tetra10 to hexa20 connection 1

[cagrisever]

Hi all,
I'd like to find a way to couple tetra10 and hexa20 elements in a region.
1- Is there a pre-processor where I can do this coupling, selecting e.g. the surfaces?
2- Is there a algorithm to write an equation between the middle uncoupled nodes of tetra10 and let's say corner nodes of hexa20?
3- Or anything.
Thank you all in advance.

 

[johnhors]

It largely depends on what software you are using. For example, both Lusas and Abaqus have "tied" slidelines which allow you to connect or "tie" together dissimilar meshes on a common surface, and this is probably best done using the pre-processors which come with these packages. Having said that, it is not good practice to use elements together that are incompatible. If possible it is best to avoid features like tied slidelines and build your model using just tet10's or hex20's.

 

[fkmeyers]

This problem is element compatibility WRT to the edge node of the tet10 that will be at the center of the hex20 face. What you will get if not adjusted is patchy stresses. What you want to do is remove that edge node on the tet10 elements that go across the hex face. I am not sure if this is still 100% correct but seems to make sense. The problem will be how to do this over a large region. I am not sure if FEMAP or Patran support such a feature but I do know that nastran allows you to arbitrarily remove an edge node on a tet10 or hex20 element. If you are using NEiNastran their surface weld element will handle dissimilar meshes without having to remove any edge nodes.

 

[cagrisever]

I think the best way is to use tetra10 and hexa4 elements. Then there won't be any node left. Do you think this will cause any issues?

 

[johnhors]

Yes !

In joining incompatible elements like tet10's and hex4's you will only get continuity of displacement. The rate of change of displacement with position (i.e. the first differential of the displacement function) = strain and hence stress will not be continuous. Thus you cannot expect to get any valid results for stress on and near the join.

 

[cagrisever]

Johnhors,
My area of interface is far away from this region. You won't get a correct stress distribution at the interface as you pointed. What if my point of interest is far away and I have at least 5 mesh layers between this joint region and my point of interest.?
Thanks for your help.

 

[johnhors]

Well cagrisever you can use the old get me out of jail free card by invoking the rule of St. Venant, which states that if your point of interest is sufficiently far aware from the poor modelling region you should be alright. However, it's not guaranteed, plus in my experience someone sometime (usually a manager with no FE knowledge) will pick up your results to look at a region other than your point of interest, blissfully unaware that the stresses are not strictly valid.