Discussion Forum

Hi

one way of explaining is that, in 2D, a mapped square mesh is like two triangular mesh elements put together (not fully as the cross edge is not defined, but almost 2). Therefore a maped mesh has more DoF's than a triangular mesh, requires more RAM and takes longer to solve.in complexity This is even more applicable to 3D there are 6 thets in a brick - some common elements (if I did my maths correctly,), hence far more RAM required, and time to solve, than for 2D

Why use mapped or bricks, and not only tri/ thets ?
Well for me some problems have symmetries of flux lines that are anisotropic, these models accepts anisotropic mesh elements too, without serious loss of precision, while thets or tri should ideally be symmetric to have no particular anisotropic influence on the results, but often the mesh of a complex part comes out with a bad "quality" = very elongated mesh shapes, this could lead to poor results, therefore, when understood, mapped mes can give far less elements than tri/thets, even if each element has more DoFs

Check also the KB )knowledge base, on the main web site) about DoF per element and RAM estimations

--
Good luck
Ivar

Hi

I tried to simulate the reinforced concrete beam element similar to tutorial (Concrete Beam With Reinforcement Bars, Application ID: 10440) by using mapped and swept functions. The difference between tutorial and my current case example was the shape of beam. I used the T-beam section rather than rectangular section. I followed all tutorial steps for creating mesh, Edge-Mapped-Swept function. And the result for mesh element builder was " Failed to create swept mesh for domain, - Domain: 1
Isolated edges are not allowed". Can some one provide me advise. Many Thanks


Maizuar

Hi
Have you tried to mesh the section and sweep ALONG the beam ?
Because a Sweep mesh only can perform if the initial section and number of boundaries (edges) remain constant.

--
Good luck
Ivar

Thanks Ivar for your advice. I divided the Inverted T-beam with several sections and the mapped and swept meshing functions can be quickly generated. However, I still have a problem with computing the beam.
It said :

"The following feature has encountered a problem: In segregated group 1:
The relative error (0.046) is greater than the relative tolerance.
Returned solution is not converged.
- Feature: Stationary Solver 1 (sol1/s1)"

Hopefully, I will have a solution soon. Many thanks.
Regards

Maizuar

Hi

that can come from several issues, often from not enough fixed BC's such that a degree of freedom is not constrained. I cannot tell much from the image, I see one symmetry BC, which, depending on what surface it applies constrains up to 3 DoF and then a rigid connector, but that can constrain only 0-6 DoF's so it's not giving me enough info. Try to carefully check your degree of freedom and identify if you have not left one fully free.

Often the results are quite explicit, even if the solver fails, it has found a partial solution, and that might give you a clue. Another way is to add some gravity load and check in the time domain if your part is "falling"

--
Good luck
Ivar

Hi Ivar
Thanks for your advice. I followed all of your previous suggestions especially for symmetry and rigid connector inputs. However, the computing results can not be displayed. Therefore, herewith I attached the file for you to see. Hopefully I can find solutions soon. Many thanks.


Kind Regards


Maizuar

Hi

first of all you are doubling the gravity as you have a body load and a gravity node, only one of the two should be used ;)

Then you are in Geometry "assembly" mode, not sure that is the best, but OK you have copied the "concrete beam" in the Application library a good starting point. Still, a question, your steel bars are these sliding in the concrete, or as I suppose, in intima contact such that the concrete expansion is transferred directly to the steel bars all along their length ? The latter is obtained with the extrusion function, but there is also the independent meshing of the two entities: concrete solid beam and the bars.

The sweep mesh does not allow you to have "free" edges, the trick here (if you use Union mode) is to define your section, as you do in a workplane, but then to unite them all and suppress internal boundaries for the individual blocks. Then you add a layer with a poly-line going through the bars with a point at each bar extremity. You must keep this internal boundary to get the mesh swept correctly.
Then for the mesh you selection your section mesh it with triangles and sweep in one go the rest of the beam in the length direction.
Your (and the Application model) way in Assembly mode is also possible, you have then a mesh continuation issue along the bars, but more freedom to define the bar mesh and the concrete mesh independently, with an interpolation for the transfer of strain, that for me requires some toy models (simple cylinder with one bar) to check how representative this is and potential side effects.

Another point in Union mode you can work with u for the dependent variable for both the Solid and the Truss (and without the "general extrusion", but in assembly mode, to make these two physics independent, you need to call the dependent variable of the Truss physics for u2, and use the extrusion function to link the concrete displacement to the steel (but currently you do not couple back from the steel to the concrete)

Finally your "prescribed displacement" BC, in the Application "concrete beam" model it is to say that the long slender beam is attached in a given way at its extremities and that whatever is done to make the end sections rigid has little effect on the full "long" beam. In your case, you have chopped it in two with a symmetry, a good point, but also your beam is very short, so the side sections with a rigid prescribed displacement BC will have non negligible side effects.
Another point if you have a symmetry plane for the concrete you need to be sure you have also a symmetry plane for the truss elements. But probably this is obtained by the Truss prescribed displacement and the general extrusion.

I haven't had time to read through carefully the "concrete beam" application model, but its absolutely required as there are many subjacent hypothesis here, and one must be sure to catch them all. Otherwise, when you change your model to another case you might violate some of the hypothesis (i.e. length to section are ration should be "long) and that will have some effects on the modeling.

I would also suggest to start with a simple concrete cylinder "toy model" with a steel edge in the middle, and check out the effects with and without assembly/union, general extrusions, with and without steel ...
--
Good luck
Ivar

Thanks Ivar for your helpful advise and comments. I will follow up all above procedures and hopefully I can find correct results. Many thanks.


Kind Regards


Maizuar

Hi Ivar

I would like to include prestressed steels in the previous Super T-Beam model. What physic interface should be used (Truss, solid mechanic, etc. ???). Also, in material properties, should I use the properties of structural steel with certain initial stress. Many thanks.

Kind regards


Maizuar