Information on mechanical simulation by MEF Catia

Out of category
1
Hi all
 
I am currently doing my internship in England, the company I work for would like me to do the modeling and mechanical analysis of a Catalan vault. However, I have not received any training in the use of the Generative Structural Analysis Workshop . 
So I am writing to you to ask for your help.
First question that may seem silly, do you know this workshop of Catia?
 
The Catalan vault that I have to study is composed of at least 3 layers of tiles which are held together by a mortar.
My first question is: Do we have to model the mortar, because it plays an important role in the recovery of the forces, or its action on the tiles is only to "glue" it together? If not, we can exclude it from the analysis. (Through a document I was able to read the following statement: 

The role of the binder as a guarantor of cohesion is considered negligible because it is the element most likely to vary over time. It is therefore not taken into account in mechanical analyses and calculations, even though it is very important for a homogeneous and regular distribution of loads. And is it correct?)

 

On the contrary, if mortar has a great influence on the analysis of the structure, how can we model it? How can we model the interactions between mortar and tiles?

 

Since my vault is made up of several layers of tiles, is it better to create a model representing reality (i.e. a vault created with tiles that we can see clearly) or is it simpler to create a uniform model (i.e. a solid with the same dimensions as a vault created with several layers). I would like to know whether the mistake we are making in creating a uniform model is negligible or not. 

 

If we have to create a vault composed of all the tiles necessary for its manufacture, can we create a specific mesh? (This is to avoid assembling all the tiles which will be long and tedious).

-       

      Do you know if it was possible to display on catia, in the Generative Structural Analysis workbench, the pressure lines/Thrust line in English of a structure. (Or something similar)

Thanks to these lines, we can know if our structure will be resistant or will collapse.
Below the link explains in more detail the importance of pressure.
 
I hope you can give me some answers to my many questions, which I hope are clear.
 
Thank you in advance for your answer and for taking your time to read my message.
 
Kind regards
2

Hello, I don't have the GSA workshop but first you have to check that you have all the modules.

for example, if you don't have Generative Assembly Structural Analysis, you won't be able to simulate an assembly.

Below is an excerpt from the GSA CatiaV5 doc

Generative Structural Analysis Workshop at a glance

The Generative Structural Analysis  Workbench allows you to quickly perform first-class mechanical analysis of 3D systems.

This workshop is composed of the following products:

 

The Generative Part Structural Analysis (GPS) product is aimed at the average user. Indeed, its intuitive interface allows you to obtain information on mechanical behavior with very little interaction. The dialog boxes are self-explanatory and require virtually no methodology because the definition steps can be performed in any order.


ELFINI Structural Analysis is an extension of the above product that is based entirely on the Version 5 architecture. It forms the basis for the development of future mechanical analysis tools.


Generative Assembly Structural Analysis (GPS) is a very useful extension of Generative Part Structural Analysis that allows you to study the mechanical behavior of an entire assembly. It has been designed with the same respect for the principles of "pedagogy" and "conviviality".


The Generative Dynamic Analysis (GDA) product allows you to work in a dynamic response context.

3

Re hello franck.ceroux.

 

It seems that you can answer all my questions and I am delighted about that.

I have the GSA workshop without any hesitation. But not the ELFINI Structural Analysis EST workshop.

I can read that it seems that GSA is a "simple" module if I may say so. However, I think I can do very good simulation with it, right?

Not being a structural analysis engineer, but an intern, I think my company will accept that I don't give it the perfect answer. In the first instance, this will allow them to have orders of magnitude I think.

Kind regards

4

On the practice of the GSA workshop, I don't have it either and it's been more than 10 years since I've touched it. So on this point, sorry but I won't be of much use.

 

On the need to model the mortar, I would say that if it is only used as glue and its thickness is small compared to that of the vault, it is not worth modeling it (case of the classic gluing between 2 metal pieces for example).

If the thickness is greater, then there is a risk of shearing in the thickness. In this case, it is not necessarily necessary to model the mortar, but it is at least necessary to be able to recover the forces to be able to check the resistance. Since I don't know if it's possible with Catia, it may be faster to model it and link the contact surfaces.

This should also answer the question of simplification by a single volume representing the entire structure. This assumption is only correct if you are sure that there is no slippage between the different layers. In other words, that the collage is "perfect".

 

Obtaining the pressure lines is, a priori, possible since the stress results are expressed in units of pressure (MPa generally). To get the results in the thickness of the material, it is better to use a volume mesh. Be careful in this case to have at least 3 elements in the thickness of the vault (otherwise Catia can give very eroded results).

 

1 Like
5

Hi all

Chamade, thank you for your answer. That's what I thought about the mortar.

My vault being very particular, its thickness is very small, about 40 to 50 cm for a vault with a span of 4 to 5m (yes, I said meter).

So no the thickness of the mortar should not be very important, if you put 5 mm thick for a tile that is 20 mm thick I think it's not bad already.

So for the slippage I'm not sure. I think we shouldn't have one, otherwise the vault will collapse. I will try to find out from someone.

 

So you think Catia could give me a pressure line, do you have a little clue to "activate this function"? (Because I can only see the deformations, stresses and Von mises, main constraints, so is it hidden somewhere?)

On the other hand I don't understand what you mean by 3 elements in the thickness? That is to say 3 different "objects" (so my 3 layers of tiles?).

Kind regards

6

If you put 5 mm of mortar every 20 mm (there is no unit in your message), it makes the mortar occupy 20% of the total volume. This is not really negligible.

For the vault to hold, there must be no slippage between the tiles. The question is whether you are sure that the mortar will withstand the shear stresses that will be applied to it. If so, no problem. Otherwise, you won't be able to analyze it with a simplified model with a single volume.

 

Concerning the pressure lines, these are the "trajectories" on which there is the most effort, and therefore constraints. The display of Von Mises constraints, for example, must therefore give the right result. Catia may allow you to have an isobar display to have it in the form of curves.

For the number of elements, for each distinct volume of the model (e.g. each tile if they are modeled separately), the mesh of the FEM (finite element model) must have at least 3 elements (cubic, tetrahedron, etc.) in the thickness.

Example: for a 21 mm thick tile, there must be at least 3 elements of 7 mm in the thickness (on the entire surface and not just on the edge).

7

Hello Chamade again,

Sorry yes it's 20 mm and I forgot.
Afterwards, concerning the thickness of the mortar, I moved a little too quickly. I can't tell you what thickness the company is going to want to use.

But they will try to use an optimal amount so as not to have waste. (I put the company back in its environment. It is a research company in new materials that are more environmentally friendly. In order to make the world of construction less polluting. For example, they want to use tiles that contain no or very little cement, and the same goes for mortar. So during the construction they will make sure to use the mortar without waste).

Regarding the slip between the tiles, so if the mortar is strong enough or not, I am unable to answer you. For the moment the samples are being tested and I am waiting for the test report.
But I think (hypothesis again) that they are trying to obtain a mortar with the best possible mechanical properties without or little cement. So it should withstand the shear stress. (At least you have made me aware of this problem of shear strength)

Concerning the pressure line, I'll see the idea of isobar lines. 

Okay so if I understood correctly the mesh must be thin enough so that we can have 3 meshes in the thickness?

For information at this stage my vault is only built of one block  per layer, I have not modeled the vault by the successive assembly of the tiles (this may make a very heavy file since it must have at least 1250 tiles for the smallest vault). 

However, is it better for me to model the vault in the most real way or can my modeling be acceptable? (I am aware that I am going to make an approximation of the structure so a "mistake" but which may be acceptable).

Kind regards

 

 

8

For the question of the number of elements, it is indeed a problem of mesh finesse.

The hypothesis of creating each layer in a single piece and not tile by tile does not shock me. A well-designed vault must actually hold itself in place under its own weight by contact. In the case of very fine structures like this, however, a buckling calculation can be a good idea to reassure yourself.

Moreover, as each layer of tile is very thin in relation to its span, a solid model may not add much. Unless the total thickness of the different layers is modelled in a single volume.

If only one layer of tile is considered, the stress gap between the bottom and top face should not be very large. A surface model would then be much more efficient.

Any calculation model contains some simplifications anyway. This is also why we take weightings and safety coefficients on the efforts, constraints, etc. Then, to quantify the differences between 2 types of modeling (e.g. one-piece layer or tile by tile), it is possible to make a comparison on 2 models of reduced size (e.g. 1m x 1m). The load applied in this case does not matter. What you have to look at is the relationship between the results.

 

9

Hello

I was thinking of creating a volume model because if we have 3 layers, these will have a different orientation namely 0°, 45° and 90°.

When you think of a surface model, do you think of a model created with the Generative shape Design workshop or with the Advanced Meshing Tool?

Kind regards

10

The orientation of layers must be managed directly in the element properties. But this does not require a volume model.

To make a surface model, it is a question of creating an average surface between the upper and lower face. Then, the mesh is made with shell-type elements. They are the ones that contain the thickness information.

There is nothing to prevent you from layering on top of each other. A surface model will be calculated much faster than a volume model. On the other hand, it will be a little less precise if we want to study phenomena very close to an external face. But as a general rule, on an FEM, it's best to avoid looking at what's happening too close to the boundary conditions.

As for the practice of the software, as I said before, it's been too long since I've practiced it.

11

Hello Chamade,

Sorry to answer so late but I tried the solution of making a surface model.

To do this, I used the Generative shape Design and Advanced Meshing Tool workshops . The first to define the geometry for the second for the mesh. Then I did the analysis using the GSA workshop.

This allowed me to make the comparison between my 3D and surface model. In the 2 models, the vaults have the same dimensions and are only subject to gravity.

For your information, the vaults have a surface area of 3m² (surface of the upper surface). 

The material is classic concrete, taken from the catia library.

I was able to make the following observations:

The surface model is calculated faster, about 5 minutes.

The 5-hour volume model.

For the 2 models I get as maximum displacement 0.0269 mm (3D) and 0.026 mm (surface).

On the other hand, I have a difference for the Von Mises constraints.

In volume we have 0.259 MPa (i.e. 2.59E5 N/m²), in surface 0.199 MPa (i.e. 1.99E5 N/m²).
So we have a difference of 0.060 MPa. This gives us about 17.7 tons.

Not having any experience/hindsight on this type of analysis, in your opinion is this difference acceptable or on the contrary significant. That it shows that one of the models is more accurate, or that I made a mistake in my initial assumptions.

For me I am surprised by this difference and I wonder if I have not made a mistake somewhere (Because my vaults have a span of 3000 mm, 40 mm thick, and a length of 1000 mm, and I have a Delta of 17.7 tons. Tons! (Unless I made a mistake in converting units).
 

Thank you in advance for your feedback,

Kind regards

12

Hello

No need to apologize? I'm not the one who has the problem. So not me waiting.

 

Otherwise, the 2 results seem to me to be quite correct and comparable. 0.06 MPa difference is almost negligible. This verifies that the surface model is much more efficient.

As a result, I admit that I don't really understand where this result of 17.7 tons comes from. Could you detail how you got there?

Would it also be possible to have some views to better understand where the gap is?

13

Hello

Let me explain for the 17.7 tons (I take rounded values though):

I have a difference of 0.06 E5 N/m², or 0.06 N/mm².

I have a surface area of 3,000,000 mm².

We have a Sigma constraint in MPa, and I'm using the formula.

Sigma = F/S.

F = Sigma*S = 0.06 * 3,000,000 = 180000 N

Now 1 kg = 10 N (or more precisely P=m*g).

m = 180000/10 = 18,000 kg, i.e. 18 t.

 

How can I insert a photo on the form, I can't seem to take them directly from my documents.

In advance, the difference is mainly at the level of the interlocking connections, i.e. where the vault will rest on the walls. (Left and right ends of the vault). 

14

That's what I told myself. But this reasoning could only be true if the vault is supported on the entire underside. With the images it will certainly be possible to say more.

To attach your images, put them in a word or a PDF and post it as an attachment in your answer.

 

You say you're on an internship. What exactly is this an internship? In the context of what training?

15

I am doing an internship as part of my engineering school curriculum. In order to graduate, I have to do an internship abroad. After the exact title I couldn't tell you exactly, the company being very very small (6 people) we do a little bit of everything.

Even if it's a bit special since I'm an apprentice at the same time for Constellium.

I am in PMOM (Process and Implementation of Materials) at the University of Technology of Troyes (UTT), it is a work-study program (2s in a company/ 2s in progress).

I attached a pdf with the screenshots and a small question inside.

Thanks for the help anyway.


capteurs_image_voute.pdf
16

I found an answer to one of my problems:

There are missing boundary conditions in motion, and therefore the matrix is singular: there are still motions of rigid solids. The linear system cannot therefore be solved. 
Catia allows you to visualize the movements that should be blocked: 
right-click on static solution (or other)/Image generation/Translation at nodes -> for each component, see if the solid is barred in one direction. 

Normally, if we model the system environment well on the first try, there should be no rigid field modes.

 

However, I'm very annoyed, it's the middle voussoirs (or the keystone) that is the problem. It could be in motion. Which is quite possible. 

In reality, it is only in contact with the other voussoirs, it has no connection, embedding or other with the other stones.
How can I solve my "singular matrix" problem? Should I add recessed connections to the joints of the stones or not?
 

17

I found an answer to one of my problems:

There are missing boundary conditions in motion, and therefore the matrix is singular: there are still motions of rigid solids. The linear system cannot therefore be solved. 
Catia allows you to visualize the movements that should be blocked: 
right-click on static solution (or other)/Image generation/Translation at nodes -> for each component, see if the solid is barred in one direction. 

Normally, if we model the system environment well on the first try, there should be no rigid field modes.

 

However, I'm very annoyed, it's the middle voussoirs (or the keystone) that is the problem. It could be in motion. Which is quite possible. 

In reality, it is only in contact with the other voussoirs, it has no connection, embedding or other with the other stones.
How can I solve my "singular matrix" problem? Should I add recessed connections to the joints of the stones or not?
 

18

I finally tested something that seems to work.

I used the function which is called "Soldered Connection Property".
And this allows me to solve my singular matrix problem and I get similar results to the other models.

Example: I have 0.205 MPa with this model compared to 0.199 MPa for the surface model.
After which is the most correct is a hell of a question, which will surely have to be verified by a small real test. 

19

I finally tested something that seems to work.

I used the function which is called "Soldered Connection Property".
And this allows me to solve my singular matrix problem and I get similar results to the other models.

Example: I have 0.205 MPa with this model compared to 0.199 MPa for the surface model.
After which is the most correct is a hell of a question, which will surely have to be verified by a small real test. 

20

Hello

I confirm that you should not take into account these maximum values and that there are absolutely not 18 tons of additional loads between the 2 models.

First of all, as I have already said, the results of a FEM should not be taken at the level of boundary conditions (embedding in this case). This creates digital overconstraints that are not real.

On the other hand, having less than 1 MPa difference between 2 models is not significant either.

 

For the calculation of stresses, you must have heard that the load in a section is broken down into normal and shear force and moment. To obtain the 18 tons, you considered that there is a compressive force on the entire surface of the vault. Now, you are here on a problem of bending between 4 points. Which is not the same at all.

 

For the question of assembly, all the pieces must be "glued" together for the calculation to work. But I do believe that assembly constraints are not automatically converted in the calculation workshop. We need to reconnect with each other.

 

After that, we shouldn't be surprised to have slight differences from one model to another. Slightly modifying the mesh will inevitably impact the result. We must not forget that this is only a model and that there is an intrinsic element of uncertainty. One model cannot be said to be more accurate than the other in this case.

1 Like