-
-
December 2, 2024 at 9:03 amsimon.paajarviSubscriber
Hello!
I am interested in modelling e.g. simple journal bearings represented by two-dimensional spring elements in rotor dynamic simulations.Â
The bearing stiffness matrix (and damping matrix) is generally on the form [K] = [k_xx k_xy; k_yx k_yy]. The bearing is thus two dimensional and only gives a force output in a plane defined by the x and y coordinates.
I am familiar with the one-dimensional spring elements (e.g. *ELEMENT_DISCRETE AND and MAT_ELASTIC_SPRING_DISCRETE_BEAM) and they do the job perfectly for the diagonal stiffnesses. However, I am not sure how to incorporate the cross-coupling entries in a simple way.
*ELEMENT_DIRECT_MATRIX_INPUT seems like a reasonable option, but it seems to require some work with the DMIG-files - which would be a last resort option. If you have any good tutorials for this, please let me know :-) -
December 12, 2024 at 9:55 pmReno GenestAnsys Employee
Â
Hello Simon,
You will find more information about rotor dynamics in LS-DYNA here:
Introduction of Rotor Dynamics using Implicit Method in LS-DYNA ® — Dynalook
http://ftp.lstc.com/anonymous/outgoing/support/EXAMPLES/rotational_dynamics_2017.tar.gz
Let me know if this helps or not.
Â
Reno.
Â
Â
-
December 13, 2024 at 9:58 amsimon.paajarviSubscriber
Thank you for the documents!Â
It seems that the preferred way to model bearing stiffness is by the use of joints with rigid bodies. However, I can only see input options for the diagonal stiffnesses (x-force as function of x, y-force as function of y), but no possibility for cross-coupling (x-force as function of y, etc). I might have to resort to either the DMIG-option or simply program forces by the use of the *DEFINE_FUNCTION-option, which would be valid for transient simulations.
However, the files give a lot of valuable information about the best practices for modeling rotating systems with contact, which I am very grateful for! Thank you. -
December 13, 2024 at 9:20 pmReno GenestAnsys Employee
Hello Simon,
Maybe the keyword *CONSTRAINED_JOINT_STIFFNESS would help assigned the appropriate stiffnesses: LS-DYNA Keyword Manual?
Â
Reno.
-
December 16, 2024 at 10:25 am
-
December 16, 2024 at 11:41 pmReno GenestAnsys Employee
Hello Simon,
Another option is *ELEMENT_BEARING (see also *DATABASE_BEARING). Refer to the LS-DYNA User Manual Vol I for more information.
Â
Reno.
-
December 17, 2024 at 11:34 pmReno GenestAnsys Employee
Hello Simon,
I checked with a developer and he said: "superelements sounds reasonable, assuming small displacements. There is also the flexible body approach, *part_modes, but not sure how well this works".
Also, have you tried modeling your rotor dynamics with Ansys? There is a section in the help about rotor dynamics:
5.15.13. Rotordynamics Analysis
And bearings:
"As required, define the stiffness coefficients (K11, K22, K12, K21) and the damping coefficients (C11, C12, C21, C22). These may be entered as Constant values or using Tabular Data entries."
Â
I think this is exactly what you are trying to do.
Â
Let me know how it goes.
Â
Reno.
Â
-
December 17, 2024 at 11:44 pmReno GenestAnsys Employee
Hello Simon,
You will find more information about *ELMENT_BEARING on the aerospace working group website:
AWG ERIF Test Example 14 | LS-DYNA Aerospace Working Group
You will find a paper, an example model, and other documents.
Â
Let me know if this helps or not.
Â
Reno.
-
December 18, 2024 at 9:24 amsimon.paajarviSubscriber
The *ELEMENT_BEARING seems to be limited to a rolling element bearing, but the numerical study you provided gave me a good idea how to apply unbalance forcing. :-)
The example you found from ANSYS is exactly what I am trying to achieve in LS-DYNA. The reason for choosing LS DYNA is that the final objective is to implement impact-rub simulations for the rotor, which seems to be a limiting factor for more specialized, rotordynamic modules available in e.g. ANSYS, NX NASTRAN, etc. They have very good capabilities for the rotordynamic simulations (e.g. bearing modeling, unbalance loads, etc) but do often not support contacts.
From your input, I think the superelement is the most suitable option. Do you perhaps have any accessible tutorials or examples for this? The manual does not describe a lot when it comes to the application. -
December 18, 2024 at 5:29 pmReno GenestAnsys Employee
Hello Simon,
I found the following in our knowledge database:
"
Superelements are not appropriate for bodies undergoing finite rotations. For that case, one could employ flexible rigid bodies (*part_modes)"
One developer told me: "We are working on extending it to large rotations, underway."
And here is more information from our knowledge database:
"A "flexible rigid body" saves cpu time by approximating response using mode superposition. The basic procedure is to first compute normal modes (*control_implicit_eigenvalue) and/or constraint or attachment modes (*control_implicit_modes) of a deformable body. Then in a subsequent explicit analysis, you approximate that deformable body as a "flexible rigid body" via the command *part_modes. Here are links to papers describing the procedure and examples: http://ftp.lstc.com/anonymous/outgoing/jday/Session_12-1.pdf http://ftp.lstc.com/anonymous/outgoing/jday/flexrb.pdf http://ftp.lstc.com/anonymous/outgoing/jday/Bitzenbauer.pdf The first two are essentially the same paper. Example input (rather old, I'm afraid) is in http://ftp.lstc.com/anonymous/outgoing/jday/flexrb_example.tar"
You will find a regular super element example here:
http://ftp.lstc.com/anonymous/outgoing/support/EXAMPLES/superel_inertia_matrix.tar
Let me know if this helps or not.
Reno. -
December 18, 2024 at 5:31 pm
-
- You must be logged in to reply to this topic.
- LS-DYNA Installation Issues with Student Workbench 2024 R2
- Mathematical model generation stuck at 10%
- Cross-coupled stiffness elements in LS-DYNA
- LS-Dyna CESE SMP d vs MPP d solver
- CESE solver – Ignition mechanism
- Initial Stress Shell Application and HistVarCosine in LS-DYNA
- shape memory alloy material in LS-DYNA
- MAT072R3- concrete damage rel3 validation
- *** Error 40058 (SOL+58) retractor 1000002:convergence failure at time1.01E+02
- Initial Velocity Generation
-
1572
-
602
-
599
-
591
-
366
© 2025 Copyright ANSYS, Inc. All rights reserved.