Can someone help explain what is meant by top and bottom for Target contact side in the surface to surface contact dialog box? What is the definition of top and bottom? In the attached image the green mesh is a cylindrical shell mesh 0.04mm thick, and contacts objects on both the inside and outside surfaces. I'm just wondering if the top is the Outer diameter surface or inner and how to figure that out in the future.
Top/Bottom designation only come into play if the region is composed of shell elements. In this case, 'Top' is the side with the positive shell normal as determined from the element connectivity using the right hand rule. Bottom is of course the other side of the shell
For solid meshes, contact always occurs external to the material so the software implicitly knows what the contact direction is on a solid free face and this setting does not have an affect.
Dear Nsmith, In fact, Top & Bottom faces in Shell elements is a very important feature that any FEA user should have a clear idea of what means. It is related with shell element oientation, and you can plot the orientation of Shell elements very easy in both *.FEM & *.SIM environments.
In the FEM click in the 2D Collector RMB and select "Edit Display ..", then you can activate to display the 2D normals using vectors (see attached image), the direction of the vector is the TOP orientation of your Shell elements, the reverse is the BOTTOM.
You can reverse the TOP/BOTTOM orientation of you Shell elements using command "Analysis > Finite Element Model Check > 2D Element Normals", simply play with it to understand the running.
Also, terms like "Source (Slave) Contact Regions" and "Target Contact Regions" are very important to understand correctly in order to solve with success contact problems.
It's important to understand how contact elements are created when selecting which region will be the source and which the target, since the two can be interchangeable. The NX NASTRAN solver projects vector normals from the source region to the target region. It then creates contact elements when these normals intersect elements in the target region and are within the search distance criteria for the contact pair. This means that when the two regions of a pair do not have corresponding one-to-one elements, the number of contact elements that the solver creates can change depending on which region it projects the elements from and which region it projects them to.
In general, of the two contact regions you use for the pair, choose the one with the finer mesh for the source region. When the source and target regions have different mesh densities, more elements on the source region will mean that more contact elements are created, which will produce a more accurate solution, clear?.
By the way, you mention you have Shell elements with contacts in both sides, in case you run an Advanced NonLinear Solution (SOL601) you may activate the "DOUBLE-SIDED contact surface (NSIDE)" option.
Well, I hope the above helps you to run your contact problem. Best regards, Blas.
Blas and Jim,
Thanks for the clarification and help! I've been looking for that option to see the element normals. always nice to double check.
I've also heard that it is good to choose the softer material as the source region also. I will check out the double-sided contact as I am using the Advanced nonlinear solution 601 for this model.
Thanks for the help and quick response.
Now I'm off to learn how to complete a restart analysis.