Problem with explicit fem with solid-structure interaction in ABAQUS 2

[Arturogdc90]

Hi all,

This is my first post, so please don't red flag me if I am doing anything bad. I hope I can contribute to the forum in the future with the knowledge I have (mainly abaqus explicit).

My problem right now is with a simulation of a tank truck, I am trying to replicate an experiment and see if numbers match between FEM and real world. I am using volume fraction tool to situate a 50% of the volume of the tank as water, the tank mesh was created using Hypermesh.

When I start the simulation it happens that big bubbles appears in some contact points between the water and the structure. I have uploaded to images of two simulations (one using 50% fill volumen starting still and another using just a big box of water that falls in the tank). I have tried with simpler cases before and they were really good, but maybe due to the increased surface covered now I am facing this problem.

Water Box:

https://www.dropbox.com/s/vtx8nakqaow89e9/Ingtips1Box.PNG

https://www.dropbox.com/s/j7zq5lesasokfuc/Ingtips2Box.PNG

https://www.dropbox.com/s/5dglzf1kmiqrvn9/Ingtips3Box.PNG

50% Fill Volume:

https://www.dropbox.com/s/0vun6m4yxa6ae2q/Ingtips3_50pc.PNG

https://www.dropbox.com/s/z4crh72au8rj14n/Ingtips1_50pc.PNG

https://www.dropbox.com/s/4352ytpejc7nf8c/Ingtips2_50pc.PNG

Tank structure:

https://www.dropbox.com/s/alny5mrfz9alpjh/TankStructure.PNG

I can upload the odb file if you think that it would be helpful.

Big thanks, hope someone can bring some light into this I have been stuck with this since some time ago.

 

[burningDiesel]

You are doing CEL modeling, correct?
In case you haven't, you should 'overlap' the eularian domain somewhat with the lagrangian (at least 1 element), then use the volume fraction tool.
What are your boundary conditions?

 

[Arturogdc90]

Yes, I am doing CEL method.

About the eulerian overlapping the lagrangian I think it is done that way. In the next image you can see how I did it:

https://www.dropbox.com/s/n7hz0i0hlik8is5/Eulerian_Lagrangian.PNG

I know that possibly this can be done in a better way (computation wise) but I wanted to try first.

For the BC I used U1=U2=U3=0 in 32 points of the tank mesh, 16 at each side. The final simulation should be moving following a senoidal.
BCs:

https://www.dropbox.com/s/9ijuvlg1g0e2ojp/BCs.PNG

Thanks a lot for the reply!

 

[burningDiesel]

I think you should just make your eularian domain +1 element bigger, the way it is now, "void" can leak through the edges, creating the problem you have.

 

[Arturogdc90]

Thanks for the reply again. I tried what you said, and still no good results that weird behaviour still happens.I think the next step will be to try with at least 3 elements wide in the structure, just to see if it is related with any fluid (or void) leaking in or out. I do not have a big machine with me so the simulations are pretty lengthy.

Here is the new eulerian-structure assembly:

https://www.dropbox.com/s/dv2eqz5rdifo45f/More_eulerian2.PNG

And the beginning of the behaviour:

https://www.dropbox.com/s/o7113x8tjqwvpvq/More_eulerian.PNG

I also have the .odb in case someone want to see it, to see the fluid Tools->view cut-> Manager -> Mark EVF_VOID and check only the second mark of it (unmark the first).

https://www.dropbox.com/s/9qnq20mjbhq9zh2/SinMov_50pc_maseuleriano.odb

Thanks a lot, all information is really welcomed. This is the first problem in all this time that I do not know why is happening to me or what could be the cause.

 

[burningDiesel]

I can only check your .odb on monday when I'm back at work (with abaqus).
From the pictures I can't tell what would be wrong, I assume your units are consistent and no warnings are given?

 

[Arturogdc90]

I have checked the units many times, they are in N/mm and I think they are Ok, although you never know. But I tried simpler things before (less fluid) and worked flawlessly. The only warning given is related to some thermal properties of the water material.

I can send you the .cae file if you think that would help.

Really really thankful to you for trying to help with this.

Hope you can see something in the odb file.

 

[burningDiesel]

I think your error is in the volume fraction tool. It only assigned 100% water inside the solid elements, and 0% where you actually want it. If you upload your .cae or .inp I could tell for sure.
Probably you need to make a "helppart" with solid elements filling your tank.

 

[burningDiesel]

Nevermind it does seem to be OK i visualized it wrong.

 

[Arturogdc90]

Yeah, I think the volume fraction is ok, but I have uploaded the .cae anyway so you can check it. Here it is:

https://www.dropbox.com/s/4vyou5p470doexi/cisterna_sinvimiento_50pc_maseuleriano.cae

I will delete it tomorrow.

Thanks again, this one is tricky.

 

[burningDiesel]

You forgot to put "rough" friction between wall and water

 

[burningDiesel]

Here's the result (I reversed the gravity direction because else its just a tank with still standing water - yawn)

 

[Arturogdc90]

Sorry I have not answered before, BIG BIG BIG thanks! This is absolutely awesome.

Although I still have to ask some things:

1. How you create this kind of rough friction? I have to add it apart from the All with self?

2. Did you do anything special to calculate so fast? Or just a powerhorse at work? I need like 1h for each 0.1s

3. How you visualize it? Hyperview? I can't get that transparency of the lagragian element.

Sorry for making you lose your time, if you need anything just ask. You saved me. Thanks again.

 

[burningDiesel]

1. in the contact properties or something "tangential contact" -> rough
2. I scaled back the steel E-modulus 10x, increased the steel density x 100 and increased the compressibility of water x 10, all of which increased the stable time increment, it ran in 10 minutes or something on my laptop. As the tank is static, increasing the steel density is no problem, and you can check the density of the water in postprocessing and decide if the error is acceptable (for making a picture, all errors are acceptable )
3. plot overlays, water is not transparent, lagrangian is, I also messed with the overlay "depth" to get a better movie

Rough friction means a "no slip" condition, which is also physically correct (speed of fluid movement at the wall is zero).

 

[Arturogdc90]

Thanks again!

1. Found it!
2. I tried this but the calculation is still the same 4 min -> 0.01s, after changing the material properties did you change anything else? In the step definition or something like that?
3. Found it!

 

[Arturogdc90]

Still the problem of the thread happenig, I am doing something wrong. Could you send me the .cae that you modified to check both things?

Thanks a lot.

 

[burningDiesel]

you can output the stable time increment (EDT), this should increase when a) you make a material softer (or for eularian, more compressible: EOS parameter) b) you make it heavier.
i ll upload the .cae tomorrow

 

[Arturogdc90]

I have tried again and it does not make any change in the estable time increment, I do not know what to think. I am doing something wrong or I have something wrong with the file or the software. Have you been able to get the .cae file?

No rushing or something like that, you have helped me a lot. Sometimes my english is still a bit rough.

Thanks again.

 

[burningDiesel]

see attachment

 

[Arturogdc90]

Wow thanks! Now is working perfectly, but I have checked the interaction properties of the file you sent me and I can't see the rough friction between water:

https://www.dropbox.com/s/2xr5dqqjnr7e897/no_rough.PNG

Did you change it in a different place?