Learning Forum

[1234mamanunu]

Hello to all,

I am fairly new to Ansys and would like to model a foot having an axial load of 300N (~half the body height of someone with 60 kg) standing on a floor. The goal is to get the load distribution of the floor.  For this, I am used the static structural model and applied a structural steel to floor and a custom isotropic material with E=1.45E6 Pa, v= 0.49 and rho of 1060 kg/m3.

I have the mesh generated [image bellow]. Its rough because of the student license simulation limitation.

I have set the force boundary condition on the foot top patch along the -y axis

 

and set the bottom of the floor to fixedSupport

 

My doubt is regarding the contact between the foot and the floor. If I set it to bonded I get the reaction on the floor, however I do not know if this is the correct setup.

If I try do apply a frictionless or friction contact the simulation will not complete and report a an internal error:

*error solution magnitude limit was exceeded. Please check the environment for inappropriate load values or insufficient supports.

Is the bonded condition sufficient to solve this? How can I make the other types of contact work?

 

Best Regards

[peteroznewman]

Hello,

When making contact between a soft object and a much harder object (Young's modulus ratio > 1000), you can save time by making the hard object a rigid body. You can't use Fixed Support on a rigid body. You have to use a Fixed Joint to ground.

Don't use Bonded Contact, use Frictional Contact. This requires more work to have the solver converge. You have to check that the contact is closed and you should use automatic time stepping with Initial and Minimum Substeps set to 100. You must also turn on Large Deflection.

Here is one measured pressure map of a foot.

That pressure map is highly dependent on the bones in the foot.

If you only have the outside shape of a foot, and fill the volume entirely with a very soft elastomer, you will not get the foot pressure map shown.

If you want to get a better simulation of the foot pressure map, you need to put some bones inside the elastomer.

Here is a website about drawing the bones of the foot in CAD.

[1234mamanunu]

Thank you very much for the reply

 

What is understood as a closed contact?

 

If possible I would like to model the case with the fixed support boundary condition

 

 

Best Regard

[peteroznewman]

Add a Contact Tool under the Connections Folder and Generate Initial Contact Status. Open the result and you will see a table for each contact pair and the status can be Open, Closed or Near.

A Fixed Joint holding a Rigid body is the same as a Fixed Support boundary condition, except you don't need as many nodes and elements so it solves faster.

[1234mamanunu]

 

The status is Near Open. Is there a tool to close the contact?

 

[1234mamanunu]

I went into Connections -->Contact and in my contact patch I set the Geometrical modification option to Adjust to Touch.
It appears to have closed the contact.

 

However, I am still getting the same mistake

 

Am I missing something?

 

solver:

 

boundaries:

Contact

 

[peteroznewman]

It could be that the foot is unstable and will tip over with any applied force on that face.  Delete the Force. 

Create a Remote Displacement on that face and set X and Z to 0 and Y to -5 mm and set all Rotations to 0.

In the Solution branch, insert a Probe on the Reaction force of the Remote Displacement. Solve. You will get a plot and Tabular Data of 100 points of Force vs Time. Look for the time when 300 N is reached.  You can right mouse click on the row that is closest to 300 N and Retrieve that result. Insert a Contact Tool into the Solution branch. Insert a Pressure result into the Contact Tool. You can look at the Pressure plot at that time.

[saifali]

Hello is it possible to share the drawing    

s96aif@gmail.com

 

[1234mamanunu]

It's available on grabCad

https://grabcad.com/library/foot-surfaces-to-solid-1

 

Best Regards

[Ashuverma]

I am also facing the same problem. I am trying to simulate the process in Explict Dynamics to test different footrests. Plz, send me your mail ID so I may send you the complete case file.

[Ashuverma]

 Sir, I am also facing the same problem with ANSYS explict Dynamics. I am trying to optimize the design parameters and design for footrest. Please see the complete case file for your reference. My mail id    ashutosh.verma2307@gmail.com