Data analysis-elastic properties computational

[dyeyanie]

Hi Louise,

I trying to analyse my data collection in order to obtain the elastic properties. However, I just found that there is no history output in the computational. normally, to plot a data in abaqus, field output and history output are needed (i'm not sure if there is another way to do so). Some more, I'm wondering to which equation that are you referring to for the elastic properties computational. Is it similar to the one in S.Li paper? i would like to obtain the mean value of E, v and G of my computational.

Yanie

[louisepb]

Hi Yanie,

I'm afraid that this is outside my field. My colleague specified the .inp format required from TexGen to implement the boundary conditions and load cases as specified in Li's paper. I'm afraid that I have no experience of actually using the output to get the material properties. Unfortunately my colleague is away at the moment so I can't get further information from him right now.

Louise

[louisepb]

Hi Yanie,

I've taken another look at this and reminded myself of what is going on. As I understand it the loads are applied at the constraint driver nodes and are scaled as Nm per unit volume. So, according to equation 31 in Li's paper these are equivalent to the macroscopic stresses. The output from the analysis is specified to be the displacements at the constraint driver nodes. The material properties can therefore be calculated as in equation 32 of the paper.

Hope that makes sense. I will double check that this is correct when my colleague returns.

Louise

[dyeyanie]

Hi,

thanks anyway. I'll summarise my data then. Looking forward your updates with regards to this.

Yanie

[dyeyanie]

Hi Louise,

I just viewed my output on Von Mises stresses with varies of fibre volume fraction. however, I found that there is no differences between them. I did the changes in linear density and fibre area to ensure the differences in fibre volume fraction were obtained. is there anything else that i left correspond to this matter? DO I need to save everytime I made changes? What is did is , once changed I straight away converted them to ABAQUS inp files. Is that wrong?

Yanie

[louisepb]

Hi Yanie,

I have asked my colleague and my earlier answer about calculating the material properties is correct.

As far as seeing the results of changes in volume fraction in your simulation goes: If you look at the .inp file you will see that the .eld file isn't actually read in and used in this case. The volume fraction information is indeed output in the .eld file but if you want to use it then it is up to you to add something to the .inp file to read in the data and decide how you want to use it in your simulation.

Louise

[dyeyanie]

Hi Louise,

Thanks for your explanation. But I'm not really clear on the displacement output for every load cases. why don't we just identify the E (strain) straight away?

Actually I'm not good in commenting . Thus, I'm glad if oyu could show me the way on how to modify the inp file so that the eld files will be read in the simulation.

Yanie

[louisepb]

Hi,

As shown in section 8 of the paper the displacements for the different load cases allow you to obtain the different material properties eg Young's Modulus (E) in the x, y, z directions etc.

I'm afraid that writing Abaqus input files isn't my field of expertise. You'll need to consult the Abaqus reference manual to find out how to do this.

Louise

[dyeyanie]

HI Louise,

Ok, I got your points. In another words, it means that the relative displacements obtained from the different load cases are act similarly as strains in every axes, right? Hence, we could obtain the values of E, nu and so on.

Will check on how to include the .eld files. Many thanks.

Yanie

[dyeyanie]

Hi Louise,

Sorry I get lost again in extracting the output that I have. I would like to calculate the E properties as expressed in Equation 32. Thus, do I need to proceed the average processes in order to get the E?? From what I have here, I will have 6 load cases frame and 6 displacement data. How could I extract them precisely?? Sorry I not really good in extracting data from ABAQUS output. Hope you could help me.

Yanie

[louisepb]

Hi Yanie,

As shown in equation 32 the 6 load cases/displacements will give you the 6 moduli - Ex, Ey, Ez, Gxy, Gxz and Gyz.

Louise

[dyeyanie]

Hi Louise,

That's not the issue. What i mean is the stresses output in abaqus as same as derived in equation 31?

Yanie

[louisepb]

Hi Yanie,

Please make sure that you understand the method being used here. You do not need to average stresses from the Abaqus output because the load is applied volumetrically as described in Equation 31. Because the load applied in the .inp file is equal to the unit cell volume the stresses as given in equation 31 are all one. Therefore in equation 32 the output at the virtual nodes used represents the strain and E etc is simply 1/strain.

Louise

[DieSure]

Hi Louise,

I'm not sure I understand the method right. Here is what I thought. The 6 ConstraintsDrive nodes are introduced to impose all the periodic boundary conditions. The load is then applied to these nodes and volume averaged to the unit cell. And the strain output from these nodes are then the macroscopic strain of the unit cell. Am I getting this right? I do not really understand the rxy,rxz, and ryz terms in Equation12.2 and 12.3 in S.Li's paper though. And also, this type of periodic boundary condition can not be applied to bending?

I'm little confused about the periodic boundary condition options for ABAQUS Voxel output. Is the option material continuum for in cases like layered 2D woven laminates, and the single layer RVE for cases like 3D through-thickness orthogonal weaves? When I use the single layer RVE option the loads only apply to constraintsdrive0,1, and 3. Should I just apply similar load to all other nodes to get modulus in other directions? And how about poisson's ratio? For the moment I apply tensile load directly on surfaces to get all of that. Is there any better way to do so?

Thank you very much. I got a lot of questions here

Shuo

[louisepb]

Hi Shuo,

Answering your questions in order:

As shown in Equation 32 of the paper there are 6 load cases each applied separately to the ConstraintDriver nodes. If you look in the .inp file then you will see how the load cases correspond to the cases in Equation 32. The output from these nodes then correspond to the macroscopic strain.

In Equation 12.2 and 12.3 I assume that by rxy etc you mean gammaxy etc, ie the shear strains, as specified in Equation 8.

These boundary conditions, as they stand, cannot be applied to bending.

In the TexGen voxel output option the Material Continuum case is that described in the paper. Because of the load cases, as described above, the output will give the modulli corresponding to each load case. This is nothing to do with the type of weave being modelled. The 2.5D method was developed (called single layer RVE ) in order to reduce the computational load. In this case the use of only constraintsdrivers 0, 1 and 3 mean that only the Ex, Ey and Gxy will be calculated - no through thickness properties are calculated.

You don't need to apply loads - because it is a material continuum, Equation 8 means that, by taking the results at an arbitrary point (ie the ConstraintsDrivers) the strains are produced.

The calculation of the poisson's ratios is also described in Equation 32 and are calculated directly from the strain outputs from the load cases.

Hope that helps. It does take a bit of getting your head around!

Louise