MEASURING ROTATION IN ANSYS MECHANICAL APPLICATION (workbench)

mauryamaurya indiaMember

hello sir 

             i required rotation of one body wrt to other body. 

first example i solved by reading some commands from internet.single body

this is single body fixed at bottom and moment of 1000 Nm at top.

For finding rotation commands are used for remote points and second command in solution.

command

measure_pilot=_npilot

 

and in solution

my_rotx=ROTX(measure_Pilot)*57.29

my_roty=ROTY(measure_Pilot)*57.29

my_rotz=ROTZ(measure_Pilot)*57.29

 

the results are:results

but if you calculate it by formulae: rotz is 4.01 correct by 16*t/G*j

question when i am using two or more bodies:

new geometry with two body

it is same as above with one more body body above that is placed having frictional contact with mue=0.8

I want rotational angle of lower body top outer edge and top body outer edge.

provide the command twice for two remote points.

command

two command are there but in solution how i will come to know for which body rotation is mentioned.

in this case i am getting same 4.015.

Comments

  • peteroznewmanpeteroznewman Member
    edited April 2018

    Here is a very simple way to apply a rotation and measure the torque. Use a remote displacement. The input is the rotation of 1 degree, the result is the moment required to rotate that face by that angle.

    If you want to apply a moment and measure the rotation, create a Remote Point on the face and insert a result called a Flexible Rotation Probe. Below I applied a Moment of 25937 Nmm and I measured a 1 degree rotation. No code required.

     

  • mauryamaurya indiaMember
    edited April 2018

    hello sir

                please send me the archieve file of this simulation.

    My main aim is to find rotation of each vertebrae wrt to fixed vertebrae in my lumbar bone model for which you created the spaceclaim tutorial.

    first i always try with simplify model to verify results. This seem absurd to you but without verifying the results it always doubt.

    L1(top most ) wrt to L5(bottom one) 

    L2 wrt to L5

     

    image

    image just to remind the vertebrae

    thank you

  • peteroznewmanpeteroznewman Member
    edited April 2018

    Attached file is an ANSYS 18.2 archive of the Moment and Flexible Rotation Probe.

  • MohankumarMohankumar Member
    edited August 2018

    Hello Mr. Peteroznewman,

    I have the same problem as well. Need to find the degree of rotation between two vertebrae. I am using Ansys 17.0. I don't find the 'Flexible rotation probe' option in solution. Please help.

     

    Thank you.

    Probe

  • peteroznewmanpeteroznewman Member
    edited August 2018

    Hello Mohankumar,

    That result was added after 17.0

    You will have to output the x,y, z undeformed nodal coordinates and the x, y, z deformation of a few nodes, spread out across the surface, then compute the rotation of that set of nodes using equations. Since it may not be rigid body rotation of the nodes, your equations will have to include a best-fit algorithm.

    Perhaps other members can suggest an APDL command that does this, even though the functionality was not exposed in the Mechanical menu system at version 17.0.

    Regards,

    Peter

  • akhemkaakhemka Forum Coordinator
    edited October 2018

    One may add a general joint and then probe a joint rotation as well.

     

    Regards,

    Ashish Khemka

  • peteroznewmanpeteroznewman Member
    edited May 17

    ahmadraza, please copy the content of your post and paste it into a New Discussion, then delete the post above.

    It is better for you to have your own discussion since you will get notified when someone posts a reply.

Sign In or Register to comment.