Different element size on shared surface edge
Altair EmployeeHi,
I am more interested in stress distribution at one location of the model than on some other parts. In the field of interest I would like to make mesh finer compared to other regions of the model.
This means that on the shared surface edge I would like to have 2 different element sizes. Could someone tell me how to do this? I am using 2D shell elements with 2D-automesh panel and this tool does not allow to have different element sizes on shared edge.
Please also see the attached figure.
Thank you.
Answers
-
Hi Ziga,
one way is to bias the elements on less priority surface(refer to picture below). After you click Mesh on automesh panel, it will take you to a secondary automesh panel, where you can bias the elements. On Biasing you can select the edge you want the elements to be biased and bias style. Make sure the elements are within the criteria after biasing.
please let us know if this helped.
<?xml version="1.0" encoding="UTF-8"?>
0 -
<table width='100% cellspacing=' 0'='' cellpadding='0' border='0' style='border-collapse: collapse; border-spacing: 0px; border: medium none; width: 660px; margin: 0px; padding: 0px;'> Re: Different element size on shared surface edge
on: July 24, 2013, 01:10
when you have two surfaces that are connected to each other you can identify/modify the three types of connectivity one surface has with the other, the three types are
free edge (red)
shared (green)
suppressed (blue)
to change the connected edge type you can use toggle edge in quick edit > toggle edge
With this lines selector highlighted, Left-click a free edge (red) to make it shared (green), or a shared edge to make it suppressed (blue). Right-click a suppressed edge to make it shared, or a shared edge to make it free.
meshing the surfaces when they have free edge will not result in any connectivity no matter what the setting is in automesh, meshing surfaces with shared edges will reflect the connectivity option you use in automesh, If you use redo connectivity then mesh in surrounding areas of the surface you are meshing now will automatically be changes so that there are no free edges/dissimilar node count.
you can see how connectivity options have an effect on the second surfaces with the green shared edge while the first with the red edge does not take connectivity into account and the third with suppressed behaves as one surface instead of two different surfaces
0 -
In the HyperMesh student guide you can go through
4.8 Meshing in Critical Areas and Mesh transition techniques and flow lines
Since you need to transition from a coarse mesh to a finer mesh.
0 -
Ziga,
you can also try surface deviation subpanel in automesh panel. but it may create tria elements.
if you don't have issue using a couple of trias, then use surface deviation option
0 -
hank you guys form such a quick response.
I will only be doing some linear static analysis so I guess trias elements are acceptable. But I am trying to avoid trias since my supervisor told me they always cause troubles. But as I already told you I think for static analysis they are ok but if you are dealing with crash analysis it is better to avoid them.
You gave me some nice ideas and I would like your opinion. Here is what I did. I made the green shared edge a red free edge. Mesh density on lower part is 20 and on the upper part 40. Still I want to keep the connectivity between those 2 surfaces thus I did the nodes equivalence (see the figure). Is this procedure ok? In this case what happens to the nodes not connected (coloured with red)? I attached a zoom of the connection.
I also checked some meshed parts again and I noticed that sometimes not all of the nodes are connected (last figure).
0 -
This can be solved by some manual editing, I would split those trias into two using 2d > edit element > split and for the points select the node you have highlighted and the node at the bottom of the tria.
0 -
Could I also get some comment about the first figure I posted in my previous reply. Is that correct method? I have seen some FE models with the change of mesh density the way I described but I do not know the background of the work.
Thank you again for the help.
0 -
Ziga,
refer to the below picture. I have used surface deviation.
you can also edit the mesh manually as Rahul said in his previous post by splitting the elements. It is recommend to avoid tria element at the edge as they can induce strains.
<?xml version="1.0" encoding="UTF-8"?>
0 -
Actually it makes sense what all you guys are saying.
This is the reason why I am confused. Please refer to the attached figure. The model was created by one consulting company and it can be seen how they made transition on some regions- I marked it with red colour. With no trias and with each second node left unconnected. But unfortunately I have just figures about it so I do not know in details how they did it.
0 -
If there is not contact definition between those two element mesh sizes, I would recommend to do it otherwise.
The problem are those unconnected nodes which can move quite a bit without causing stress. Correct me if I am wrong, but that is like using second order Elements whith one node in the middle causing sometimes the problem of overshooting.
I would suggest talking to the consulting company and asking them what they thought about this transition.
0 -
Hi,
I spent some time investigating the mesh transition technique I described- please refer to the figure posted on July 25, 2013.
I had a meeting with my supervisor and I asked him about this method. He told me this technique is called “TIED INTERFACE”. He told me that this technique is enabled e.g. in LS-DYNA solver. I attached the figure from some papers I found. Some recommendations from the paper:
-good for tying parts with disparate meshes
-Criteria for tying: the slave node lies within the orthogonal projection of a master segment
-Side with finer mesh should be slave sideStill this does not help a lot because I use RADIOSS Bulk- linear static. I checked the Features of Finite Element Analysis using Bulk Data Format and one bullet point is: Contact, tied interface. Further on I found card image TIE which defines a tied contact.
Does anyone have experiences using this contact? How appropriate is it?
Thank you.
0 -
Ziga,
Tie or freeze should work,
Try with a simple model and see the differences between
mesh transition
Tie
freeze contactIn RADIOSS bulk - TIE element is created of a same structure as FREEZE CONTACT element. TIE element enforces zero relative motion on the contact surface – the contact gap opening remains fixed at the original value and the sliding distance is forced to be zero. Also, rotations at the slave node are matched to the rotations of the master patch.
0 -
Rahul,
I have just seen you modified your post. I already had prepared answer for you:
“I am modelling cab structure of the truck which is fabricated using thin walled members thus the cab is idealized using 2D shell elements. I am going to perform linear static analysis- RADIOSS Bulk Data. Few load cases are going to be considered: -longitudinal inertia 1g, -lateral inertia 1.2 –torsion.
In the critical area I want to use much finer mesh compared to general areas. I have read about Meshing transition techniques in Student guide (refer to figure attached) but this works only for small transition. If the difference in mesh density is big then I might get more distorted elements (automesh tool).
This is why I wanted to use TIE connection to avoid diamond and trias elements at transition. But if this option is only for non-linear analysis I guess I cannot avoid that.”Now according to your edited post I see the TIE option is available also for linear static analysis. The comments for TIE card image are really a bit misleading- comments for nonlinear quasi-static analysis.
I will try what you suggested, first with the simple example and try to see if there are any differences.
So actually TIE and FREEZE CONTACT should do the same? And probably you meant CONTACT card image for freeze contact?
0 -
Ziga,
Yes, they should do the same for this use case,
Yes, I meant CONTACT card image with type as freeze,Another option is use rigids to connect the different meshes but I would not advise it,
You will have to manually edit the distorted region or mesh with the other techniques in such cases.
0 -
Hi,
Finally I did some testing on TIE connection, I used the example from the documentation:
-RD-1000: Linear Static Analysis of a Plate with a Hole (I used same boundaries and loading)
I did 3 cases:
1) Plate is cut in the middle with no connection. The response is symmetric as it should be.
2) Plate remains the as one piece as one component. Once again the response I get is symmetric.
3) Plate is cut in the middle and TIE is used to connect the surfaces. Mesh is 2x finer on the right side of the plate (finer mesh as slave). In the figures I attached it is seen that displacement response is symmetric but stress distribution is not symmetric- be focused on the mid line. Is there any explanation for that?
Please refer to the figures I attached for all the cases.
Regards
0 -
Another 3 figures:
0 -
Ziga,
the simple answer to why there is a difference in symmetry: Its the mesh size.
The finer the mesh, the finer the results one can say. Remind the finer half and do a analysis with the complete model meshed with this meshsize and I bet it will be symmetric.
You are looking at discrete values on your hyperview pictures. Roughly it is symmetric (Maxima are at the same spots e.g.). For different mesh sizes a discrete result will be never the same (for the same loading and constraint)
Best Regards,
Manuel.0 -
We must also consider the loads applied, how are you dividing the loads in the hole, are you using the same number of nodes or a different size? perhaps you can skip a node on the finer size when applying the same load as you are using half the element size?
The interpolation functions of quads must be considered and how element size factors in this,
0 -
Altair Forum User said:
Actually it makes sense what all you guys are saying.
This is the reason why I am confused. Please refer to the attached figure. The model was created by one consulting company and it can be seen how they made transition on some regions- I marked it with red colour. With no trias and with each second node left unconnected. But unfortunately I have just figures about it so I do not know in details how they did it.
As per the figure, Can I also define freeze contact between two element which has two different meshes like trai10 and Hexa 8? Please tell me how?
0 -
0
