Modelling of unit cell of woven composite in ABAQUS

[amrah]

Hey Anurag,

I am a student doing my masters in Aeronautical Eng. I am trying to model a 2x2 twill weave (modelled in texgen and imported to abaqus as voxel mesh, with periodic boundary conditions as material continum and element type as c3d8r) and I have come across the same two warning as you have mentioned above, in the .dat file. What modifications/changes did you make to run the analysis.

Kind regards,
Amrah

[anuragdixitiitd]

Hello amrah,
Nice to know about your masters. Coming to your problem instead of directly importing the model (.inp) file in ABAQUS CAE try to run the .inp file from the command window in ABAQUS. From that you will obtain .odb file. Your errors significantly reduces.The command prompt to run the .inp file is:
At the command line
abaqus job=filename int (in the file name do not write .inp)

Hope that helps!!!!
Regards
Anurag

[patricia_arnv]

Hi everybody,

I'm new using TexGen and I'm very glad of finding this forum so useful for so many of you. I'll start explaining you all what I'm actually working at. I was using WiseTex software to model several textiles, since my main objective is to numerically predict both elastic and strength material properties for different combinations of resin and textiles. The problem is that the mesher that Wisetex software pakage uses is quite obsolete, since it doesn't deal with the yarn interpenetration problem and is not capable of exporting the matrix volume (it only exports yarns), so I have decided to start using TexGen. Fortunately, I have found the voxel mesher very useful and easy to use, but I would like to know compute a tensile test using the same periodic boundary conditions. To do this, I am directly writing into the ABAQUS .inp file, changing the static linear pertubation for a static general linear analysis and applying a linearly time increasing force to the constraint driver 0, keeping the rest of the forces applied to the constarint drivers as 0.

Since I have seen that Anurag has asked here in this topic about which conditions to apply in order to simulate this, I was wondering if you have made any advance on this and could help me del with this matter. And I would also like to ask Louise if you have ever tried to simulate something similar to this. If you have, can you please give me some hints? Does what I have said sound consistent?

Thank you very much in advance for your help.

Patricia

[anuragdixitiitd]

Hello Patricia,
First of all sorry for the delay in post.Nice to hear that you are also working in the same area. May I know what exactly your problem is. As far as the elastic properties are concerned ABAQUS voxel mesh will be helpful. The point is that after obtaining the .inp file you will have to run it using the command line option in order to retain the compatibilty in BC. After running the .inp file you can follow the method prescribed in my earlier thread for elastic property computational.
I hope this helps.
Regards
Anurag

[patricia_arnv]

Hi Anurag;

First of all, thanks for the quick response. Iĺl try to clarify what my problem is. I've already dealt with the elastic properties computation and now I interested in further analysis...I would like to numerically model a tensile test implementing a damage model to both matrix and yarns, up to textile failure, using a unit cell, which means that I have to keep the Periodic boundary conditions but I don know how to apply the loads. I think this is because I'm not able to clearly understand the role of the constraint nodes, because they are actually nodes in ABAQUS but these are in real life actual macroscopic deformations, aren't they? So, let's say, If I want to model a tensile test; i would have to apply a macroscopic tension in 11 direction up to failure, but how can I do this in ABAQUS? Applying a concentrated force in constraint node 1? while keeping the rest of the load cases to 0?? And after computing the analysis, I would have to obtain the macroscopic deformation, would this be the displacement of constraint driver 1?

I hope I've been able to explain what my issue is. I ask to you because you asked on the forum some time ago about simulating a tensile test. Thanks a lot

Regards

Patricia

[anuragdixitiitd]

Hello Patricia,
First I apologise for the delay in reply, as i was away from my office.
For numerically modelling tensile test, first you will have to determine the strain rate at which u are performing experiment. Secondly try to maintain the Boundary conditions exactly the way u are performing in experiments (one cross head stationary and other one moving), at the moving end you can prescribe the strain rate instead of load and let it deform till the fracture occurs.
I hope that helps.
Best regards
anurag

[anuragdixitiitd]

Hello patricia,
hope you have read the reply. I wanna ask u one thing as in the previous thread u were saying that you have already done elastic property computational. I have also done the same but let me verify whether we are following the same steps. What were the loading conditions in that computational? whether we applied any load or simply followed the periodic boundary conditions without any load? While calculating the final results (E1,E2....) I got the displacements at constraint driven nodes0,1,3... as per file shown in my previous thread and calculated E1, E2... by the method described by louise in my thread. So my question is what does these final values of moduli and poissons ratio really reflect without any loading conditions. I hope I am clear .
I am also working on simulation of tensile and compressive tests of composites plates (strength analysis).
Best Wishes
Anurag

[anuragdixitiitd]

Hello Louise,
Hope you may be fine.
After successfully completing my elastic property computational. Now I am interested in compression modelling.For that I went to abaqus dry fibre option and selected the feature compression plates, but after running the .inp file from command line and obtaining .odb file I didn't find any plates in ABAQUS, though in the model tree Top and bottom plates are mentioned. Why is it so?? I wanna ask you few question regarding this.
What does X Scale, Y Scale and Z scale means in Abaqus option dialog?
From where or which option I can provide material properties to the compression plates?
What about if I want to model fibre + Matrix (combined) in TexGen? As compression plate option is only available for dry fibre only.
Thanks for your cooperation.
Best wishes
Anurag

[louisepb]

Hi Anurag,

If you view the model in CAE you will see that the compression plates are created when the option is selected. These are analytical plates and therefore do not have material properties as such and will not appear in the output file. If you look at the .inp file, however, you will see that there is a "Surface interaction, Name=Plate" command but that that no parameters have been specified. There is an equivalent section for the yarn. You may need to experiment to find if you need to specify a friction for the plate in this section or not.

The X, Y and Z scales specify the load. so, for example, if you have compression plates and want to specify a 5% compression you would enter 0.95 here.

If you want to model the fibre and matrix you will need to use one of the other export options. In this case, as you would now have a solid, you wouldn't need to use compression plates to model the compression.

Hope that helps,
Louise

[anuragdixitiitd]

Many Thanks to you.

[anuragdixitiitd]

Hello louise,

When I am imported the .inp file directly to CAE, instead of running through command line, I am not able to import some features correctly these are:
1. Abaqus/CAE allows only the first node set in a *EQUATION definition to contain more than one node. Node set BOUND0B violates this rule. The equation using this node set will not be imported.
2. The following keywords/parameters are not yet supported by the input file reader:
*INITIALCONDITIONS, TYPE=SOLUTION
*NSET, UNSORTED
Secondly: The analytical plates in the CAE are not meshed, when I tried to mesh them it denied to mesh analytic rigid part or part instance.
After that when I tried to submit the job for analysis there was problem with orientation of yarns i.e. Texgenorientationvectors no longer exists. Any ways after suppressing these orientations when I submitted the job for analysis, the Job was aborted as the NODE SET ASSEMBLY_DUMMY0 and DUMMY 1 HAS NOT BEEN DEFINED.
How to cope up from these warnings/errors??


And if I am running the .inp file from command line I am getting the .odb file and during its visualization I can easily see unit cell is compressed between two plates. But the plates are unmeshed. Should I remain them unmeshed.?
Now my question is which is the correct method of analysis:
Method 1. Importing model to CAE and analyzing it for results or
Method 2. directly run .inp from the command line and go for the results.
I hope I am able to explain it. Sorry for too many questions.
Regards & Best Wishes
Anurag

[louisepb]

Hi Anurag,

Apologies for misleading you: when I said that you could see the plates when loaded into CAE I just meant that this would illustrate that they are there - you can see from the errors that, for the same reasons discussed before, you can't actually run from CAE.

The plates are analytical and therefore don't need to be meshed. If you run from the command line then hopefully you should get some results out.

Best regards,

Louise

[anuragdixitiitd]

Hi Louise,
Thank you very much
Regards
Anurag

[anuragdixitiitd]

Hi Louise,
Sorry to disturb you again, but after much brain ache in analyzing the fabric under compression by exporting it to ABAQUS dry fiber file and running the .inp file from command line, my analysis was terminated, I faced many fatal errors and was wondering few things:
1. Where did i prescribed the boundary condition in my analysis as it was not asked during export of dry fiber file and if I haven't then what BCs my analysis is following (whether periodic I dont know???)
2. If i want to resolve/edit certain issues related to contact problem, mesh refinement,BC's,material definition of plates which command option should I follow in TexGen or whether I should make changes in my .inp file.
3.In .sta file it is suggesting to use penalty contact algorithm instead? Where i would find this option?
I hope you wont mind!
Thanking you
Best wishes
Anurag

[louisepb]

Hi Anurag,

If you look in the Periodic Boundary Conditions section of the .inp file you will see the boundary conditions for the dry fibre export. You will see that the nodes on each boundary are collected into note sets where BoundxA and BoundxB represent matching nodes on opposite sides of the domain. You will also see the equations specified. (These were implemented in TexGen some time ago and therefore do not follow Li's equations ). You should change the equations here if you want to change the boundary conditions.

You can specify mesh refinement in TexGen by using the SetResolution functions described here: http://texgen.sourceforge.net/api/class ... _yarn.html If you want a preview of the mesh generated by the dry fibre export use the Rendering->Render Textile Volume option.

If you want to change the contacts or friction for the plates you'll need to edit the .inp file.

I'm afraid I don't know anything about the penalty contact algorithm. You'll have to look at the Abaqus manual on that one.

Louise