Learning Forum

[unknown123456789]

Hello guys,

I've got a tube composed of composite material that consists of a stainless steel coil covered by two layers of identical TPU (both from inner and outer diameter), in which the material properties of the TPU is to be determined.

The idea is to temporarily substitute material properties of the softest generic TPU found on the MatWeb, make an identical real-life and simulation setup to measure the deflection of the tube under a given loading, and then fine-tune the forementioned TPU material properties until the results from both scenarios agree with each other.

It should be noted that the tube itself is straight but is (and will be) bent and fixed at both ends in each scenario, because it is rather soft and will deflect by a lot even with minimal loading. By pre-bending the tube we should be able to make it stiffer and get more repeatable result.

It should also be noted that there is a small cut-out at the middle of outer TPU layer from the top, in which 10 MPa of pressure is applied on a 4 mm² face, which implys that the tube is subjected to a 40 N load. However, the result shows that the maximum deflection is about 8 mm occured at the middle, which deemed unreasonable for such a soft structure even after taking the pre-bending and coil reinforcement into account. So I wonder if there are settings that I have overlooked, or if I have made some wrong settings in the first place.

I have also attached a link to my .wbpz file below. Any help would be greatly appreciated.

https://drive.google.com/file/d/1gYPHAEO7mEnMIQ7DkQB9EVe-BlpLJN-W/view?usp=sharing

Thanks,

Patrick

[Ashish Khemka]

Hi Patrick,

Looking into the model might be out of scope for Ansys Employees. Can you please share the snapshots? Did you turn on the large deflection? Also, check the contact status befor and after the solution if the bodies are behaving as expected.

Regards,

Ashish Khemka

[unknown123456789]

Hi Ashish,

I have encountered the same error message that Peter mentioned when uploading my screenshot. Could you suggest an in-scope alternative for you as an Ansys employee for a better understanding of the setup?

Also "Large Deflection" has already been turned on in the setup, but could you tell me more about how to check the contact status?

Regards,

Patrick

[peteroznewman]

Hi Patrick,

 

I'm not an Ansys Employee, so I can open your model. I noticed that you are using Ansys 19.0 which is many years older than the current version. Using the current version may help get a better result. Looking at your model, I see the three solid bodies meshed with quadratic solid elements. Because the bodies are very thin compared to the other dimensions, solid elements are not ideal.

Looking at the steel coil, it has only one element through the thickness. Two elements through the thickness is the minimum to get accurate bending results.

 

Looking at the inner layer, it also has one element through the thickness. The smaller elements of the inner layer follow the curvature better than the larger elements on the coil. While the nodes of all bodies are on the geometric surface, you can see the faces of the coil buried in the inner layer. It would be better if the elements were closer to being equal in size. The outer layer also has only one element through the thickness.

  

Because of the difference in element size between the large elements on the coil and the smaller elements on the tubes, the bonded contact will not be as accurate as possible.

I see you imported a STEP file to mesh these solid bodies. One way to get a better mesh is to import the geometry into DesignModeler or SpaceClaim and use the Shared Topology that is available in those systems. That will cause the meshes to be perfectly matched and connected at the shared faces then no bonded contact will be needed.

 

I see this website has "Failed to upload image with an HTTP Error: 504". I hope they fix that soon.

 

Another potential area of improvement is in the choice of the material model. The tubes are defined with Linear Isotropic Elasticity, but a Hyperelastic material model may give more accurate results. However, you will need to obtain the material constants for that model before you can use it.

 

Regards,

Peter

[unknown123456789]

Hi Peter,

Your recommendation seems legit to me, and I will definitely look into it!

However, since I am new to Ansys, would you tell me more about your recommended mesh setting over quadratic solid elements?

Regards,

Patrick