Learning Forum

[ChelsyClaire0328]

Hi how can i make a lifting simulation in Ansys where the structure i want to analyze will show different step of rotation, my structure will have a sling wire at both ends, starting at horizontal position until it reach vertical position, i attach an image for easy understanding.

I have found a sample video in youtube showing how the structure will react when it rotates vertically

https://youtu.be/VkPAkY0lYxE

 

Thanks

[peteroznewman]

Hello ChelsyClaire,

I have inserted the image from your attachment because ANSYS Staff cannot open attachments.

• The video showed them using springs for the cables and you can do the same.


• Let the left spring be fixed to ground.


• You know the start and end points of the top of the right spring. Is the path between them a straight line?


• If so, I suggest you create an extra body to attach the right spring to.


• Under the connections folder, Insert a Translation Joint between Ground and the extra body.


• Edit the coordinate system under the Joint to point the X axis along the line from the start to the end point.


• Add a Joint Load, Displacement, using the distance between the start and end points.


• Under Analysis Settings, turn on Large Deflection, turn on Auto Time Stepping.


• Set the Initial, Minimum and Maximum Substeps to 100.


• The model will have an Inertial load of Standard Earth Gravity.


• Make this a two step analysis, where step 1, the Joint Displacement is zero, but the springs stretch due to gravity.


• In step 2, the Joint Displacement occurs.

If the endpoints are in the XY plane, you might add a Displacement BC of Z=0 to make the solution easier to compute.

 

[ChelsyClaire0328]

Hi Peter,

Can i do this under static structural?

If so, I suggest you create an extra body to attach the right spring to. <<<<<<<<<<< The extra body that i will create will be at the right top position on step 1?

Under the connections folder, Insert a Translation Joint between Ground and the extra body. <<<<< The ground will be the right top position of step 3?

in step 1?

 

[peteroznewman]

Hi Claire,

Yes, the extra body will be at the top of the spring and will travel along the dotted line.

[ChelsyClaire0328]

Hi Peter,

Is the arrangement going to be like this?

Do i need to add only 1 extra body? which to be located at the initial positon of the right hook

Then the last point will be the reference coordinate system point for Translational joint?

 

[peteroznewman]

Yes, but the X axis of the Joint Coordinate System is the translation axis, so you have to use the fields in the Detail window to orient the X axis to be parallel with the dotted line.

[peteroznewman]

Hi Claire,

Here is an idea, put the coordinate system at the center of the orange circle with Z pointing out of the screen. Change the Translational Joint to a Revolute Joint.  The Load then becomes a rotation that takes the end of the spring along an arc. This will behave like a four-bar mechanism and will keep the tension in the springs much more even during the move.

Regards,
Peter