Learning Forum

[Sam Fares]

Hello All,

The mesh symmetrical as shown in the second picture. In the analysis it shows the elements are not symmetrical. I am not sure why.

Regards,

Sam

[peteroznewman]

Sam,

Maybe there is a difference in the geometry and it it not a perfect mirror image, or maybe it's just the way the software works. In either case, you can apply Mesh Controls until you get the mesh you want.

Both images show a single solid element through the thickness of a part. That is a poor mesh. Use the Sizing feature of the Mesh details to Capture Proximity and set the Num Cells Across Gap to be 2 or more.

Regards,
Peter

[Sam Fares]

Hi Peter,

Attached is the model

I already had Num Cells Across Gap=2. 

1. What does Num Cells Across Gap do?

2. What does capture proximity do?

Also in this model the yield strength of steel Fy=50,000 psi, with the allowable yield strength=30,000 psi. This is a typical joist seat that we use and we never had any issues. The purpose of this model is to check the joist for wind uplift force.

Why i don't understand is that the stresses seems to be awfully high and way over 30,000 psi.

 

Regards,

Sam

[jj77]

It looks like this happens (remesh with tets), when you run through your design points. In the first run it is OK, but then (other design points) due to remesh it gives tets and hex element, thus different to your first mesh you see, which is structured and hex dominant. Sure peteroznewman will have some more feedback for you, because I never done a parametric study like that .

 

Seems also if you delete all the results then it runs only once, while if there are as they are from your original file then the simulations runs many times, and for the second run the mesh always changes to tets on some parts.

[Sam Fares]

Thank you jj77 for your reply. I didn't realize it re-meshes the model for every design point.

 

Regards,

Sam

[jj77]

 No worries. As for the stresses is because you need to add plasticity to your material models (engineering data). Say bi-linear isotropic hardening, as shown below (the limits you set I think are used by the safety tool only, not by the solver).

[peteroznewman]

Hi Sam,

I suppressed the existing mesh controls to demonstrate the global Proximity Sizing control under Mesh.

The thickness of the angle is 3.6 mm.  If the Proximity Min Size is > 3.6 mm then the Num Cells Across Gap is ignored.

But if the Proximity Min Size is < 3.6 mm, then the Num Cells Across Gap is applied.

Note that it doesn't work perfectly for this example. So additional mesh controls are required to achieve the desired mesh.

In the image below, the angles have been sliced into multibody parts with Shared Topology, and the Contact Sizing mesh control is being used to put smaller elements through the welds.

That last model is attached as an ANSYS 19.2 archive.  I did find a split face on one angle that was on one side only. That may be why that side used Tet elements. I didn't check it carefully, I just merged the two faces into one.

I didn't run the model to look at stresses. One of the loads needs repair. Once you fix that and run the model, see if the stress values have become more reasonable.

[EDIT: The first time I attached the file didn't have good contacts. This one has contacts that work.]

Regards,
Peter

[peteroznewman]

Hi Sam,

Now I can answer the question as to why the mesh went from a nice hex mesh that you saw above to this...

It's because you put a Convergence into one of your results. I almost never use this feature of ANSYS.

Your model has a stress singularity in it, the mesh just keeps getting refined and it doesn't converge on a true stress result because there isn't one.  Stress singularities are created when there is a sharp interior corner in the model like this one.

Regards,
Peter

 

[Sam Fares]

Peter,

Thank you for your time and effort!

 

1. Should i round all corners or certain ones? I am not sure which corner in that picture

2. Do i need to include a bi-linear material as suggested earlier?

Regards,

Sam 

[peteroznewman]

Sam,

2. Add a bi-linear material, as jj77 suggested, to relieve the geometric stress singularity by plastic yielding.

1. Only a ground and polished weld can hope to get away from a stress concentration. Simple welds like you are using are filled with stress concentrations.  The interior corner is where the red Max flag is in the images above.

If you have an answer to your original question, mark that post with Is Solution or ask a follow-up question. Open a New Discussion for a new question.

Regards,
Peter

[Sam Fares]

Thank you Peter!