# How to apply connecting stiffness using spring in circumferential direction

• 359 Views
• Last Post 25 February 2019
• Topic Is Solved
Devaiah posted this 08 December 2018

Hi,

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?

Thank you.

Attached Files

peteroznewman posted this 08 December 2018

Hi Devaiah,

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.

Regards,
Peter

Devaiah posted this 08 December 2018

Hi Peter,

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 In the paper, the bolts have been replaced by springs with stiffness as mentioned earlier.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.

Regards,

Devaiah

peteroznewman posted this 08 December 2018

Hi Devaiah,

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.

Regards,
Peter

• Liked by
Devaiah posted this 10 December 2018

Hi Peter,

Thank you for the suggestions.

Regards,

Devaiah

peteroznewman posted this 10 December 2018

Hi Devaiah,

Regards,
Peter

mahmoud14 posted this 25 February 2019

Hi Peter,
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?
Many thanks,
Mahmoud

Attached Files

jj77 posted this 25 February 2019

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.

Normally one applies a pre load/stress, that keeps the supports where they are. In order to do that the only reasonable way is to apply a bolt preload, that works fine, and applies the pre tension say on the beam, something that should increase the freq. of say the bending modes.

Attached Files

• Liked by