Data analysis-elastic properties computational

[DieSure]

Hi Louise,

It helped a lot! Thanks you~Now I know why the single layer unit cell model does not have a periodic boundary condition for FaceE and FaceF. And if I'm trying to model a through-thickness unit cell, I should manually change the periodic boundary conditions of FaceE and FaceF (and corresponding edges and nodes) because they have no images in the Z direction, right?
About the rxy term in equation 12. I just didn't understand why shear strain terms appeared in the last two directions. To me all three directions should be treated the same. Perhaps I need to read through it more carefully.
Thanks.

Shuo

[louisepb]

Hi Shuo,

If you want to model a through thickness unit cell simply choose the Material Continuum option and that will give you the through thickness results as well, with boundary conditions for all three pairs of faces.

The shear values in equation 12 result from the substitution of equation 10 into equation 8.

Best regards,

Louise

[DieSure]

Hi Louise,

Thank you for your help. I did use the material continuum option. My question is since the top and bottom surface (FaceE and FaceF) are free surfaces they should not have any periodic boundary condition in Z-direction, is that right? The periodic boundary conditions on these two faces in Z direction would impose extra constraints to the unit cell. The current periodic boundary conditions are derived from a cell which has images in all three directions. I got the full strain field of the unit cell and the top and bottom surfaces deformed as there are images above and beneath them, which is not the case. Am I getting this right?

Thanks

Shuo

[louisepb]

Hi Shuo,

Sorry for the delay in replying. The material continuum method was developed with the assumption that the unit cell is small in comparison to the overall material and that it repeats in all directions. You are right, this is not the case for a single layer of weave which is why the 2.5D option was developed. In our tests we have found very little difference in the results for the values output by both the 2.5D and 3D methods. If, however, values in the z direction are to be calculated then, in order to use this method, we have to assume there is a continuum in all three directions.

Louise

[dyeyanie]

Hi Louise,

It means that if I choose a 2.5D method so I'm constructing a plane stress analysis to the geometry and this define the in-plane behaviour of the geometry. Am I right? How about if I assume as a material continuum to the geometry even the thickness is considered thin. Do Material continuum and 2.5D results showing a big difference?

Yanie

[louisepb]

Hi Yanie,

We have used both the material continuum and 2.5D analysis on a 3D orthogonal fabric and found very little difference in the results for Ex and Ey between the two. You can always try both ways and compare the results.

Louise

[dyeyanie]

Hi Louise,

Sorry, I have another questions here regarding the data obtained.

Right now, I'm trying to have only the yarns section and I would like to determine the elastic properties for these yarns. Could I just follow the same step as similar to the computational method for yarn+matrix? However, I obtained 2 types of variable solution if I just cater the yarns. I'm not really sure how to analyze them. Hope you may help.

Yanie

[louisepb]

Hi Yanie,

You should be able to create a voxel mesh for just the yarns and apply the same method as before. I'm not sure what you mean by "2 types of variable solution" - could you be more specific please?

Louise

[dyeyanie]

Hi Louise,

if that so then it's clear now. What I meant by 2 types of solution is that the displacement variable and rotational displacement rotational in abaqus. But then, i guess it's fine because the values of displacement rotational are all zero.

yanie

[dyeyanie]

Hi Louise,

I'm trying to use the python script for automated extraction of elastic properties. However, I got a message as attached. I already copied them into the same folder. Or do I need to state the model name with the folder details?? For example; model name = 'H2'.

yanie

[louisepb]

Hi Yanie,

Your odb file and the two python files should all be in your Abaqus working folder. The model name doesn't require a path.

Louise

[dyeyanie]

Ok, problem solved. Thanks Louise.

Yanie

[dyeyanie]

Hi Louise,

I would like to double check my calculation with the automated extraction that recently implemented. I found some misinterpreted data on calculating G23 and G13.

Let say my node labels are, (which corresponds to Load 0 - load 5)
175447
175448
175449
175450
175451
175452

If I'm not mistaken, the way to calculate them are as follows;
E1=1/U1 at 175447 in load 0
E2=1/U1 at 175448 in load 1
E3=1/U1 at 175449 in load 2

v12=U1 at 175448 /U1 at175447 in load 0.
v13=U1 at 175449 /U1 at 175447 in load 0.
v23=U1 at 175449 /U1 at 175448 in load 1.

G12=1/U1 at 175450 in load 3
G13=1/U1 at 175451 in load 4
G23=1/U1 at 175452 in load 5

However, according to the .rpt that I obtained from the extraction, it shows that the data of G23 and G13 are from G23=1/U1 at 175451 in load 5 and G13=1/U1 at 175452 in load 4.

I attached here the sample of my output for load 4 and 5.

Kindly apologize me if I'm wrong.

Yanie

[louisepb]

Hi Yanie,

I agree, it is confusing! If you look at the output requests in the .inp file you will see that the order of output is reversed for ConstraintsDriver4 and 5 as follows:

***********************
*** OUTPUT REQUESTS ***
***********************
*Output, field
*Element Output, directions=YES
S,
*** FIELD OUTPUT: Output Request Fx ***
*Node Output, nset=ConstraintsDriver0
U,
*** FIELD OUTPUT: Ouput Request Fy ***
*Node Output, nset=ConstraintsDriver1
U,
*** FIELD OUTPUT: Ouput Request Fz ***
*Node Output, nset=ConstraintsDriver2
U,
*** FIELD OUTPUT: Ouput Request Shear_xy ***
*Node Output, nset=ConstraintsDriver3
U,
*** FIELD OUTPUT: Ouput Request Shear_yz ***
*Node Output, nset=ConstraintsDriver5
U,
*** FIELD OUTPUT: Ouput Request Shear_zx ***
*Node Output, nset=ConstraintsDriver4
U,

When the results are read in using dataHandling.py the shear_yz is therefore in frame[5] and shear_zx in frame[6] and they are assigned accordingly. I'm not entirely sure what the reasoning behind this was but I think that it was something to do with the order in which Abaqus stores the shear stresses. You should find that the end results are correct.

Hope that clears things up,
Louise

[dyeyanie]

Hi Louise,

I think something is wrong in datahandling.py because if I'm referring to the output results, the values that I obtained for my analysis is totally wrong.

Perhaps, I need to double check them again.

Thanks.

Yanie