Is there a tutorial for STEADY STATE DYNAMICS?
Prepomax Forum could be the right place to ask.
Try packing it to .zip. If it doesn’t work, just use some hosting website like WeTransfer or more lasting one (Dropbox, Google Drive, OneDrive). On the PrePoMax forum you won’t be able to upload it directly as a new user either.
The only video tutorial for SSD procedure in PrePoMax is this one: https://youtu.be/dLkmF7UesgE?si=rXHWqlS_64PQ4itj
This procedure is still quite buggy in CalculiX so be careful with it.
https://askoh.com/misc/acceleratingBeam.pmx
zip is not allowed either.
The beam simulation runs. But I struggle to make it animate. The beam should accelerate upwards and stresses in the beam will occur.
Thanks.
Like this ?
It’s 5 times scaled deformation because true scale would be barely visible.
Looks promising. Thanks.
Expected answer: Beam should vibrate while accelerating upwards. When the transient vibrations die down the beam deformation should behave like beam pinned at one end and simply support at the other end and under uniform gravity. It is still accelerating upwards, but the deformation is steady.
Can STEADY STATE DYANMICS find the steady deformation without doing the transient calculations?
Indeed, deformation is very tiny compared to body motion. So, show stress changes instead.
My attempt with Dynamics
https://askoh.com/misc/acceleratingBeam.pmx
Here’s the file I also shared on the PrePoMax forum (let’s maybe stay on the CalculiX forum here to not duplicate posts):
As you can see, the biggest issue is the lack of boundary conditions.
But generally speaking, I’m not sure if SSD is a good choice for your purpose.
I am a novice to Calculix. Instead of me guessing how Calculix works, let me ask for good advice.
Given the acceleratingBeam problem, how can I find the stresses in the beam when transient vibrations die down?
The SSD analysis procedure is meant for that (steady-state vibrations following transient ones) but comes with some assumptions that might be provlematic in your case. Most importantly, the results are in frequency domain and assuming harmonic (sinusoidal) excitation. Thus, you always need to know the frequency range in which you want to evaluage the response. Moreover, the results are given in complex form (with imaginary components). Also, this procedure needs to be preceded by natural frequency extraction and a sufficient mode shape base must be obtained.
Then there are time domain procedures - modal dynamics (also preceded by frequency extraction and fully linear) and implicit/explicit nonlinear dynamics. They solve for transient vibrations and steady-state is achieved only after some time. But they are much more versatile and I would imagine they could make sense for use with MBD.
On the other hand, if there were angular acceleration loads for static analyses in CalculiX other than CENTRIF, this could be the way to go. For example, I know that SolidWorks Simulation can use the results of MBD in SolidWorks Motion by applying linear (gravity-like) and angular accelerations as body forces and remote forces and moments to joints. Inertia relief (also not available in CalculiX) is then used to stabilize the model. Perhaps we should look for other examples of such approaches in existing software.
1 Like
There is a way that solves this problem with Steady State Dynamics.
The idea is that, ideally, an harmonic load decomposition with frequency zero, would correspond to a load with infinite oscillatory period (constant value).
Ccx fails to find the HArmonic response for zero frequency but focusing in the very lower bound range (cycles/time), close to zero, the result agrees well with the other three methods.
*STEP
*FREQUENCY,STORAGE=YES
20,1E-8
*END STEP
*STEP
*STEADY STATE DYNAMICS, HARMONIC=YES
1E-2,1E-1,50,3
*CLOAD.....
That would add a fourth possible approach.
I get the feeling that this is a somewhat forced way of solving the problem, but it may serve as a sample of the current flexibility of ccx.
@Disla Are you solving acceleratingBeam.pmx?
Glad you know SolidWorks Simulation. That is what I want to implement in FreeCAD. It would be easy if Calculix can handle angular acceleration like Centrif. Any chance someone can implement angular acceleration inside Calculix? The current workaround is to apply a Grav proportional to R x Angular Acceleration for each element and perpendicular to the R vector to element.
Inertia Relief can be handled by removing the rigid body degrees of freedom. Node1 is fixed (3 constraints). Node2 must remain inline to the original Node1-Node2 line (2 constraints). Node3 must remain in-plane to the original Node1-Node2-Node3 plane (1 constraint). Can Calculix do that?
Thanks.
This would require modifying the source code written in Fortran: GitHub - Dhondtguido/CalculiX: This repository contains the source files of CalculiX, a three-dimensional Finite Element Program (www.calculix.de).
It’s not as easy as writing a user subroutine but dload.f in CalculiX is meant only for user-defined pressure loads, not for body forces (unlike in Abaqus). Guido is the most familiar with the ccx source code so I would ask him at least for a tip how to start (he’s quite busy as we are close to the next release of CalculiX though).
Inertia relief is implemented in SW Simulation and some other software (including Abaqus) as automatically applied (to the whole model) acceleration balancing the other loads: Inertial Relief - 2024 - SOLIDWORKS Help
NO. pmx file had many discrepancies with mine.
Different Density,
Dimensions 1000m instead of 1000mm…¿?
Insufficient meshing
Only one element per thickness in a bending problem.
Yesterday I did it with Prepomax and results were pretty much the same as Mecway.
That sounds more like the 3-2-1 method not inertia release.
Very interesting. Even Solidworks ignores angular acceleration.
“In the Simulation application, only the translational field is considered; any induced rotations are ignored.”
Please share your *.pmx.
Is there a tutorial for 1,2,3 method to remove 6 dof?
Thanks
Only for inertia relief. But transfer from SW Motion includes angular accelerations.
It’s typically called the 3-2-1 method. It only makes sense for self-balancing loads and is fully manual - based on the proper selection of supports.
Will code below prevent rigid body motion in accelerationBeam.pmx model in static analysis?
I expect force in Node 1 is 2000N. Correct?
** Applying Boundary Conditions to Node 1 (Fixing it)
*BOUNDARY
1, 1, 3, 0.0
1, 4, 6, 0.0
This will just block the 3 translations in one node (there are no rotational DOFs in nodes of solid elements). The model will still be able to rotate about it. Hence the 3-2-1 method is used to eliminate all RBMs.
Got it.
How to apply 3-2-1 method when the 3 nodes are not aligned to x,y,z directions?