Learning Forum

[Dorian Tapia]

Hello community, I hope you are all doing well. My problem is that I'm trying to design a CFM resembling a gripper in static structural using TPU95A as the material. So far, I've tried activating large deflection, setting initial and minimum substeps to 100, and maximum substeps to 1000. I used Keyopt(6)==1 and Keyopt(2)==1. Additionally, I sized my mesh to 1.6mm, which I think is decent. I tried all these things because TPU95A is an elastomer; nevertheless, deformation results are still linear instead of nonlinear. What can I try now? Has anyone designed a CFM in ANSYS before?

PD: Sorry for my bad english.

[peteroznewman]

Hello Dorian, please insert an image from the Engineering Data page of Workbench showing the TPU95A material in your reply. Do you have a hyperelastic material model in that material? Please insert an image of your gripper and describe the loads and boundary conditions.

[Dorian Tapia]

Thanks for your reply, here is an image of the TPU95A properties, also I don´t think it's a hyperelastic material model since I just realized nonlinear behavior is off as seen in the next image:

For my gripper, red arrows indicate where there are fixed supports. There´s also a yellow arrow that indicates a displacement in the 'x' axis.

And I increase that displacement one by one (mm) analyzing how it influences the force at the tip of the gripper, like showed in this image:

Again, thanks for your help :)

[peteroznewman]

Is this model 2D or 3D?  It’s hard to tell from the image. If the CFM is an extrusion and that profile is extruded to a depth longer than the width of the part in the image, then it is reasonable to create a 2D Plane Strain model which would reduce the time the solution takes to compute.

The mesh is too coarse. Change the default element size so that there are at least 4 elements through the thickness of the thin walled arms.

The material is linear elastic, which will behave differently than a hyperelastic material. Look for stress-strain data for TPU95A. If you have the resources, obtain samples of that material and perform the material testing to produce the stress-strain data for that material. Ideally, several types of testing is performed such as Uniaxial, Biaxial and another test. Then coefficients for a material model are fit to the test data. how-to-perform-curve-fitting-for-hyperelastic-material-models

The fixed boundary condition on the vertex of the tip of the mechanism should be replaced with a more realistic boundary condition. In reality, it is not possible to hold a vertex. Change the geometry to the real shape of that constraint.

What is the real mechanism that creates the displacement?  Is the TPU95A material bonded to a flat metalic actuator?  Or does the real mechanism push on that face and the face is free to slide on the tip of the actuator?  The deformation will be more realistic if you add the actuator tip into the model and use Frictional Contact between the actuator tip and the inner faces of the gripper.

[Dorian Tapia]

It´s a 3D model, 4mm thick and that´s where one of the fixed supports is.

 I'll make the changes you suggest to my mesh and look for the stress-strain data you mentioned. As for the mechanism that produces the displacement is another besides the gripper, wich is in contact with the gripper through the fixed support shown above, so I guess I'll also add it to the simulation.

Thanks for your patience and support, you've really been helpful.