Hello everyone I hope someone can take a look at an analysis that I am working on. It’s regarding a coupling with conical clamping element. (see file below)
I will be doing this in multiple steps, but currently only one is in progress and in my opinion the trickier one.
Clamping
Temperature
Torque + Centrifugal forces (or maybe these need to be split)
Basic explanation, you clamp the conical ring with bolts which then bend the hub to act upon the shaft. The bolts used are M8. The shaft and the hub have a fit of D40H7/h6 which gives around 41 micrometers of clearance which is the worst case scenario. According to the manufacturers documentation the tightening torque for the bolts is around 30 Nm, analytical calculation results in 23 kN. But this largely depends on the coefficient of friction of course.
Initial conditions:
Initially I use a temperature “shrinkage” on the bolts due to the analysis being non-linear. The temperature is arbitrary picked through experimentation. This work fairly well but I do have “high” stresses on the ring underneath the bolts.
Contacts:
The contact between the hub and the ring is frictional + hard.
The contact between the shaft and the hub is something i’m not 100% sure about, because initially there is a geometrical gap of 41 micrometers. If this can be done another way without making the shaft diameter 41 micrometers smaller that would be awesome. Another thing to note probably is the meshing of this diameter, perhaps I lose accuracy if the elements are too coarse.
Questions:
If I shrink the bolts using temperature dilatation, how would i implement the second step? The second step would make all parts have around 60 degrees Celsius. This would mean it would go from e.g. -1000 to 60 degrees, which will basically “reset” the bolts.
What would be a proper way of modelling the shaft → hub connection?
How much should I refine the mesh between the shaft → hub (element size) ?
Recent updates have added cylindrical coordinate system. Is there a way to display displacement relative picked coordinate system?
This means some of the output saved in the .dat file can not be parsed correctly. Can you share the .pmx file throwing the error or the .dat file for me to work with?
Since I could not find the proper place to add the *CLEARANCE card I have added it beneath the contact definition:
*Contact pair, Interaction=friction, Type=Surface to surface, Adjust=0
ring_inner, hub_outer
*Contact pair, Interaction=Surface_Interaction-2, Type=Surface to surface, Adjust=0
hub_inner, shaft_surface
*CLEARANCE,MASTER=shaft_surface,SLAVE=hub_inner,VALUE=0.041
If this is not correct, my next hint would be to add it in the *STEP definitions.
I just assumed that the pretension would not work on a non-linear analysis (ANSYS rejects doing a non-linear simulation with pretension).
Since the video does not have any sound (at least on my side) what would be the purpose of creating the “Compound boundary layer” with 0.1 mm? How does the value affect the pretension?
EDIT: The files are using development version 2.1.5.
Note that the results of the simulation are not available in PrePoMax not sure why. But the .dat file is from the last done simulation.
I changed the input geometry of the simulation at one point and then re-referenced all the node sets, etc. When the results were available the error poped-up.
But basically, a boundary layer is needed because of the CalculiX limitation that the pre-tension surface shouldn’t include edges or vertices of elements that don’t have any faces belonging to that pre-tension surface. So a layer of prismatic (wedge) elements is created in PrePoMax to ensure that.
The problem you reported for reading .dat files is strange. For some reason, CalculiX exports the number of contact elements for a single time increment multiple times and PrePoMax does not know what to do.
Currently, you have two solutions. If you do not need the number of contact elements in the history output - CNUM, turn it off. Everything should work in this case.
If you need the data you can fix the .dat file by hand. Open the .dat file in an text editor and search for the entry:
total number of contact elements for time
You will notice that it repeats the same value twice. Delete all three rows for the second appearance of the number of elements:
total number of contact elements for time 0.2000000E+00
19600
Then open the results again. But, in this case, you have to do this automatically after each simulation run.
I will fix the .dat reader to cope with such situations for the future.
Following model was simplified as a quarter for faster solver execution. PMX file
It seems I can not get the simulation to converge when using the *CLEARANCE card. It succeeds a few steps and then just “zig-zags” around without lowering residual force / displacement with the contact elements staying pretty much the same.
I’ve tried placing tied contact between the shaft and the hub and this does converge but a strange thing happens. The contact area between the conical ring and the hub is pretty much 0 throughout all of the steps - even though there is a contact pair definition.
I also didn’t remove the clearance card when placing the tied contact - not sure if it has an effect in this type of contact.
Another question is, even when i specify preload of ~46kN for two bolts - the forces on the node sets are nowhere close to this force, is there a reason for this? Perhaps I need to keep the total of 184kN even though the model is symmetric (an oversight on my side?).
Reaction forces in the direction of the X-axis of “THREAD_1”:
direct incrementation may not be a good idea when convergence issues occur
you don’t have to add *INITIAL CONDITIONS, TYPE=TEMPERATURE and *TEMPERATURE via keyword editor, they are available in GUI (under Initial Conditions and Defined Fields)
are those rigid body constraints on bolt used to connect them to the hub ? Apparently, they are using the same reference points. ? Abaqus wouldn’t allow it. Tie constraints could be sufficient at least for some of such connections.
you could read the pre-tension force from bolts using section print (has to be added via keywords)
as discussed in the linked CalculiX forum thread, the *CLEARANCE keyword may not work as expected but tied formulation may at least help with uniform results
it’s good to check contact field outputs such as CPRESS and COPEN to see if contact is established properly/uniformly
you should reduce the force in the bolts due to symmetry only when the bolts are cut too
it’s always good to simplify the model for tests if there are issues with more advanced features (like *CLEARANCE)
The problem is how you defined the surfaces for pretension. You created the surfaces based on node sets, this results in element distortions and wrong reaction forces, even though you have created a layer of C3D15 elements (1). Just skip creating node sets, create or select the wedge-element surface directly (2):
