December 8, 2018 at 4:38 amDevaiahSubscriber
I'm performing a modal analysis on two cylindrical structures(shells) connected to each-other by springs.
The spring must have stiffness in all the 3 coordinate system directions and a rotational spring .
I was able to provide body-body contact for the longitudinal direction and Body-ground condition individually to the two shells for the transverse direction. I was able to change the definition to torsional to simulate the rotational spring.
However, I'm unsure on how I must provide spring stiffness to simulate connecting stiffness in the circumferential direction.
Is there any way of providing it?
December 8, 2018 at 2:38 pmpeteroznewmanSubscriber
What physically connects the two cylindrical structures to each other (and to ground) and why don't you model that directly? Then you would delete all these springs, which are just an approximation anyway.
To answer your question: if you create a series of short springs that are aligned with the tangent to the circumference, you would have stiffness in the circumferential direction. I suggest a minimum of four springs at each of four points around the circle.
December 8, 2018 at 5:30 pmDevaiahSubscriber
Physically the two structures are connected by bolts.
I'm trying to work on a research paper where two cylindrical shells(surfaces) have been connected to each other by bolts. In the paper, the bolts have been replaced by springs with stiffness as mentioned earlier.
The work was carried out in APDL and I was finding it difficult to implement the same in WB.
Thank you for the answer. Let me try to incorporate the method you've specified in my model.
December 8, 2018 at 5:50 pmpeteroznewmanSubscriber
I recommend you add the bolt holes in the two cylindrical shells. Then you have the quick and simple approach or the complex and detailed approach.
Quick and Simple
RMB on the Connections Folder, Insert > Beam.
One bolt hole edge is assigned to the Reference Scope, the other is Scoped to the Mobile side. You then define the bolt shaft diameter and material. If you want the bolt a bit longer than the distance between the two circular edges that represent the bolt holes in the midsurface of the flange, you can override the coordinates that get filled out when you select the circles.
Complex and Detailed
In addition to creating the holes, you also have to model a bolt with solid geometry to represent the Head, Shank and Nut. Then you define frictional contact between the head and the flange on one side, and the nut and flange of the other side, and also frictional contact between the flanges. You can also define a bolt pretension to squeeze the flanges together. You also might want contact between the bolt shank and the hole edges to support torques in case the frictional force at the flange is overcome.
December 10, 2018 at 2:23 amDevaiahSubscriber
Thank you for the suggestions.
December 10, 2018 at 3:51 ampeteroznewmanSubscriber
If my post above answered your question, please click the Is Solution link below that post to close this discussion.
February 25, 2019 at 3:30 ammahmoud14Subscriber
I am doing a pre-stressed Modal analysis in ansys workbench. I have a column and used torsional spring at the top and bottom of the column, and a nodal force on the top. But when I am performing an analysis, the force increasing or decreasing , has no effects on my vibration.
Could you please let me know bout the semi-rigid support by torsional spring, modeling, How it would be? and why my force has not being taking account in my analysis?
February 25, 2019 at 10:00 amjj77Subscriber
I think Peter is on a well deserved vacation, so I will try and answer.
The revolute joint is blocking all dof except of the rotation (RZ), thus the applied force is cancelled out, thus not doing anything (by the dof restrains).
You could see this by plotting the displacements for the static analysis, and you will not see much going on.
Not sure how to overcome this - the only way I can think of is to model the springs at the end explicitly (just add two small line bodies at the end of the beam), restrain (extra line bodies that will be springs) them fully at their ends, apply force on the end of the beam, restrain the opposite beam end as needed, and on the same end as the force of course (not though the dof that is in the force direction of course), and that works. These two end line bodies are also converted to combin14 3D torsional spring elements. More details (including commands snippets) can be seen in the attached.
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- How to calculate the residual stress on a coating by Vickers indentation?
- Errors – Reinforced Concrete Beam
- Solver Pivot Warning in Beam Element Model
- An Unknown error occurred during solution. Check the Solver Output…..
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Large deflection
- Colors and Mesh Display