Modelling of unit cell of woven composite in ABAQUS

anuragdixitiitd · Post by **anuragdixitiitd** » Fri Mar 02, 2012 6:18 pm

Hi everybody,
I am interested in Meso Level modelling of unit cell of woven fabric composite (especially 2x2 twill weave) in ABAQUS in order to determine the fundamental mechanical properties of woven composite laminate from its individual constituent properties (fibre+matrix). Now once when the unit cell has been identified and built up in TEXGEN further analysis is required in ABAQUS or any other FEM software for identification of mechanical properties. I am not clear about analysis aspect of unit cell in ABAQUS and would further like to request you all to kindly provide me any solved example problem or any useful study material or any useful link if possible, pertaining to analysis of any weave architecture in ABAQUS.
Solved example problem will be highly appreciated.
Regards
Anurag

Post by **louisepb** » Mon Mar 05, 2012 9:30 am

Hi Anurag,

The easiest way for you to use Abaqus to obtain mechanical properties would probably be to use the Abaqus Voxel Mesh export as described here http://texgen.sourceforge.net/index.php ... BAQUS_File. This gives a .inp file which provides a set of boundary conditions as described in the paper by S Li (given in the previous link). If you read the paper this will explain how the mechanical properties are then calculated from the Abaqus output.

There is further discussion on this in the following thread: http://texgen.sourceforge.net/phpBB3/vi ... ?f=1&t=698

I hope that helps,

Louise

anuragdixitiitd · Post by **anuragdixitiitd** » Mon Mar 05, 2012 5:21 pm

Hello Sir,
Many Thanks for the reply. Will get back to you soon after implementing it.
Thanks & Regards
Anurag

anuragdixitiitd · Post by **anuragdixitiitd** » Sat Apr 28, 2012 4:13 pm

Hello louise,
Hope u will be fine! I find TexGen very easy and useful for modelling. As per your tips I modelled the unit cell of twill fabric composite in texgen and export the .t3g file to ABAQUS voxel mesh option with relatively low voxels in z directions. Everything was going well as I successfully imported the model in ABAQUS /CAE 6.10.1 but with certain warnings :
(1) TEXGENORIENTATIONVECTORS used as the orientation no longer exists or no longer valid for defining the orientation
(2) unknown assembly level node set 'constraint driver 0',1,2 &3
While running the job orientation problem occured regarding orientation saying that input file was not generated and the job was not submitted for analysis.

Now I want to know that while modelling in texgen I haven't given any boundary conditions nor step nor orientations nor constraints nor load so how it is happening automatically or as per paper by S.Li. ?
and when I verified all the commands in the model tree in ABAQUS I was little confused with B'Cs, load and constraints. Kindly help me in understanding what commands texgen is following while creating .inp file. Can i reduce these errors by running .inp from command line?

I tried to find my answers in the thread http://texgen.sourceforge.net/phpBB3/vi ... t=487#p725 but still not clear with whats going on!!
Sorry for too many questions at a time.
Thanks and Regards
Anurag

Post by **louisepb** » Tue May 08, 2012 10:58 am

Hi Anurag,

When you create a model and then export it as an Abaqus voxel file TexGen creates a .inp file which contains the boundary conditions and steps which implement the theory described in S Li's paper. This is discussed in some detail in this thread: http://texgen.sourceforge.net/phpBB3/vi ... ?f=1&t=698

You cannot run this file from Abaqus CAE. CAE cannot cope with the equations which match multiple node sets and also will not import the .ori file.

I hope this helps,

Louise

anuragdixitiitd · Post by **anuragdixitiitd** » Wed May 09, 2012 10:37 am

hi louise,
Thanks for the reply!! i tried many times to run the .inp file created by texgen for evaluation of material properties, as directly importing in ABAQUS CAE results in missing of some equations and orientations problem. I also tried to find this answer in the discussion http://texgen.sourceforge.net/phpBB3/vi ... ?f=1&t=487 but finally I was confused with so many comments. I read the paper "Unit cells for micromechanical analyses of particle-refined composites", Shuguang Li, Anchana Wongsto, Mechanics of Materials 36(2004) 543-572. and found section 4 to be concerned of dealing boundary conditions and section 8 with load cases and found the .inp file accordingly. Please give me some hint to how to cope up from this ABAQUS imorting issue.
Best Regards
Anurag

Post by **louisepb** » Wed May 09, 2012 12:49 pm

Hi Anurag,

I'm unclear as to what you've actually done. Could you be specific please? Have you run the .inp from the Abaqus command line? Did you get errors? If so, what were they?

Louise

anuragdixitiitd · Post by **anuragdixitiitd** » Fri May 11, 2012 6:28 am

Hi Louise,
I apologize for the inconvenience from my side. Now i will clearly tell you that what I have done & what actually my problem is.
I have generated a single layer fabric unit cell of 2x2 twill composite with each 4 weft and warp yarns with default settings in TexGen. Then I succesfully exported the above unit cell with Abaqus Voxel file with following options (x count =50, y count=50 and z count =30, with periodic boundary conditions as material continum and element type as c3d8r and both output yarn and matrix) for 3D elastic properties computational. After that I managed to run my .inp file from command line in ABAQUS and obtained various file including .dat and odb. There are 2 warnings showing in .dat which are.

1. WARNING: MPCS (EXTERNAL or INTERNAL, including those generated from rigid
body definitions), KINEMATIC COUPLINGS, AND/OR EQUATIONS WILL
ACTIVATE ADDITIONAL DEGREES OF FREEDOM

2. ***WARNING: IN A STATIC PERTURBATION STEP USER SUPPLIED DATA CARD IS IGNORED.
ONLY ONE INCREMENT OF ANALYSIS IS POSSIBLE. THE TIME INCREMENT AND
THE TIME PERIOD ARE SET TO A SMALL NUMBER.
After looking .inp and .dat file I was little confused with boundary conditions!!

Now my questions are as :
1.What are these warnings?
2.Currently to what BC's and load my unit cell is subjected to?
3.Whether TexGen is always following the simple cubic packing boundary conditions as specified by Eq. 12, 13, 14 in S.Li paper irrespective of weave pattern? and whether it including or excluding Traction boundary condition's as in Eq. 15?
4. How should I look for my results (3D Elastic properties) in ABAQUS?
and Lastly
5. What changes should I do in boundary condition and load cases to run simple tension and compression test on a unit cell?
Sorry for too many questions!!!
Best Regards
Anurag

Post by **louisepb** » Mon May 14, 2012 9:07 am

Hi Anurag,

I'll try to answer your questions in order:

1. I'm afraid that I'm not actually much of an Abaqus user myself. You'll have to consult the Abaqus user manual to find out the cause of these warnings.
2. The boundary and load conditions are as specified in S Li's paper.
3. Yes, TexGen follows the simple cubic packing equations and, as described in the paper the traction equations are excluded.
4. Use of the equations is described in section 8 of the paper. In TexGen the force applied is equal to the volume, therefore giving a unit stress and the Young's modulus is simply 1/strain. The process is shown in the tutorial posted recently here: http://texgen.sourceforge.net/workshop/ ... alysis.pdf
5. Any other conditions you will need to decide yourself what you want to do.

Louise

anuragdixitiitd · Post by **anuragdixitiitd** » Tue May 15, 2012 4:21 am

Thank you very much for the answers Louise !!!
Will get back to you with some positive results
Best Regards
Anurag

anuragdixitiitd · Post by **anuragdixitiitd** » Fri May 18, 2012 10:34 am

Hello Louise,
Many thanks to you for making me understand and run the analysis! As far as I understood in my case there are 6 load cases (acting in 1 direction) each of them are applied separately to the ConstraintDriver nodes 0,1,2,3,4,5 and the output will give the modulli (Ex, Ey, Ez, Gxy, Gxz and Gyz) corresponding to each load case. Am I right??
The output is obtained in .rpt file in the form of displacement (6 outputs for each constraintdriven nodes i.e. total of 36) which correspond to the strain's and now by the use of Eq. 32 we can calculate all the modulli for each constraint driven nodes.Am i right up to this point?? If not then please correct me...
Now if I am right my question is how to obtain the Total or final or effective modulli (six or nine significant values) for whole unit cell and after that for whole composite laminate from the available output. I mean how to make use of these available elastic constants (36 nos.) for there overall final values ??
I hope u understand my question!!!!
Best Regards
Anurag

Post by **louisepb** » Thu May 24, 2012 9:03 am

Hi Anurag,

If I understand what you're saying then I think that you are nearly right! The output from the constraint driver nodes will give you the values for the whole unit cell. eg. For constraint driver 0 Ex = 1/strain in x and vxy = strain in y/strain in x. For constraint driver 1 Ey = 1/strain in y and vyx = strain in x/strain in y and so on.

Louise

anuragdixitiitd · Post by **anuragdixitiitd** » Wed May 30, 2012 6:00 am

Hi Louise,
Thank you for the answers and sorry for the delay in replying!
After much exercise once again I lost in extracting the output from the .rpt file.I am getting 6 values of displacements for each single constraint driver node.As displacements act similarly as strains in every axes, how could I achieve a significant value of Ux, Uy and Uz for each node from the available 6 displacement value of my computational. I hope I have problem in understanding (reading) the output (.rpt) I am attaching the .rpt file for your reference. In my odb field output request I have opted for (U1,U2,U3) for constraint driver 0,1,2,3,4,5. The displacement U2 and U3 for all nodes are zero.

Best Regards
Anurag

Post by **louisepb** » Wed May 30, 2012 9:54 am

Hi Anurag,

In the .inp file the constraints drivers are assigned as follows: 0 = x, 1 = y, 2 = z, 3 = xy, 4 = xz, 5 = yz.

To extract your mechanical properties therefore:

For line 1 (ConstraintsDriver0, x): Ex = 1/column1 (strain in x)
Vxy = column2/column1 (strain in y/strain in x)

For line 2 (ConstraintsDriver1, y): Ey = 1/column2 (strain in y)
Vyx = column1/colum2 (strain in x/strain in y)

and so on, as per equations 31 and 32 in Li's paper.

Hope that helps,

Louise

anuragdixitiitd · Post by **anuragdixitiitd** » Fri Jun 01, 2012 4:20 am

Many Thanks ...

TexGen