Singularities (or not...) in 3D flange model on Ansys Workbench 1

[murteira13]

Hi there!

I have been reading some posts on eng-tips about singularities, so the reason I am posting this thread is that I can't quite understand what type of singularity I'm getting on my analysis. I suspect there is one because as i refine my mesh, the maximum value for the von-mises stress on the flange keeps rising with no signs of stopping. This is a problem because I want to guarantee that the yield stress for my material isn't reached. And since there is no convergence of the stress value, i can't do that.
The images i'm attaching are successive refinements and corresponding stress distributions. I hope someone can lend me some insight into the subject, as my thesis presentationnis close and I should be able to produce reliable results.
It is part of the top face of the flange. The elements are hexahedral with 20 nodes. I applied a 10 kN force in a washer that sits on the shown face.

Thank you in advance for looking at this!

 

[murteira13]

Here's one image of the model in isometric view with applied forces and bc's

 

[corus]

Your results don't appear to be correct as you have spurious peaks at nodes within the mesh. Your results should be mesh independent, if anything. Generally though, when you have square regions then you'd expect peak stresses to occur at the corners. Your peak stress appears to be at the mid side of a face away from the corner so isn't a singularity.

 

[murteira13]

That's what I thought initially. In fact, the peak stresses don't appear at spots where singularities should present. But they are there and don't converge to finite values. I refined the mesh further and max stresses climb even more abruptly. I have already tried to remake the CAD model with different softwares and the peaks continue to appear. Any thoughts on why that happens? Could the element type have influence on this? Should I change to tetrahedral elements?

 

[corus]

Tetrahedral elements give worse, inconsistent results than brick type elements, so avoid them. Looking at the results again though I don't think you're using 20 noded brick elements but rather 8 noded ones. 20 noded brick elements are the best. The main problem I see isn't the increase in maximum values but rather that your results aren't consistent anywhere with strange peaks and troughs scattered around. This maybe due to splits in the model or perhaps loads are being applied inconsistently and not where you intended, or your material properties are being scattered around.
Personally I prefer not to use CAD models whenever possible as it takes longer to fix them than it does just to build the geometry yourself. Generally if you build the model use symmetry when possible and also check the mesh to make sure there are no gaps.

 

[aerostress82]

It looks like you are applying compression forces on your flanges. But your forces are being applied from those 4 circular structures (washers). So, you probably have "contact" defined in this interface between the washers and your flanges.

If this is the case, your contact parameters might be too stiff for sliding mechanism between the 2 contacting parts (actually 8 contacting parts in your case - given that you have 4 of these mechanisms in every corner).

And as you are refining it, you are hitting the jackpot more and more as your domain (elements) is getting "more sensitive" with decreasing mesh sizes.


This is the only thing I can think of. Not very familiar with Ansys, above comment was only by looking at the stress & boundary condition photos. If you could put the Ansys file somewhere, someone knowledgeable with Ansys would definitely catch what is wrong at once.

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[murteira13]

Thanks aerostress82, that actually seems to be the problem. Before I read your post I changed the contact type from bonded, which in my understanding is the stiffest possible contact, to frictional, and the red spots ceased to appear. Reading your post confirms it. I was a contact problem!

My thanks to corus and aerostress82 for helping me solve this problem!
Best regards!

 

[aerostress82]

You are very welcome Murteira. I myself suffered from lack of knowledge/experience when I first started stress engineering, so I try to solve whatever I can here when I have the time and the experience on the problem.

I think stress engineering is a very critical profession and you will also find lots of mistakes (already made) in your future FEA projects as well. This is mostly due to teams not discussing things at full length - or trying to look like they know what they are doing whereas they actually don't..


Let's clear whatever we can here on this website and in our companies, so that the safety of others is "never" compromised..

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer