It depends on the meshing method (sweep vs regular), type of mesh (rectangular vs tetrahedral), and the type of element (linear vs quadratic)

However, if everything is the same you should find similar results as FEA software are using more or less same solving methods

If you are trying to mesh this part, I highly recommend the use of sweep along an axis in Abaqus. Like that you may avoid small elements near the edges which may cause the appearance of stress concentration

It depends on the meshing method (sweep vs regular), type of mesh (rectangular vs tetrahedral), and the type of element (linear vs quadratic)

However, if everything is the same you should find similar results as FEA software are using more or less same solving methods

If you are trying to mesh this part, I highly recommend the use of sweep along an axis in Abaqus. Like that you may avoid small elements near the edges which may cause the appearance of stress concentration

abaqus by default uses linear reduced integration elements, ansys 2nd order...have you checked element types?

I agreed all answers below. And I add you can look the numbers of iterations in each step, which could be different in Abaqus and Ansys. Depending of where you export your geometry, both programs can understand this geometry in a different way, refining distinct regions of the geometry.

It depends,

a_ Mesh

b_ Type of Element

c_ No. of Iterations

d_ Average Stress Results and so on

The simulation with the finite element method gives approximated outcomes. For this problem type the convergence of the solution it is guaranteed with the uniform h-refinement of mesh. Within of regions with fast change of the stress there is the possibility of discrepancy of the results.

However, I recommend to simulate at the two programs with the most similar mesh possible, including: same elements (tetrahedral ou hexahedral and linear or quadratic) with minimum distortion, same refinement level, equivalent number of degree of freedom .

If not work I recommend review all the input data and units.

If the framework is linear, try to use higher order elements for both simulations. Also be carefull about the Units in these two software.

If it involves nonlinearity. Then you should check all the items listed below:

linearization method

convergence criterion

considered tolerance

You also need to keep in mind that stresses are calculated at integration points and then extrapolated to the boundaries of your model. If you read off maximum values directly from the contour plot, that may be off by a large amount from what happens at the integration points; depending on how the extrapolation is done, you can easily get very different results.

Before using any software, you should check the convergence of its results with analytical solutions or with different meshes until you get acceptable results. Then, you should use the same type of elements and same meshes in comparison.

As already mentioned by many of those who has responded, you will need to ensure that the mesh and elements types are similar along with convergence criterion etc. In addition, do also consider the flow stress data being used by ANSYS and ABAQUS although I do not suspect that there will be a huge difference but if you are not inputing your own flow stress data, the two software could be using flow stress properties that can be quite different. That may be something to check as well.

HI

YOU NEED KNOW THAT THE MESH IT TOTALLY DIFFERENT AND ALSO THE ELEMT TYPE AND THE NUMBER OF NODES THAT IF WE SAY THAT THEY HAVE THE SAME BOUNDARY CONDITION , MOREOVER SEE THE ACCURACY OF RESULTS FOR EACH PROGRAM AND MAKE SURE THAT ALL THE INPUT ARE THE SAME IN BOTH PROGRAMS , TRY TO SEE THE MESH DIFFERENCE AND THE NUMBER OF NODES IN EACH PROGRAM AND IS IT THE SAME ELEMENT TYPE?

.

REGARDS

I'm so glad that there's a great community to help students like me.

Thank you all for taking your time to answer my question.

Even-though still I didn't get a proper time to do an analysis with exact same mesh in the two software's.

I will definitely update when I get a result from such a simulation.

Thank you All!

It depends on the type of elements and meshing methods in the two software mentioned.

Good question.. Please share me the best answer might you trust...

Regards…

Dear All,

These are the reasons why the simulation results were observed to be different,

In Abaqus - Meshing was done in Hypermesh using linear elements. Results were post processed using Hyperview, where the default result viewing type is elemental stress.

In ANSYS - Meshing where done in ansys mechanical with quadratic elements. Results were post processed inside ansys mechanical where the default result viewing type is nodal average stress.

Mesh density - In both software mesh density was kept as close as possible.

Boundary conditions - same in both software.

At the time of the simulation I thought the default result type in hyperview is also nodal average. But when the results converge the elemental stress and nodal stress should be in close magnitude.

But for this simulation fairly low resolution mesh is used, where there would be significant difference between the nodal average and elemental mean results.

After finding out the reason I viewed the results at elements in ansys and the stress results were nearly close to ones obtained from abaqus even though two types of elements were used.

So in conclusion following are the reasons,

1) Using low number of elements where there is significant difference in nodal stress and element stress.

2) Using two types of results for processing.

Stress concentration in corner of partsis happend. Result of simulation isnot valid in these aeria. Pless point to near point to corner for correct stress in abaqus.