 When I model the reinforcement, do the bars and stirrups have to be in geometric connection (with common intersection points) or they can be modeled according to their axis so that they do not touch one the other in geometric sense?), especially when bond damage is represented by cracking of the concrete near the bar.