Unexpected simulation results for a flat S-shape structure deformation

[carleene]

Hello!

I have a relatively simple engineering case that I hope you can help me with. I am trying to simulate the behavior of a flat "S shape" structure under deformation (50% strain). What I am expecting from designing such "S shape" structure is a release of strain by unfolding on the Z axis/normal plane, similar to this:

https://www.researchgate.net/figure...serpentine-bridge-designs-A-SEM_fig5_23479781

We made a little experiment using a thin 0.1mm Kapton tape to confirm this.

The results I am obtaining, however, do not match with the experimental results. The structure does not unfold on the Z axis (see results of U3 displacement below) and therefore there is a high concentration of stresses and strains (see results of S mises and E below).

I modeled this structure as a 3D deformable part with a shell section 0.1mm thick (overall structure is 16mm long), but it seems it is doing the simulation as if it was a 2D planar part. For the boundary conditions, the very left edge has the X displacement and Y=Z=0, and the right edge has X=Y=Z=0. I tried to change these boundary conditions slightly but results were the same.

I hope you can give me a little helping hand to solve the mistery. Thank you very much for your help, and happy holidays!

C.


----

- CAE file:

https://files.engineering.com/getfi...7-357b-437c-acf6-3a407f168abc&file=Sshape.cae

- Undeformed shape:

https://files.engineering.com/getfi...88-a806-75ed0eb30a9d&file=Sshape_undeform.png

- Von Mises:

https://files.engineering.com/getfi...4ef9-be9c-5f08b63fbc6f&file=Sshape_Smises.png

- Strain:

https://files.engineering.com/getfi...0-4838-85a2-b915fb7d71e2&file=Sshape_Emax.png

- Z displacement:

https://files.engineering.com/getfi...db9-4a55-9dc1-500eb5ddd391&file=Sshape_U3.png

 

[FEA way]

I can't open your CAE file now so I have to ask - is NLGEOM turned on in this analysis ? What you want to achieve is a form of buckling so geometric nonlinearity will be necessary to capture such effect.

 

[carleene]

Thank you so much for your prompt reply! Nlgeom was not turned on, but I tried again turning it on (under "Steps" section), unfortunately with very similar results (actually slightly worse, 107MPa instead of 105MPa of maximum stress).

PS: I have the 2017 version, maybe that's why .CAE can't open. You can find the .inp file here in case that works

https://files.engineering.com/getfi...110-4381-a708-43869da41bb6&file=Sshape50p.inp

 

[FEA way]

For next tests I would leave NLGEOM turned on since most likely it is necessary to achieve such effect. Try lowering Young's modulus and shell thickness. I would also consider modifying the geometry and increasing strain level. At some point this out-of-plane deformation may become visible.

It's not that your CAE file doesn't work. I just don't have access to Abaqus today. But thanks for uploading .inp file. I will take a closer look and perform some tests myself later on.

 

[carleene]

I tried lowering the shell thickness, changing the young's modulus and increasing the strain level but there is still no out-of-plane deformation.

It seems there is something else missing in the simulation parameters. Thanks for your support so far, I appreciate it a lot

 

[FEA way]

You can also try performing linear buckling analysis and then using eigenmodes as imperfections for actual stress analysis (with NLGEOM on). This is very common approach and I see that the same was done by the authors of this article. There’s a very high chance that it will work and you will get the expected results.

Also I’ve found another research paper on this topic that might be interesting for you: "Design of metal interconnects for stretchable electronic circuits" by M. Gonzalez et al.

 

[carleene]

That's wonderful! Many times researchers don't share their simulation parameters, it's great to see they did.

I think we are getting closer from getting some interesting results. I am following the manual about how to introduce imperfections:

http://dsk.ippt.pan.pl/docs/abaqus/v6.13/books/usb/default.htm?startat=pt03ch06s02at03.html

I did the following:
1) I made a Buckling analysis. From the output, eigenmode #7 seems the closest to the desired solution
2) I supressed the Buckling step and then created a Static Riks analysis with the same boundary conditions as my previous Static General analysis. I run the analysis to check it computed a similar solution.
3) I then introduced the imperfection of eigenmode#7 from the buckling analysis job I called "buckling" by inserting the following lines on a specific location on the Edit Keywords model section (as indicated by the tutorial):

https://files.engineering.com/getfi...4257-bcf5-b87963813982&file=tuto_buckling.PNG

Unfortunately, after submitting the file the following error appears: Abaqus Error: The following results file(s) could not be located: buckling.fil

Interestingly, I can't find this .fil file anywhere on my PC... I've spent a few hours doing this and it's quite frustrating so I will take a break for now. Feel free to play around with the .cae file here:

https://files.engineering.com/getfi...-48c2-a46a-ecda4854a0b6&file=Sshape_riks3.cae

You can first run the buckling job so that it generates all the buckling output files. Then, supress the buckling step & resume the riks step, introduce the imperfection as shown above, and submit the riks job. Let me know if you try it out and it works for you or if you find any error or alternative ways to do it!

 

[FEA way]

Before introducing imperfections to static (or static Riks) you have to write them to results file generated during eigenvalue buckling analysis. For this purpose use the following keyword in this first analysis:

*Node File
U

This will write displacements from buckling modes to .fil file so that they can be used by *Imperfection keyword.

Another thing to try is prestrain. Notice that it was also done by the authors of the article. But first give a chance to imperfection approach.

 

[carleene]

I tried again with your advice and entered the *Node File keyword in the buckling analysis after *Output requests. The riks simulation WORKED! I introduced the imperfections from buckling mode 7 and stretching the system 50%. I could compare it to the results from introducing no imperfections, you can find the screenshots here:

https://files.engineering.com/getfi...8-e1103fce5d6b&file=Mode7_buckle50%strain.PNG

https://files.engineering.com/getfi...90bd-06db672473bb&file=Nobuckle_50%strain.PNG

However, you can see in the outcome the stresses are only alleviated by 7.6% because of the buckling (99.2 vs 107.4 MPa), which is far from the results in literature.

Moreover, the computation is very sensitive to the increments set on the Steps. For example, I fixed the maximum number increments to 50 and arc length increment to 0.02 and it worked well for 50% stretch/displacement (If I left it on automatic the stretch goes far beyond the 50% displacement I introduced, until 400% or so until computation aborts). When trying 100% of total stretch, the computation computed only to 14%, so I decided to add more increments (500 and 0.002 arc length) but then the computation started to add *Conflicts and aborting immediately.

Seems we are making a bit of progress! Thank you so much for your advice so far, you've been super helpful

 

[FEA way]

If you want to stop the Riks analysis before it goes too far with increasing displacements, use stopping criteria options available in Basic tab and leave automatic incrementation instead of fixed one. Stopping criteria options allow you to specify maximum load proportionality factor or maximum displacement for selected nodes. When the criterion is reached the analysis will stop.