# How define tow (cable, rope ....) for elevator machine in ansys workbench?

• 741 Views
• Last Post 02 July 2018
• Topic Is Solved
Vladimir posted this 01 July 2018

Good day. Can anyone tell me how define tow (cable, rope ...) for elevator machine ? Thanks.

peteroznewman posted this 01 July 2018

It depends on what types behavior you want to simulate with the cable in the model.  For example, if the spring rate of the cable is all that you care about, then you can use a spring element between the top pulley and the elevator car. Then the static and dynamic vertical position or motion of the car will include the flexibility of the cable.

If you want to include the mass of the cable and its lateral vibrations, then you could define beam elements.

Regards,

Peter

• Liked by
sk_cheah posted this 01 July 2018

For tension only cables, take a look at LINK180

Kind regards,
Jason

• Liked by
Vladimir posted this 01 July 2018

It depends on what types behavior you want to simulate with the cable in the model.  For example, if the spring rate of the cable is all that you care about, then you can use a spring element between the top pulley and the elevator car. Then the static and dynamic vertical position or motion of the car will include the flexibility of the cable.

If you want to include the mass of the cable and its lateral vibrations, then you could define beam elements.

Regards,

Peter, i need to calculate stress in cable

Vladimir posted this 01 July 2018

For tension only cables, take a look at LINK180

Kind regards,
Jason

Thanks but how use this element in  ansys workbench ?

peteroznewman posted this 01 July 2018

Cables are multi-strand assemblies and so the distribution of stress among all the strands is very complex. Cable manufacturers specify a safe load for using a cable, which is in terms of force as well as a minimum breaking strength, also in terms of force. Refer to the table on this page.

When you use a spring element in Workbench, you can insert a Probe and recover the force in the spring once the system is solved.

Jason suggested a LINK180.  [Edit: see my next post for images from Jason's example]

One advantage of using a LINK180 is that by specifying the cross-sectional area of the link and the material (which has a density property) for the link, your simulation can automatically include the weight of the cable. If you use the spring element and you want to include the weight of the cable, you will need to add a point mass to the elevator car and calculate the weight by using the length and multiplying by the last column in the table for Wire Rope.  Note that the area you specify must be calculated from the last column in the table by dividing by the material density. That way ANSYS will calculate the same value for the same length that you would calculate by hand.

The LINK180 also has a FORCE output which is shown in my next note.

Regards,

Peter

Attached is an ANSYS 18.2 archive of a small model to figure out how to get a LINK180 to work. It needs a material and cross-sectional area defined.

Attached Files

• Liked by
sk_cheah posted this 02 July 2018

Kind regards,
Jason

• Liked by
peteroznewman posted this 02 July 2018

Below are snaps from Jason's example of using LINK180.
I see it starts as a line body in DesignModeler (or a Beam in SpaceClaim).

Then the force in the link is easily extracted in the results.

Thanks Jason!

Note: Jason's example was done in ANSYS 19.0

• Liked by