 ## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

• freud farid
Subscriber

my problem is a cantilever curved beam under follower load (as mention in the image ) i follow all steps to apply a follower load but without result
i create a new coordinate system and use it to create a remote point on the second free end of the curved beam
then i linstall an extension named 'follower load ' and use it
always give me this error message "The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information."
"The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.

• peteroznewman
Subscriber

From your original discussion, I created a model using Beam elements. Here is the link to that model.  You should use Beam elements.

The image you show above will be meshed with solid elements which are not recommended for this type of problem.

• freud farid
Subscriber

thank you very much peteroznewman

it's very useful and give acceptable result
i have some question about the project

1- when i change the material to a hyperelastic it give error , i know that the geometry is line and l must to convert it ot area or solid  in order  to work with hyperelastic material

how i can convert the geometry to solid without creat  geometry from the begining

2- when i change the direction of applied the load (from y to x ) or the apply a moment it give error ? where is the problem

3- how i can extract the nodal coordinate of the deformed shape , i mean that (x,y) coordinate of the nodes in the deformation configuration

thank you again

• peteroznewman
Subscriber
1. The Mooney-Rivlin Hyperelastic material model supports Beam elements, you don’t need a solid body and solid elements. You may not have created the hyperelastic material correctly. What is the error?
2. When you change the load direction, what is the error?
3. Create a Directional Deformation for the X axis and a second Directional Deformation for the Y axis. Export the nodal deformations for these two axes.  You also need the initial X,Y coordinates of all the nodes. The final X, Y coordinates of each node is the initial X, Y coordinate of the node plus the X and Y directional deformation added to the initial nodal coordinates.
• freud farid
Subscriber

when i open the file this warning appear the error message when i change the material to mooney rivlin

"An unknown error occurred during solution.  Check the Solver Output on the Solution Information object for possible causes."

another error message appear

"The unit system of Command object(s) such as  Static Structural>Commands (APDL) at the time of creation, differs from the solver unit system.  Check your data and results accordingly."

• peteroznewman
Subscriber

You have two warnings and one error. The first warning, just follow the instructions provided.

The error is because you don't have the mooney rivlin material model properly defined.  You may find evidence of this in the Solution Output.

The last warning is because you have an APDL command and you are not solving in the same units as were used when the APDL command was inserted. This is a problem when you have numbers in the APDL command that need to change when the units change such as a spring stiffness.  This warning is not a problem when all the numbers in the APDL command are dimensionless, such as Keyops.

• freud farid
Subscriber

i try all the hyperelastic material but alwaus give errorr

but when i try another elastic material it work ?

i think the problem is in the element choice !?

can you explain more this point ,

1. Create a Directional Deformation for the X axis and a second Directional Deformation for the Y axis. Export the nodal deformations for these two axes.  You also need the initial X,Y coordinates of all the nodes. The final X, Y coordinates of each node is the initial X, Y coordinate of the node plus the X and Y directional deformation added to the initial nodal coordinates.

please can you make video like tutorial and explain how to create the example

• peteroznewman
Subscriber

Create a solid model of a straight cantilever beam, meshed with solid elements and assign the hyperelastic material, do you get the same error?  If so, you have not correctly defined the hyperelastic material model.

I will see if I can find some time to explain more on the point of exporting two directional deformations and adding them to the nodal coordinates, but I have limited time. Have you tried exporting a directional deformation?

• freud farid
Subscriber

yes i create 02 deformaton x , y  and i export the nodal deformations for these two axes from the result summary

• peteroznewman
Subscriber

Read this discussion, it tells you what to do.

Where it says to export to text file, right click on the result and the popup menu has Export on it.

• peteroznewman
Subscriber

Ansys can create all the data needed to make the plot shown in matlab by implementing 24 equal load steps and exporting the data from each load step. It would be a bit tedious to do that manually. If you want to learn to code, I expect you can automate the process of extracting the data with a script.

The matlab example shows a force that is tangent to the tip, which would be vertical at the start of the simulation.  You are showing a horizontal force. Are you trying to get the matlab plot with a horizontal force? That is not the same problem.

• freud farid
Subscriber

the first photo is the matlab plot of the vertical force load (y direction ) , i ask if can we plot the same figure with ansys ?

the second photo for another example with a force in x direction , i try to change the direction of the force but it give an error , i ask if you can do it with x force direction and show me the result ?

• freud farid
Subscriber

hi

i use a newhookean hyperelastic material , the geometry is solid instead line

i apply the follower load but not converge ?  please check it and fixed it ?

• peteroznewman
Subscriber

Ansys can't plot a figure like that. Ansys can provide all the data needed to plot a figure like that in a program that is good at plotting such as Excel or Matlab.

You put this file: hyper_follower_load.wbpj in dropbox.  That file is useless without the hyper_follower_load_files folder.  Open the file in Workbench and use File Archive to create a hyper_follower_load.wbpz file instead, which contains all the files needed for me to open.

• freud farid
Subscriber

i modified the previous link , and this is the link again

• freud farid
Subscriber

hi peter any new ?

• peteroznewman
Subscriber

Hi Freud, Your beam is very thin in the plane of the arc, but thick in the radial direction. That means when you apply a force in the -X direction, the beam will buckle.  Buckling is a difficult behavior to capture in a Static Structural model. It is very difficult to capture when the load is a force and it is much easier to capture when the load is a displacement.

If you change the profile of your beam so it is thick in the plane of the arc and thin in the radial direction, then the part will not buckle and you may find it much easier to converge.

• freud farid
Subscriber

freud1889@yahoo.com

• peteroznewman
Subscriber

How will that help?

• freud farid
Subscriber

as you like !!

for the same our previous example , did you try the load in x direction instead y direction? can

try it and share the result ?

• peteroznewman
Subscriber

The buckling problem is the same whether you push in the X or the Y direction. The arc will buckle out of plane at a very low force.  I created a linear material to run two Eigenvalue Buckling analyses to find out the Load multiplier for X or Y direction loads when the upstream Static Structural model has a 0.0001 N unit load.  The load multiplier is 0.997 for a load in the Y direction and 0.852 or a load in the X direction.

https://jmp.sh/b6vPT8Yi

• freud farid
Subscriber

thank you any way , but not helped and not give the correct results

• peteroznewman
Subscriber

You can easily convert this model from 3D to 2D by simply setting a Frictionless Support on one face. That will prevent out-of-plane buckling and force the model to deform in the plane.   