Modelling of unit cell of woven composite in ABAQUS

[anuragdixitiitd]

Hi Louise,
I have gone through the link provided by you for mesh refinement (Yarn set resolution function). As far as I understood is by setting the number of slave nodes will alter the resolution along the length of the yarn and setting the number of section points will alter the number of points around the circumference of the yarn, and hence the number of elements across the cross-section. Am I right??
I juggled a lot to implement the above in my simulation, but didn't succeeded
Now my question is that how these changes (number of section points) will be implemented in my simulation?
Whether I should edit my python script or .inp file its not clear. I tried a lot to implement the codes but it shows error again & again.
I am actually not able to make changes in my script. Please provide me any benchmark problem or any example file if possible.
Or is there any other way or option to change the number of section point.
I hope you understand my problem.
Best Regards
Anurag

[louisepb]

Hi Anurag,

You will need to change your script to call the SetResolution function as here: http://texgen.sourceforge.net/index.php ... ate_Models ( in this case it only sets the number of section points but you can set number of slave nodes as well by sending two parameters).

Alternatively you can edit the .tg3 file of your saved textile. For each yarn you will see "NumSectionPoints" and "NumSlaveNodes". Just change these values and that will change the resolution when you reload the file.

Louise

[anuragdixitiitd]

Hi Louise,
Sorry to disturb you !! While editing my .tg3 file after selecting a particular yarn I nowhere found the option to fill the "NumSectionPoints" and "NumSlaveNodes". I searched in TexGen. Can u please tell me where it is?
In order to change the element used during analysis should i change it from .inp file?
Best Regards
Anurag

[louisepb]

Hi Anurag,

I think I didn't explain myself properly. What I meant was for you to open the .tg3 file in a text editor. It is basically an XML file saved with a .tg3 extension. In the yarn sections you should find NumSectionPoints and NumSlaveNodes. Just change the values in the text file, save it and then load it again into TexGen.

I'm not sure what you mean by "change the element used during analysis"?

Louise

[anuragdixitiitd]

Hello Louise,
I tried to run my .inp file after refining the mesh both along length and cross section but still I am getting error again and again and finally the analysis terminates.
The warning that occurs are:
1. ***WARNING: Master surface YARN3UPPER of contact pair # 4 contains facets with
out-of-plane warping of at least 20.000 degrees in increment 780.
Large warping that develops during an analysis often corresponds
to severe distortion of the underlying elements. It may be
appropriate to rerun the analysis with a refined mesh.
(This occurred after refinement of mesh; (150,150))
Whether it requires further refinement??? But it will increase the computational time. This message occurred for all 4 contact pairs.

2.***WARNING: In contact pair 4, node 80700 on the slave surface YARN3UPPER has
35.914 times more mass than the mass of node 120 on the master
surface YARN0LOWER. Significant contact noise may result with the
kinematic contact algorithm when the slave nodes have
significantly greater mass than the master nodes. Suggested
workarounds include setting the WEIGHT parameter so that surface
YARN0LOWER is a pure slave surface in the contact pair, using
mass-scaling to adjust the ratio of nodal masses, or using the
penalty contact algorithm.
I referred ABAQUS manual to resolve the above issue by implementing penalty contact algorithm to my analysis, but not able to execute it due to improper syntax addition in .inp file. This message also occurred for all 4 contact pairs.
3.***WARNING: For contact pairs that are not tied, unresolved initial
overclosures will result in initial accelerations on the order of
the penetration distance divided by the time increment squared,
which can lead to significant mesh distortion. These overclosures
can be avoided by user adjustment of the mesh.

Finally the analysis terminates in between. Can u please refer me any solution to the above problems/warning.
Sincerely Yours
Anurag

[louisepb]

Hi Anurag,

I need to talk to one of my colleagues, neither of whom are in the office today, about this. It sounds like you may have a problem with intersections in your mesh, particularly the 3rd warning, but I will need to confirm this. Try using the Render Interference options to see if there are intersections in your textile. If so try using the Adjust Intersections option in the Dry Fibre export. If intersections turn out to be the issue and adjusting intersections doesn't solve the problem then you will need to adjust your model to solve the problem.

I'll get back to you further when I've had a chance to ask someone about this.

Louise

[louisepb]

Hi Anurag,

Yes, it sounds like a problem with intersections. Changing the geometry to account for these will probably be your best course of action.

Louise

[anuragdixitiitd]

Hi Louise,
Thanks for your quick reply. Actually there were 12 intersection found between the yarn in the textile, though I tried to export using adjust intersection tolerance (0.0000001) but that also didn't worked. What do you actually mean by changing the geometry of the model (Does it means i should go for 2X2 fabric instead of 1X1 or should i edit my initial create 2D weave data i.e. yarn width, yarn spacing, fabric thickness, gap size etc. or is there any other way of adjustment of mesh). I have also further refined the mesh to avoid Warning 1 but the result is same (i.e. asking for more refinement). Further refinement will result in increase computational time......
What I think is that I am not able to provide adequate contact definition to my analysis (i.e contact between (yarn and yarn) and (plate and yarn))!!!! Because when I am visualizing my results with terminated analysis (.odb file) I can see that during compression the front surface of the yarns are coming out of the plate.

Best Regards
Anurag

[louisepb]

Hi Anurag,

The Adjust Intersections will only remove small intersections less than one element of the volume mesh deep. There is therefore a trade off: refining the mesh will mean that size of intersection that the adjust intersections removes will be smaller. To change your model you will need to manually adjust the yarns. Either move the nodes or change the cross-sections. You may also need to add extra nodes so that you can change the yarn path. Did you use the refine option when you generated the textile? This normally does a pretty good job of removing intersections. Ideally look at images of your actual textile so that you can see what is happening at these points to give you a good idea of what your model should look like.

Louise

[anuragdixitiitd]

Hi Louise,
Defining the minimum gap size between the two yarns really worked and the third warning regarding removing intersections is now completely eleminated. But still the analysis was not completed saying that there are a total of 6 excessively distorted elements and The ratio of deformation speed to wave speed exceeds 1.0000 in at least one element. This usually indicates an error with the model definition. How to tackle with these excessively distorted elements??
Best Regards
Anurag

[louisepb]

Hi Anurag,

The most likely thing is that you still have some intersections in your model. You will need to look at your Abaqus output file to find the exact location of the problem elements and then go back and look at your model to the problem areas. The render intersections in TexGen checks for intersections at the nodes but will not necessarily pick up intersections between. You will probably need to make small adjustments to your model (maybe to the yarn path or cross-sections) to remove these.

Louise

[anuragdixitiitd]

Hi Louise,
Finally I ran my analysis by making some changes in my model as directed by you. Many Thanks....
Now when I visualized the results in ABAQUS I see that:
1.The top plate is compressing the unit cell but the deformed shape appears to be largely in blue color rather than mixture of colours (red, green, yellow etc)?Why is it so?
2. Should I change the material property of plate (density, E,nu) or let it be default?
3. How I will be able to view the complete deformed surface of unit cell as it is hidden by the plate? How I should visualize my results?
4. In one of thread you discussed about Scale x,y,Z in dry fiber+compression plate export.I further wanna clarify if I want to achieve 50% compression in Z direction I should enter 0 in Scale X and Y while 0.50 in scale Z. Am I right?
5.While modelling in Tex Gen i am providing all the 9 material properties to the yarn(E1,E2,E3,G.....,nu.......) but in my .inp file I am only getting E1 and nu12 in elastic properties?

Many Thanks
Regards
Anurag

[louisepb]

Hi Anurag,

I'm afraid that I can't really help you with questions 1-3. You need to find someone who is knowledgeable about analyzing ABAQUS output to help you with that.

4. Yes, put in 0.5 in the z direction if you want to achieve 50% compression.
5. Only the voxel mesh .inp file currently uses all 9 material properties. If you want to use all the properties for the dry fibre analysis you will need to edit the .inp file yourself and then write your own UMAT subroutine in order to use them.

Best regards,
Louise

[louisepb]

This topic was diverting from the original topic so has been split to form Meshing textile for dry fibre analysis thread

[dyeyanie]

Hi Louise,

I'm interested to know detail on dry fibre options. In your other thread, you did mentioned about creating geometry without matrix, where there are 2 options; a) exporting them using Dry fiber or b) voxel mesh without matrix. However, in Dry fiber options, I need to state the compression percentage that I would like to achieve. Let say, I created a design in voxel mesh options, how could I get the same design as in voxel with dry fiber options? I mean in terms of the loading condition. I intend to put in the friction info in my geometry in which I did created a geometry with voxel mesh options previously. Since you mentioned the only way to modify the friction is with Dry fibre option so I'm aware about the implementation of load in both cases.

Yanie