Can we do following type of analysis inside FEMAP? If Yes, in which module?
Scenario: There is cylindrical Part mounted on a Shaft with Interference Fit. (Cylinder is heated and Slid on Shaft which forms a grip when cooled down)
Failure : This cylinder slides off the shaft when the shaft is rotated in excess of 12000 RPM. Due to Inertial or gyroscopic effects
Simulation needed :
Failure : grinding wheel comes into contact with the job. This grinding wheel deforms to become convex in shape. This results in inaccuracy grinding of part. (These machine do grinding up to 5 Microns).To overcome this they using in process gauge which measures the job as it gets grinded. This gauge cost ¼ of machine cost.
To learn how to solve an interference-fit problem ("Snap-Fit“, “Press-Fit“, “Overlapping“, etc) using NX NASTRAN (SOL101) analysis take a look to my blog in the following address:
Basically you need to create the geometry of the contact parts with its real geometry, mesh them using high-order elements CHEXA 20-nodes (making sure to have midside nodes moved to the geometry for sure!!) and define surface-to-surface contact using a NEGATIVE MINIMUM SEARCH DISTANCE in the contact property to capture the existing interference, this way the NX NASTRAN solver will resolve the interference fit and compute the stress results in both parts, OK?.
You can solve your problem in 2-D as well, for instance a plain strain analysis, or in 3-D using 3-D Solid elements, in this case you can study 1/4 problem in order to stabilize the solution using symmetries ...
An extra piece of info which might help is that you can control the intereference level using the "Region Options" button when creating or editing a Connection Region. The Region Option allows you to set a Region Offset which moves the effective location of the region's contact interface. A positive offset "thickens" or "increases" the contact region, whilst a negative offset thins or decreases the contact region.
The best results for detailed interference analysis occur if the mesh at the interface is well matched - even though it is very easy to set up contact and intereference without the mesh being matched. Similarly, because contact intereference stresses are highly sensitive to node position, it is wise to have Femap write the Nastran model using large field format. This is via Model | Analysis... -> Options -> Bulk Data -> choose Large Field (All but elements).
And if you cannot get good mesh matching or a nice fine mesh at the interface, it is worthwhile knowing that Region Offset is evaluated AFTER "Initial Penetration" shown in Blas' reply. Thus if the mesh at the contact interface is not "perfect", then it is perhaps better to set Initial Penetration to Option 2 (ignores initial penetration), and then control your interference level entirely through the Region Offset.
Lastly, keep in mind that to avoid singularity, you may need to set a friction coefficient, which must be sufficient to sustain any torque or lateral force on the interface (even if nominally negligible) . If not, then you will see that contact convergence is likely to be very erratic.
Applying the RPM load is easy via Model | Load | Body, and choose the rotational velocity, direction and centre of rotation.
Looking at your blog, I was wondering, and excuse me for kidnapping this thread...
The results of HEX20 and TET10 are practically the same (as you stated in the blog) and the computation time is only about 25% longer, it seems that the benefit of HEX elements doesnt exist. If I am thinking about the simulations I am doing on daily basis - the meshing in HEX is most of the times impossible (very complex geometries), and where it is possible it will take me the whole day (or a few days) to get a reasonable mesh. I know this is a philosophical debate, but it seems that with todays powerfull computers and very complex geometries allowed by modern manufacturing processes - the choice of HEX elements (at least in implicit analysis) is not reasonable in a lot of scenarois,
What is your opinion about this?
I love the HEX elements for multiple reasons (high accuracy & reduced model size), but the use of TET or HEX elements will depend of the complexity of the geometry, and your ability to prepare complex geometries to mesh with HEX elements, if not the full body but slicing the solid in regular portions, and them to use GLUE FACE-TO-FACE, this way you can reduce model size a lot, as well to obtain accurate results.
Also, in the near future I hope to see in action in FEMAP soon the HYBRID 3-D SOLID MESHER: HEX mesh in the surface, TET elements in the core and PYRAM elements for transition!!, stay tuned.
Sometimes there is no choice but to use hex elements. I had a model where the geoemtry was such that I tried to mesh with tet elements and ended up needing well over 3 million nodes before the mesh quality was sufficient. Below that it was just rubbish. That was just too large to solve in a reasonable amount of time so I bit the bullet and did a lot of slicing and dicing to enable meshing in hex elements and ended up with a much more reasonable 600,000 nodes.
I was reading a little bit on pyramid transition elements.
As I understood, the general reccomandation is not to use them in stress concentration / important areas of the model - they are not reliable. The question is - what is their advantage on the glue method?
Any transition method (being GLUE, PYRAM or TRIA elements) should be avoided to use locally just in the region of stress concentrations, of course!!. In the case of HYBRID meshers, the benefit is that the transition is done without geometry, internally in the solid, so far from the surface. Please note for thick solids the region of interest in general is to compute the stress field in the outer surface where HEX elements are used.