displacement driven torsion boudry for an cylinder

[cji]

Hello,

I use the FEAP Version 8.6 and I want to simulate a displacement driven torsion test for an cylinder (r=0.3, h=20). The longtinual axis (symmetry axis) of the cylinder is the x-axis. At one buttom of the cylinder (x=0) the surface is fixed and the other buttom of the cyliner (x=20) should be spinned around the x axis propotionally to the timestep.

I want to use the SPIN command in the following way:

EBOU
  1 0 1 1 1
  1 20 1 0 0

SPIN
  CENTer 20 0 0
  NORMal 1 0 0
  RATE 1
EDIS
  1 20 0 1 1

Afterwards I want to use the following code to define the displacement, where the spin.txt concludes the spin angle per timestep:
BATC
  prop,,1
END
2,2
incl,spin.txt

However, the code does not work and I could not figure it out where the problems are.

I would be happy to get a response! Tank you!

[Prof. R.L. Taylor]

Please post your input file so we can help

[Prof. R.L. Taylor]

You ALWAYS should check your output file to make sure all the input commands were used.  You are missing a blank between the spin and edis above.

[cji]

Hello professor,

thank you for your quick response!

Here is my input file, my mesh and also the spin.txt as the spin angle per timestep in the uploaded zip-file.

The outpufile states "*WARNING* Zero right-hand-side vector" and I could not figure out what causes the problem.

Thank you very much for your help!

Best regards

[Prof. S. Govindjee]

(1) Your BCs are a bit odd.  What what problem do you want to solve?  Do just want to twist one end of the rod relative to the other?

(2) You are missing the END command for the end of the mesh.

(3) Your PROP command appeared twice.

(4) For the second PROP command you want 2,1 not 2,2;  2=table input, 1=one pair per line in the table

[Prof. R.L. Taylor]

There are lots of problems -- you should start with a small problem to learn how to use any program.  Also never, never try to do the whole analysis -- only one step.

You need finite deformation, you cannot use nu = 0.5 with any element except full incompressible (with lagrange multipliers).

I attach a working input file

[cji]

Thank you very much!

I have noticed that the loaded part of the beam increses its cross section. For my problem, I just want to twist the end without changing the cross section.

Is there then another BC to set?

[Prof. R.L. Taylor]

The rotation b.c. Should not change area.  How are you computing differences?  Do you have a small problem that we can see this?

[cji]

I used the input file that you uploaded and in the results of the simulation the cross section increases. So the BCs in the file is then as you coded:

EBOU
  1 0 1 1 1
  1 20 0 1 1

LOAD PROP 1
  SPIN
    CENTer 20 0 0
    NORMal 1 0 0
    RATE 1

  EDIS
   1  20 1 1 1

LOAD END

I suppose it is the command EDIS 1 20 1 1 1 that causes the increase of the radius. I also tried to use EDIS 1 20 1 but the radius still increases.

[Prof. R.L. Taylor]

are you sure all your material models are finite strain?  the EDIS does nothing I hope.

using a small strain element in finite rotation will produce an apparent dilation.

[cji]

Yes the materials should be finite strain, they work for large strain in tension and compression

[Prof. R.L. Taylor]

What element do you use?  Do you set FINIte for the material data?   

I ran your mesh with a lot of rotation and it does not dilate.

If you are using the FEAP large deformation  elements then you should get the same type of result.  If you are using your own modules they may need to be checked.

There is a difference between "large strain" and "finite deformation".

[cji]

Sorry, I just found out that the radius just increases because auf the scaling in paraview. The code works perfect. Thank you again for you help!