Stress level too high

FOL

Dear all,

I have simulated with Mecway several metal sheet parts and the obtained stress levels are x100 times higher than expected. I have tested several elements (surface and volume) and several analysis types but the stress level are still that high.
The steel material is defined with a Young Modulus of 210GPa (Poisson’s ratio of 0.29, density of 7.85kg/cm3). The ambition is to check 1st. that we do not have plastic deformation and 2nd. to find out the needed force to produce a certain elastic deformation.

Any idea about where is the error will be very welcome. I enclose an easy model as an example. Thanks.

Thanks.

David

[Deleted User]

should the units on density be g/cm^3?

FOL

Yes, you are right. It's a typographic error. Density considered= 7.85 g/cm3

Victor

Was this originally a .liml file or .inp? If .inp, then I agree with prop_design that units don't look consistent. If it was .liml, then kg/cm^3 is OK. [EDIT: Except 8kg/cm^3 is much too high for steel - now I see that's perhaps what you meant prop_design.]

If .liml, please upload the original since this file seems to have too many different constraints for Mecway to open. I solved it with CCX and it shows peak stress about 220 GPa at the middle of the wavey parts, which sounds like it's consistent with your 100x something reasonable.

From that solution, I think the displacements are too high for a linear analysis and you should change the analysis type to nonlinear (or NLGEOM=YES in .inp). As a rule of thumb, if the deformed view with an amplification factor of 1 is visibly differently shaped from the undeformed view then it may need nonlinear analysis.

FOL

Thanks Victor. Please find enclosed the original document (*.liml).

I will try with non linear analysis.

Victor

Mecway's own solver can't do non-linear analysis on this because it has non-zero displacements. Instead, I solved it with CCX and the solution is very different from the linear solution, so you definitely need to use a non-linear analysis.

The stresses are a lot lower than with linear analysis, but not 100 times lower. The peak stress is still about the same but it occurs at a stress concentration at the end of the boundary condition so you should ignore that because it's an artifact of the idealized perfectly rigid boundary condition.

With just one time step and constant displacements, CCX didn't converge, so I changed it to 10 time steps and ramped the displacements up from 0 to 4mm.

I also deleted many of the low-stress parts just to speed things up.

FOL

Thanks Victor. I use CCX for the non-linear analysis and, as you said, the stresses decreased significantly. Sorry for the following basic question, but I am not familiar with the "boundary" command. What is exactly constrained with 1,1,1 or 2,2,1?. Thanks.

Victor

The *BOUNDARY keyword defines fixed displacements.

Here "xface,2,2,1" means constrain the nodes in xface so that dof 2 (y-displacement) has the value 1 m multiplied by the amplitude. The amplitude ramps up linearly from 0 m at time 0 to 0.004 at time 1 s.

See the CCX or Abaqus manuals for more information.

FOL

Thanks.