Learning Forum

[wh05]

Hi, why my meshing only have the vertical line in the beam and horizontal line in column (picture 1) ?My geometry model is using line body to represent the beam and column. 

I need to generate both vertical and horizontal line in the whole structure which look like picture 2 meshing. Because I want to know the stress at the top and bottom of the beam.  What should I do?

 

[peteroznewman]

If you have solid geometry of the beams, and you fill those solid bodies with solid elements, then you can plot the stress at the top surface and the bottom surface of the beams directly. However, such a model will have a large number of nodes and elements, perhaps exceeding the Student license limits. If you are not limited by the license, it will take more time to solve.

The alternative is to represent the beams as line bodies and assign a cross-section to the line. Then the number of nodes and elements is very small and will solve in the Student license limits and will not take much time to solve. However, the output for beam models is different from solid models. You have inserted a Beam tool. I created a simple beam model that is simply supported at each end with a vertical line pressure. Look at the Maximum Combined Stress.  If there is no Axial Stress, then the Combined Stress is just equal to the Bending Stress.

The maximum stress of 217 MPa is the bending stress + axial stress. In this example, we know the maximum bending stress is at the bottom of the cross-section, because that is the side that is in tension.

The minimum combined stress of -217 MPa is the bending stress + axial stress. In this example, we know that the compressive stress is on the top of the beam.

Now I could change the direction of loading and push on the beam sideways, now the minimum combined stress is -148 MPa and we know that occurs on the right side of the beam.

While the Maximum Combined stress is 148 MPa and we know the tension is on the left side of the beam.

If the loading combines vertical and lateral forces, the maximum and minimum value are only for whichever one is larger, and does not show the combined stress, but the Total Bending Moment will show the combined loading.

[wh05]

Thank you for your detail reply. Yes, that is what my struggling. I cannot plot it in solid because exceed the student limit. Also, I am not sure if I plot in 3D element, will it affect my result?

I am using the line bodies and section applied which is your alternative method. The loading is combined vertical and lateral load in my model. Whether the result of deformation and BM would not affected by this meshing?

Thank you for your explanation on stress. Is that a only way to show the stress in workbench? Because my dissertation need to express in the way same as my above second picture. Do you think that ANSYS APDL can do that? If so, do you know how can import my workbench geometry into APDL?

 

[peteroznewman]

Plotting does not affect the result.

The result can be affected by meshing, that is why you do a mesh refinement study, to make sure you have enough elements for the result to stop changing.

I don't think APDL can give you anything more.

Ask your school if it has an unlimited Research license that you can use during your dissertation.

[wh05]

I asked my school before, but unfortunately they only get the student license as well. So I don't have any method in workbench now..

In APDL, I know if choosing beam type for the element type (below picture 1), it can work out the stress result with horizontal meshing line. (below picture 2)

 

However, when I tried to import my workbench mechanical model with .inp file into APDL, it cannot run any result on shear stress and bending moment. So, I am get lost what I can do now.

[jj77]

APDL Peter can give much more in terms of plotting the stress on beam cross section - workbench is not great at that, since it does not render the full stress (tension and compression) on the section, which is very confusing for many engineers.

(Have in mind that Workbench is just another pre/ post processor for APDL, thus APDL methods/solvers run in the background ).

 

As you can see in the above image APDL with ESHAPE command renders the complete stress on the cross section, thus both tension and compression parts, as it should be. (here it is EQV, which is strictly positive hence no negative side, but if one plots X stress that will be both tension and compression)

 

As you can see wh05, the cross section mesh (different to the one we talk about along length), can be seen there. This internal mesh is used to calculate internal stresses on the cross section just as you show and also for the nonlinear calculations (see all key-options in beam188 in help where the cross sectional calculations can be defined and changed). This mesh can be changed possibly (in Strand7 we can). In your case as you can see there are 4 (2X2) elements on the cross section, but that should change (say to 8 or something). See below how to change the cross section mesh (change yellow marked fields)

 

 

[hamzaDZ13]

Hi , I've actually the same situation here , i modeled a steel frame with lines bodies but it didn't gave the proper mesh and besides i can't get the von mises stresses  and maximum principals strains from results as shown on the second pic under . 

Is it available to draw a simple frame with solid bodies in ansys workbench or it's better to use AutoCAD or solidwork and import it ?

[peteroznewman]

Workbench includes two geometry editors, DesignModeler (older) and SpaceClaim (newer).

Use SpaceClaim to sketch the cross-sectional area of a beam, then Pull that area into a solid of the desired length of beam. On the Prepare tab, you can click on the Beam Extract tool and it will replace that solid body with a line body and the proper cross-section.

You can also use AutoCAD or SolidWorks to create extruded solid shapes then open the file in SpaceClaim to use the Beam Extract tool on the Prepare tab.