Hi Mohammead,

I have been working on similar problems in the past 2 years. I have modelled succesfully FRPstrip by using an older layered element SOLID46, element thickness being the thickness of the layer (for example1mm). In this case you can use the element as homogeneous (for SOLID185 - keyopt(3)=0).

In this case you ANSYS will inform you that some of your elements are not properly shaped (which would be exactly the case). You will be able to run the analysis however. I have validated my results by experimental results and they are quite good.

There is another way to model your FRP, and I strongly recomend it, as it is much nicer to use: as you are modeling RC beams, you can use the concrete SOLID65. You can model the FRP as reinforcement through the real constant of the outer layer of your beam. Model your beam with different volumes. The one with the FRP reinforcement should not be very thick - no more than 5cm for example.

I have validated this approach, too, and it gives very close results to the one with layered element.

If you need more information, please, contact me here.

Hi Mohammaed,

I am not much familiar with ANSYS. But I think as you are using a solid element for modeling the FRP strip, you will not need to define any section. The element has its section as you define its geometry in 3D space. Definition of section is usually used for beam or truss elements. 

I hope this answer can be useful!!

Strip thickness is a geometric feature. Unless you are using elements to build geometry of RC beam, I see no reason to define strip thickness using solid element.

Hi Mohammead,

I have been working on similar problems in the past 2 years. I have modelled succesfully FRPstrip by using an older layered element SOLID46, element thickness being the thickness of the layer (for example1mm). In this case you can use the element as homogeneous (for SOLID185 - keyopt(3)=0).

In this case you ANSYS will inform you that some of your elements are not properly shaped (which would be exactly the case). You will be able to run the analysis however. I have validated my results by experimental results and they are quite good.

There is another way to model your FRP, and I strongly recomend it, as it is much nicer to use: as you are modeling RC beams, you can use the concrete SOLID65. You can model the FRP as reinforcement through the real constant of the outer layer of your beam. Model your beam with different volumes. The one with the FRP reinforcement should not be very thick - no more than 5cm for example.

I have validated this approach, too, and it gives very close results to the one with layered element.

If you need more information, please, contact me here.

The model which is quite used and simple is - you take the solid element for continuum and mesh in such proportion that later you can place a Link or Beam element through the nodes. Then you obtain homogenized fiber composite. The things are working even composite is reinforced at various angles - in this case you have to obtain the corresponding mesh allowing to do so. The method is used in practice and quite well experimentaly validated. 

First of all you should define one of shell element, Then choose section part in preprocessor section and click on the shell. In lay-up. select add/edit. A new window will open and you can add various layer with any desired orientation which represents a multilayer fiber reinforced composite. Good luck  !!!

You can model your FRP strip as an area and then use the element SHELL63. In this way you can specify for this element the thickness of your composite (by defining a specific real constant)  and attribute to the FRP areas the material properties of your composite, the type of element (SHELL63) and the real constant set (through the main menu or with the command AATT).

Dear all,

Thank you so much for your helpful answers. I am trying now  all suggested approaches by you and I will check the results. But before that, I shall define the mechanical proprieties of fiber composites.

The needed information for defining properties of fiber composites materials as an orthotropic material is:

Modulus of elasticity (EX,EY,EZ)

Poisson Ratio (PRXY,PRXZ,PRYZ)

Shear Modulus (GXY,GXZ,GYZ)

&

Maximum Tensile Strength or Stress (Stress Limit)

Maximum Strain at Failure (Stain Limit)

E, PR, and G can be defined in ANSYS from:

Preprocessor>Material Models> Structural>Linear > Elastic > Orthotropic

But, How I can define the stress and strain limits in the preprocessing stage?

I tried to define it using

General Postproc>Failure Criteria>Add/Edit

But it did not work, and regardless of the entered values of strain and stress limits, the solution will not be affected or changed, as if ANSYS is not considering these values during preprocessing stage (analysis stage).

So, how I can define the fiber composites stress and strain limits in a way that will be considered in the analysis stage?

Regards

Dear Mohammead,

To define the maximum stress and strain, you can add to the deffinition of your material model a multilinear elastic properties (Preprocessor->Material Models->Nonlinear->Elastic-> Multilinear elastic). As FRP is actualy a linear material, you need only one set of stress-strain values, namely the limit ones. Make sure that the strain/stress ratio is exactly equal to the modulus of elasticity, else your analysis will not run (ANSYS will give you an error massage about it, so there is no way to miss it).

However, keep in mind that if you want to model the FRP as a reinforcement in SOLID65 (see my previous post), you will not be able to use orthotropic material model. In that case, if you have fibres in two dirrections, you can define two different isotropic materials, using the modulus of elasticity and Poisson ration for the relevant direction, and then model the FRP as two different reinforcements. I am not sure how well this would work though, as I have not actually tried that one - I have only used one-way fibred materials for my models, so I use one material with the charachteristics of the main direction.

Best regards, Tanya

Dear Tanya Chardakova

I tried to define the stress and strain limits for CFRP strip - defined as volume with Solid185 (layered) - using multilinear elasticity, but unfortunately ANSYS gave me an error message that (TB, MELA plasticity option is not currently supported by Solid185), what means that Solid185 is not supporting this material model. This material model is supported only by two elements: Solid65 and Solid62.

I don not know how things will work now!

Regards

Hi, Mohammead,

If your element does not support MELA, try MISO instead (Preprocessor->Material Models->Nonlinear->Inelastic-> Rate Independend->Isotropic Hardening plasticity->Mises Plasticity->Multilinear).

I hope this works better!

Dear Muhammad Zeeshan Siddiqui

Regarding modeling the CFRP strip, when I am modeling it as a volume using Solid185, with an element thickness equal to strip thickness (0.5 mm for example), ANSYS will warn me that element aspect ratio has been exceeded, and this is right, because the RC beam mesh elements (with Solid65) are 25mmx25mmx25mm, and I am bonding the new CFRP strip to this beam with its original mesh. (The RC beam is 3200 mm length)

That is why I was asking about the relation with layer thickness defined in shell section, and what thickness ANSYS will consider, but as you said before , the thickness of volume will override any thickness definition by the shell section in case of inconsistent values.

I was thinking that I can enlarge the CFRP strip volume thickness, and depend on the layer thickness defined in the shell section, but things came wrong.

The problem now, that I have to use Solid185, since it is the best choice to model fiber composites materials, and I do not know how to define the small thickness of the CFRP strip when meshing the strip volume, without exceeding the maximum aspect ratio. Keeping in mind, that I can not re mesh the RC beam with a very fine mesh consistent with CFRP strip to be in the range of shaping limits.

So, I hope that you have any ideas about getting out of this problem.

Regards

I general, the critical element of the composite is the bond layer. You can model this in two ways:

1. CFRP area as a reinforcement (line element) and then the interface properties or bond-slip behaviour can be assigned.

2. CFRP sheet as a volumetric element as you did. The same thickness can be assigned. Then the epoxy layer should also be included as a volumetric element or can introduce interface properties since the thickness of adhesive layer is negligible.

The 1st one is more accurate than the second one.