Same Stress values for different Materials????

[sbhushankumar]

Hello everyone,

I created an assembly with three different parts. I first ran an analysis by assigning al2014.mtl to all my parts and then by assinging fenodr.mtll . What I found out that the vm stress values for both the analysis are same(almost) i.e 2.255e+02 and 2.264e+02. Howevere, there is big diference in other values like displacement, strain energy etc(which is OK as the assigned materials are different in both the cases). How is this possible that stress values(von mises) are approximately same.I have added a snapshot showing the study status of both the analysis.Does it anything have to do with the warning mesage that is displayed at the bottom ??

Thank you,

Shashi.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[sdensberger]

I see no issue that the stress values are near identical. Think back to the definitions of stress, (normal, shear, and bending); no where in them do you define the Young's Modulus or Poisson's Ratio.

That being said, you do need to worry about the warning message. Somewhere in your model you have stress singularities, which are artificially high areas of stress that can pollute stress results in other areas. You need to handle these areas using a combination of mesh refinement and isolating elements.

[neomechanikos]

Probably a geometry driven singularity (i.e. re-entrant corner). Stress is force/area. Given the same constraints, same force, and same geometry... both solutions can run off to infinity as the area gets smaller, trying to converge and only stop at some element order limitation. At some point down the rabbit hole, minute differences in material properties that affect stiffness (stress is calculated from nodal displacements) that you would normally see make no noticeable contribution to such a large stress and get washed out in the noise. That's my guess anyway.

Changes to geometry can also help in addition to what Shaun mentions. For instance, a small fillet or radii can sometimes eliminate/limit the singularity.

Are you using any non-linear material definitions? I'm guessing not...

[sbhushankumar]

No Eric I hvnt used any non linear material definitions.

[gkoch]

Hello Shashi,

have the answers from Shaun and Eric helped you improve the accuracy of your analysis?

Or helped you understand the results better?

Eric had asked about whether you use non-linear material definitions.

Gunter

[SylvainA.]

Your results appear logical:

As Young's modulus is defined by "stress/strain", using a material with a smaller Young's modulus can lead to a bigger displacement but (near) unchanged stress.

As the load stays unchanged and if part's shape doesn't change too much between both analysis, the force/area ratio (in other words, the stress) will not change much.

I just had a try with a quite simple part :

Steel:

max_beam_bending: 0.000000e+00
max_beam_tensile: 0.000000e+00
max_beam_torsion: 0.000000e+00
max_beam_total: 0.000000e+00
max_disp_mag: 3.841889e-02
max_disp_x: -6.662084e-03
max_disp_y: -3.813594e-02
max_disp_z: -6.697378e-03
max_prin_mag: -7.838474e+05
max_rot_mag: 0.000000e+00
max_rot_x: 0.000000e+00
max_rot_y: 0.000000e+00
max_rot_z: 0.000000e+00
max_stress_prin: 5.117959e+05
max_stress_vm: 5.181108e+05
max_stress_xx: -2.697148e+05
max_stress_xy: 3.419581e+04
max_stress_xz: -1.084008e+05
max_stress_yy: -2.697999e+05
max_stress_yz: 7.928438e+04
max_stress_zz: -7.758318e+05
min_stress_prin: -7.838474e+05
strain_energy: 1.402551e+04

AL6061:

max_beam_bending: 0.000000e+00

max_beam_tensile: 0.000000e+00

max_beam_torsion: 0.000000e+00

max_beam_total: 0.000000e+00

max_disp_mag: 1.114146e-01

max_disp_x: -1.950946e-02

max_disp_y: -1.105832e-01

max_disp_z: -1.935979e-02

max_prin_mag: -8.167479e+05

max_rot_mag: 0.000000e+00

max_rot_x: 0.000000e+00

max_rot_y: 0.000000e+00

max_rot_z: 0.000000e+00

max_stress_prin: 5.269868e+05

max_stress_vm: 5.019081e+05

max_stress_xx: -3.216662e+05

max_stress_xy: 3.401469e+04

max_stress_xz: -1.092101e+05

max_stress_yy: -3.210814e+05

max_stress_yz: 8.113525e+04

max_stress_zz: -8.038244e+05

min_stress_prin: -8.167479e+05

strain_energy: 4.062394e+04

[sbhushankumar]

Thank you everyone for your responses(and sorry for coming late)

I am not an expert in simulation so I handed this to my senior but still I would like to know the standard procees for carrying out the Load analysis. All I am worried about is that how can I come to know if the results are correct (those marked with *). Even though the results are displayed there isnt a surety that the results are accurate as it is displayed in that warning message at the bottom??

[SylvainA.]

If there are no " * " nor alert message, these values can be considered as reliable.

Anyhow, I would not use these values without having a look at the stress (or other quantity) over the model.

Found in the help file (Creo/Pro 5.0) :

"The way you evaluate results depends on the type of result window you are working with. For example, if you are examining fringe plots, you are likely to be interested in the location of the quantity maximum, the value of the quantity at specific locations, how one quantity compares with another, and so forth. If you are looking at animations, you are likely to be interested in how the model deforms, the pattern of deformation at different steps, how behavior in one mode compares with behavior in another, and so forth. "

[sdensberger]

All I am worried about is that how can I come to know if the results are correct (those marked with *).

This process can be rather involved and isn't something that can be summed up easily on a forms site. That being side, you first need to determine if there are any model properties that can cause singular results (e.g. a reentrant corner) and isolate the singular elements from convergence consideration. You then need to look at the measures of interest after running a Multi-Pass Adaptive (MPA) convergence scheme to see how the value changes with the p-loop.