asdeasoft.net

I have done a dynamic analysis on 2 models.
1. model 1 elastic analysis
2. model 2 nonlinear model - concrete asd3d and steel 02 with min max. It is a model with a layered shell element.

In model 1, the deflections at the corner of the SLAB are as follows: While in model 2 they depend on the density of the mesh.
a) fine mesh

b) coarse mesh

My units are N/m.
I don't understand how for a nonlinear model deflections could reach -1.5 m ? BY SETING MIN MAX FOR STEEL.

SECOND WHY DO THE RESULTS DIFFER SO DIFFERENTLY FROM THE DENSITY OF THE mesh. THE LENGTH OF CALCULATIONS ALSO FOR THE FINE MESH HAS INCREASED AND IT IS A SIMPLE MODEL.
I was watching THE WEBINAR ABOUT STRAIN LOCALIZATION and MY QUESTION IS, IF I USE 1 PARAMETER IN CONCRETE MATERIAL PROPERTIES IS THE AUTOREGULARIZATION FUNCTION ON? AS IT IS FOR USER DEFINED POSSIBILITIES?

DOES THE OVERALL IMPACT ON THIS RESULT ALSO HAVE THE NUMBER OF LAYERS IN THE layered SHELL MODEL?

Thanks for your help.
Best regards

I took a step back. And I performed a pushdown anlize first to know approximately what the displacement of the plate corner node might be.

Since I obtained more than 1m deflection for the dynamic anlysis, it seems to me that something is wrong.

Why are the results for the nonlinear static analysis so different from the settings in the analysis. E.g. for newton metod with line search I got 3.5m, for implicit and newton method are different values than for implex. Without corotation I also have significantly different results.
Doing 3 different anlysis (elastic, nonlinear static, and nonlinear dynamic I don't know where I am closest to the truth.

I noticed that the results change for the test settings. What should be the tolerance and number of iterations? As it was in Francesi's webinar it depends on the units of the structure. I have meters so the tolerance (norm dipslacement increment test) I set about 0.0001 0.000001).

The worst thing is that changing the density of the mesh significantly changes the results. Using adaptive time step is a significant improvement, but as I wrote above plate deflections over 1m are not realistic.

Let's focus on the dynamic test now.
It's fine that you get a larger displacement in the nonlinear case, but your results are wrong (it's too much more than the elastic response).

The main source of error is that you attached the column to 1 point of the slab (this indue huge shear forces to a single node of the slab).
In nonlinear analysis this will make the slab fail in out-of-plane shear. Because the shell section does not account for shear reinforcement.

With the modification I did here () I imposed an elastic transverse-shear behavior, while the membrane and bending behaviors are still non-linear.
In this way the results are much better, But you will always experience a dependency on the mesh size, due to the point-intersection between column and slabs. (Huge moments on small elements).

I also had to increase the number of layers of concrete (1 in the middle is not enough to represent bending).

Try this and see what happens when you refine the mesh.

Then try to make the corner portions of the slab rigid (portions of the size of the column cross section) and see what happens

Dear STKO,
thanks for the answer.

Try this and see what happens when you refine the mesh.

I have made analyses for mesh sizes 0.7 and 0.4. For 0.7 the result of deflections I got as for elastic anlysis Uz=-0.02m, for size 0.4 I got UZ=-0.3.
Still the result depends on the mesh size, but the deflections are not of the order of 1.3m.

Then try to make the corner portions of the slab rigid (portions of the size of the column cross section) and see what happens

Please check if I understood correctly.
Method 1
In the existing plate, using lines, make a square with the size of the columns (for example, a 0.25x0.25 column). Then merge the lines with the slab. Give restraint on 4 edges (which are the edges of the columns) and they will change according to the size of the mesh.

Method 2
Make the corners of the plate as 4 small plates corresponding to the size of the column. Then merge them with the rest of the slab.

The main source of error is that you attached the column to 1 point of the slab (this indue huge shear forces to a single node of the slab).
In nonlinear analysis this will make the slab fail in out-of-plane shear. Because the shell section does not account for shear reinforcement.

This answer made me realize that I did not understand the principle of the elements I used. I would really like to ask you to answer some questions about shear, since in my work I mainly focus on bending and membrane action of the plate at large deformations. I am afraid that these very questions may occur during the presentation of my results.

1. You wrote that the slab failed due to shear (Vz) and that the multilayer shell element does not contain shear reinforcement. Then how much (or what) is the shear capacity of the slab? E.g. in designing according to the Eurocodes, the shear resistance of a slab without shear reinforcement is always checked first (just bending reinforcement is taken into account, so my 0 and 90 degree reinforcement).

2. I don't really understand the issue of shear in the slab. By anlizing the zone above the column, punching or bending failure can occur. Am I able to anlyze punching in the elements I use? If the supporting element would be a long wall, how am I able to check whether shear or bending failure has occurred?

This question introduces a 3rd way of modeling the Column Zone. How about making a 0.25x0.25 slab as an elastic slab? But won't this method result in not capturing the formation of a hinge due to bending, as happens in beams ?

3. Using ASD3Dconcrete material, shear failure is possible (it has a certain load capacity), but using a multilayer shell element, the shear capacity is zero?I don't understand this ralation. Is there somewhere a description of the layered shell element used in opensees from a mathematical point of view . The page that openssees in STKO does not have much information about it. (http://www.luxinzheng.net/download/Open ... enSEES.htm)

4. Is the convention of internal forces in a shell element available somewhere? In the isntruction of STKO it is only that the forces refer to the local coordinate system. But what is, for example, the gamma of y13, y23, y12 in the section fiber strain result.

5. In summary, the main issue is whether yielding of the reinforcement due to bending or shear failure will occur first? Since the element has no shear resistance (as I understand it well, the multilayer shell element is responsible for this) and not asdshellq4 ? Unless only concrete is responsible for out-of-plane shear resistance ?

6. Just do I understand your procedure correctly. The procedure that you performed by adding Plateformplanestress caused that only bending damage can occur?

Best regards

I have made analyses for mesh sizes 0.7 and 0.4. For 0.7 the result of deflections I got as for elastic anlysis Uz=-0.02m, for size 0.4 I got UZ=-0.3.
Still the result depends on the mesh size, but the deflections are not of the order of 1.3m.

I knew about that. I just wanted you to realize what is going on.

This is how it should be done, do completely get rid of mesh-dependence: don't use point load / point connections: In this example I kept the columns and slab separated, and joined them via rigidLinks. There are other ways to do the same. For example you can attach the columns (with a boolean operation) to the piece of slab representing the column section, and assign an elastic rigid section to that portion of the slab. But it's up to you. The idea is: the column, modelled as a line, should go in contact with a finite portion of the slab, not to a point of the slab

1. You wrote that the slab failed due to shear (Vz) and that the multilayer shell element does not contain shear reinforcement. Then how much (or what) is the shear capacity of the slab? E.g. in designing according to the Eurocodes, the shear resistance of a slab without shear reinforcement is always checked first (just bending reinforcement is taken into account, so my 0 and 90 degree reinforcement).

In that case the shear capacity of the slab will be the shear strength of concrete only (almost same as ft) multiplied the thickness of the slab. This will give you a shear strength per unit length

6. Just do I understand your procedure correctly. The procedure that you performed by adding Plateformplanestress caused that only bending damage can occur?

Bending and membrane, but not out of plane shear

Dear STKO,
thanks for the model. It has helped me a lot. In addition, I changed the columns to fiber sections yousing displacement based formulation and everything works.
I have one more quastion:

In that case the shear capacity of the slab will be the shear strength of concrete only (almost same as ft) multiplied the thickness of the slab. This will give you a shear strength per unit length

.

I found an article in which the damegeTc3D material is first attributed to the nD.plateFiber and then to the layerd shell element. You have used the nd.PlateFromPlaneStress command in the model to neglect shear damage out of plane.
What happens if I first assign the ASD3D material to a nd.plateFiber, omitting the nd.plate from plane stress?
In addition, I see that in STKO I can do both. First asd3d----then nd.platefromplanestress --- then nd.plate fiber --- then layered section.

In the webinars on the STKO website, the concrete material was generally attributed to layerd fiber cross-section, but I understand these were walls and there was no out-of-plane failure.


In addition, I have done some research on layered shell elements.
The STKO refers to http://www.luxinzheng.net/download/Open ... enSEES.htm.
One of te authors is prof. Guan H who is the author of the LFEM formulation. (nonlinear Layered Finite Element Method).
In one of her older papers it is described that the shell fiber element is suitable for punching analysis, that is out of plane shear. Since Prof Guan is the author of the article referred to by STKO, I was surprised by this provision:

Because the shell section does not account for shear reinforcement.

I found an article in which the damegeTc3D material is first attributed to the nD.plateFiber and then to the layerd shell element. You have used the nd.PlateFromPlaneStress command in the model to neglect shear damage out of plane.
What happens if I first assign the ASD3D material to a nd.plateFiber, omitting the nd.plate from plane stress?
In addition, I see that in STKO I can do both. First asd3d----then nd.platefromplanestress --- then nd.plate fiber --- then layered section.

• ASDConcrete3D (or DamageTec3D) is a 3D material (6 voigt components: s11, s22, s33, s12, s23, s13)
• The shell elements want 5 components (in shells the s33 is assumed to be 0)
• The PlateFiber material transforms a material from 6 components to 5, imposing s33 = 0. Typically you should use it before putting a 3D material into a shell section, because not every material can convert itself automatically from 3D to PlateFiber, however, the ASDConcrete3D can do it automatically, so it is not strictly necessary for it.
• With PlateFiber (or 3D converted to PlateFiber) you have 5 non-zero components, among which s23 and s13 are transverse shear components.

In addition, I have done some research on layered shell elements.
The STKO refers to http://www.luxinzheng.net/download/Open ... enSEES.htm.
One of te authors is prof. Guan H who is the author of the LFEM formulation. (nonlinear Layered Finite Element Method).
In one of her older papers it is described that the shell fiber element is suitable for punching analysis, that is out of plane shear. Since Prof Guan is the author of the article referred to by STKO, I was surprised by this provision:
Because the shell section does not account for shear reinforcement.

I didn't say you cannot use it for punching shear. I meant:
In a shell you can only model in-plane reinforcement for membrane and bending actions.
If you use the PlateFiber (and not the PlateFromPlaneStress) the transverse shear components will be treated nonlinearly, but the only belong to concrete. So it's fine if you are modeling slabs without shear reinforcements. But if you have shear reinforcement (not available in shells) you will underestimate the slab strength

Dear STKO,
Thank you very much for your help.

This is how it should be done, do completely get rid of mesh-dependence: don't use point load / point connections:

I have one last problem with this topic

The initial model assumed a single-span slab and was a test model.
I would now simply like to investigate how the multi-span and multi-storey model behaves.

Copying the model horizontally, I created a multi-span slab, copied the RIGID LINK connections to the new columns, then selected ONLY the slabs and gave the MERGE option.

This way worked and I think it is appropriate?

Unfortunately, I have a problem copying the model vertically, i.e. adding one storey. The analysis is not progressing. I tried, creating a new rigid link only for the nodes of the first storey, I tried to MERGE only the columns but this caused the original rigid link to disappear.

Then I also assigned the original rigid link to the nodes of the new storey and this caused a strange link between the columns.
In the deformation it looks like the existing slab is not connected to the columns. In simple analyses I was giving MERGE to the whole model and it was ok, but now because of the load distribution over the area of the columns, I don't know how to deal with this problem.

Can you fix my model, please?
Thank you for your help

.

As you noticed, interaction can be tedious to handle, especially when the model gets complicated.
In such cases, you can find an alternative (equivalent) solution.
What you want to do, from a physical point of view, is to make the portion of the slab under the column section, rigid. Instead of you using interaction with kinematic constraints, you can simply make those portions approximately rigid by using an elastic section slightly stiffer than the real one.
In this example I used an elastic section with a E 100 times stiffer than the original one.
In this way you can simply merge slabs and columns in a single geometry