I am trying to model a 6” thick steel plate that will be installed on a massive concrete section and will cantilever from each side of the concrete section. The cantilevered parts will be loaded with a very big force of 810 kips on each side thru PT bars running thru the holes. The middle section that bears against the concrete will have only compression constraints. The two cantilevered parts are loaded with uniform pressure calculated from the total force from the PT bars. The bottom edge of the plate has a boundary condition to restrict translations in all directions so that the model can run. I used a Quad-dominated mesh. Also a very high K constant to simulate the rigidity of the concrete. Plate is modeled in Rhino and inserted into PrePomax and then assigned as a shell section with t=6”. The model runs however the deflections make no sense, they go up to 20”+ which apparently cannot be the case. I attach a snippet below for better understanding of the geometry. The yellow part is the one bearing against the concrete. The blue parts are the cantilevers that are loaded with uniform pressure. Any thoughts and help will be very much appreciated. Thank you!
Did you double-check all units ? I’m not really familiar with the imperial system, but mismatched units (especially related to Young’s modulus and load) are considered to be one of the most common causes of such errors.
Yes of course and thank you. I cannot attach the model as the system does not allow me to attach, but I provide wetransfer link for the model. Here it is : Unique Download Link | WeTransfer
As far as units yes i checked them E = 29000 ksi = 29000000psi. Poisson = 0.3 and pressure on the cantilevers = 5060 psi coming from the massive forces. Takes a lot of time for convergence but my computer is old so perhaps it is part of the problem. Based on manual calculations deflections should be minimal with the massive thickness of the plate but cannot get the same in PrePoMax.
I will check it later, but do you have any nonlinearities in the model ? The compression-only constraint needs them to work properly.
Instead of fixing the edge, you could try modeling 1/4 of the plate and applying symmetry BCs. Just keep in mind that constraining rotational DOFs of shell element nodes can be very problematic in CalculiX.
You could also use the Thicken Shell Mesh tool and try with solid elements (especially since the plate is thick). Shells in CalculiX are expanded to solids anyway and there are several limitations/bugs related to them so it’s often better to just switch to solids instead.
Thank you I’ll try your suggestions with a solid elements and see how that works. And yes I have activated NLgeom in the step to account fro compression only. Please see snippet below.
Are you sure the dimensions of the plate are correct ? Is it supposed to be 1219 x 812.8 in ? What deflection do you expect according to your hand calcs ? IMO there’s something off with the units.
Thank you so much! This was a stupid mistake. I never even thought to check the dimensions once imported into PrePoMax. The dimensions are 48”x32” i.e. factor of exactly 25.4, conversion inches to mm.
Several observations:
Model in Rhino is in inches. In Prepomax I chose specifically imperial inches, but when imported somehow the model is scaled up by a factor of 25.4. So I manually scaled it down in PrePoMax to bring it back to what is supposed to be. Not sure if this is the correct approach.
To get a convergence and final result I had to tweak the initial time increment to 0.1 s with automatic incrementation.
My manual calculation derived less than 2 mm upward deflection in the middle of the steel plate when the two cantilevers are subjected to pressure. I am trying to get a full contact between steel plate and concrete, thus this middle defection is important.. With the revised geometry in PrePomax I am getting now less than 1 mm which I think is to be expected. VonMisses stress also seem to be good about 21-22 ksi witt ha bit more around the holes stress concentration.
I’m glad that we’ve found the cause of the problem. My highly simplified hand calcs showed the deflection of something around 17 m, and Nlgeom was preventing the analysis from running (due to excessive deformations), while a linear run with true scale deformation showed absurd deflection.
I have such problems with STEP files from FreeCAD too, and I always end up scaling the geometry (even if I just use meters instead of millimeters). Fortunately, it can be easily done in both FreeCAD and PrePoMax.
It’s best to always check the dimensions after each import/export. In PrePoMax, you can use the Query → Distance tool for that or just align the model with the ruler at the bottom of the screen.
This is absolutely normal. The initial time increment of 0.1 s is, in fact recommended setting in most cases.
You should also refine your mesh significantly, especially around the holes. It’s best to perform a mesh convergence study.
