Unexpected results from ANSYS workbench

In summary, if you want to deform the muscle layer you will need to increase the Young's modulus of the top layer.
  • #1
Akarsh
6
0
Hi,
I have problem of finding the deformation of skin using a probe. I have identified the different layers of skin and made the model accordingly along with a probe in contact with the top layer of skin. The model is basically 15x15mm model with extrudes of different thickness for each layer.
The layers are stratum corneum, epidermis, dermis, hypodermis and muscle respectively. Each layer has different mechanical properties and is given isotropic elasticity condition.
The force of 0.1N is given to the probe and the bottom and the sides of the skin model are given fixed support condition.
The deformation in the first four layers are acceptable but the muscle layer acts like a cube of immense stiffness in a sense that no stress, no deformation, no strain occurs in the muscle layer. I cannot seem to identify the cause of this problem and i need some HELP figuring this out!

PS: I have attached the picture of the model, the sectional view of the results and the material properties of each layer
The model was created on SOLIDWORKS 2015
 

Attachments

  • Entire model with 5 layers and 1 probe.PNG
    Entire model with 5 layers and 1 probe.PNG
    17.9 KB · Views: 755
  • Layers of skin.PNG
    Layers of skin.PNG
    12.6 KB · Views: 656
  • Normal strain (Y-axis).PNG
    Normal strain (Y-axis).PNG
    40.6 KB · Views: 861
  • Sectional view of deformation.PNG
    Sectional view of deformation.PNG
    27.3 KB · Views: 1,277
  • Material properties.PNG
    Material properties.PNG
    10.5 KB · Views: 717
Engineering news on Phys.org
  • #2
I notice that your top layer has a modulus that is two orders of magnitude or more above that of any of the lower layers. So I am wondering if the composite restraining force at the tensile stress of primarily that layer plus the two underlying layers with all edges constrained is sufficient to resist any more deflection of the probe from its penetration point without requiring any support from the muscle layer.

I would suggest that you do a simple diaphragm analysis without the bottom restraint on the muscle and a similar diaphragm analysis without the muscle layer to see the results of those two cases.
 
  • #3
With regard to the above, increasing the area of your model beyond the current 15x15 mm size will reduce the tensile restraining effect of your peripheral edge restraint on the relatively high modulus top layer.

Also a test you could perform on your model would be to temporarily remove the top three layers and place a test point load on only that remaining muscle layer to see how it responds in order to determine if there is some basic issue with its modeling or meshing.
 
  • Like
Likes Akarsh
  • #4
@JBA i tried doing the same analysis without the muscle layer and keeping the bottom of the hypodermis layer fixed. I got the similar results except that there is no muscle layer in the results.
PS in this result i did not add the friction between the skin and the probe. If i did add it then i would i get the same result as the one's i initially posted
 

Attachments

  • Deformation.PNG
    Deformation.PNG
    40.6 KB · Views: 598
  • #5
From what I see comparing the results, it would appear that the diaphragm tension in the top (and to some degree, the second layer) is the controlling factor due to its high modulus. The modulus in the third and fourth layers is so low that they are almost fluid in their behavior.

To test if this is true, rerun the problem with a reduced modulus (possibly 300) for the top layer, that will transfer more of the loading to the supporting underlying layers and to the muscle layer. If it is true, you should see a deeper probe penetration and some deflection of the muscle layer.
 
  • Like
Likes Akarsh
  • #6
@JBA i removed the top layers and placed the probe on the muscle layer and saw whether it would deform or not.
It did deform and caused some normal stress
I know the mesh is not refined properly as i just wanted to see whether i could get any deformation for the muscle layer
 

Attachments

  • normal stress.PNG
    normal stress.PNG
    33.9 KB · Views: 631
  • Deformation1.PNG
    Deformation1.PNG
    38.5 KB · Views: 589
  • #7
@JBA i changed the young's modulus of the top layer to 30MPa and ran the simulation,
The results were that there was more deflection in the model but the muscle layer was still not deformed at all

I tried changing the young's modulus of the muscle layer to a value lower than the hypodermis (the layer prior to the muscle layer). The results from this trial shows deformation in the muscle layer
 
  • #8
Looking at your initial strain diagram you can see that as the loading progresses down through the layers the strain area is also expanding and therefore as this area of pressure is expanded it reaches the point that the area is so large and evenly distributed that it is deforming the entire surface only a minuscule amount.

If you look at that initial strain display values chart you will see -00248... is the minimum negative strain value given and .00193... is the minimum positive strain value given and there is no distinguishable color variation in the color band between those two values. As result, if the strain across the surface of the muscle layer lies in the zone between those values, it is not discernible even if it is not actually 0.000.

Considering all of the above, it would appear that is the most probable answer to what you have perceived to be a problem, that does not actually exist, in your analysis.
 
  • Like
Likes Akarsh
  • #9
Thanks for your help @JBA.
Really appreciate it
 
  • #10
So when the force is applied through a series of other layers the strain would be lesser?
 
  • #11
As a test of my theory I ran the below simple strain calculation for your .1 N force distributed over the 15x15 mm surface area of the muscle material (think of it as a the end of a square bar of your muscle material) and the results compared with the below copy of your original strain diagram with a solid color strain range from + .0019 to - .0092 tend to confirm that a similar distributed loading on you muscle area might fall between those two boundaries. (please forgive the units conversions, I am simply more confident using USA units)
upload_2016-12-11_23-50-25.png

upload_2016-12-11_23-57-7.png
 
Last edited:
  • #12
In response to your last question, It is the extreme softness of the third and forth layers that causes them to act like a fluid trapped between the top two layers and the bottom muscle layer and spread the probe load across almost the entire surface of the muscle layer that results in that layer's very small, but not zero, deflection.

If you look carefully at the above strain plot you will see that the horizontal grid line between the fourth layer and the muscle layer is not actually flat, it has one negative offset just inside the second grid line from the outside end on both ends; and second negative offset just outside of each vertical grid line next to the centerline that indicate a small but present strain in the top surface of the muscle layer.
 
  • Like
Likes Akarsh

Related to Unexpected results from ANSYS workbench

1. Why am I getting unexpected results from my ANSYS Workbench simulation?

There are several reasons why you may be getting unexpected results from your ANSYS Workbench simulation. Some possible reasons include incorrect boundary conditions, mesh errors, or convergence issues. It is important to carefully review your simulation setup and troubleshoot any potential errors.

2. How do I troubleshoot unexpected results in ANSYS Workbench?

To troubleshoot unexpected results in ANSYS Workbench, you can start by checking for any errors in your simulation setup, such as incorrect boundary conditions or mesh errors. You can also try refining your mesh or adjusting convergence settings to improve the accuracy of your results. Additionally, checking for any physical or numerical assumptions in your simulation can help identify potential issues.

3. Can software or hardware limitations cause unexpected results in ANSYS Workbench?

Yes, software or hardware limitations can sometimes cause unexpected results in ANSYS Workbench. This can occur if your computer does not meet the minimum system requirements for running ANSYS, or if you are using an outdated version of the software. It is important to ensure that your computer is capable of running ANSYS and that you are using the most up-to-date version.

4. How can I improve the accuracy of my ANSYS Workbench simulation results?

To improve the accuracy of your ANSYS Workbench simulation results, you can try refining your mesh, using a higher-order element type, or adjusting convergence settings. It is also important to carefully review your simulation setup and ensure that all physical and numerical assumptions are accurate. Additionally, using experimental data or performing a sensitivity analysis can help validate your results and improve accuracy.

5. What resources are available for troubleshooting unexpected results in ANSYS Workbench?

There are several resources available for troubleshooting unexpected results in ANSYS Workbench. The ANSYS Help documentation provides detailed information on simulation setup and troubleshooting. The ANSYS customer support team is also available to assist with any technical issues. Additionally, there are many online forums and communities where users can ask questions and receive support from other ANSYS users.

Similar threads

  • Mechanical Engineering
Replies
5
Views
3K
Replies
1
Views
6K
  • Mechanical Engineering
Replies
3
Views
3K
Replies
6
Views
30K
  • Mechanical Engineering
Replies
1
Views
3K
  • Sci-Fi Writing and World Building
Replies
21
Views
1K
Replies
9
Views
3K
  • Beyond the Standard Models
Replies
2
Views
3K
  • Computing and Technology
Replies
19
Views
13K
Back
Top