Learning Forum

[Matthew Pirkle]

When using the command:

PLNSOL,PDMG,MT                     !(Plot nodal solution for progressive damage, matrix tension failure mode)

what do the numbers in the color scale at the bottom of the screen represent? Are these the failure index? Please see attached. 

 

Thank you!

[Wenlong]

Hi,

So MT is the damage variable (Ref: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_cmd/Hlp_C_PLNSOL.html%23plnsol.tab.fn9) Typically, a damage variable has a value between 0 and 1, in which 0 means undamaged and 1 means damaged. 

For more information about material damage modeling, please refer to: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_mat/mat_damageall.html?q=hashin

 

Regards,

Wenlong

 

---

Useful Links

---

• How to access Ansys Online Help Document


• How to show full resolution image

 

[Matthew Pirkle]

Wenlong,

 

Thank you for your help!

Is it normal to not be able to get the failure index to reach a value of 1, even when the stresses in the lamina are high enough to satisfy the Hashin criterion equation? In fact, I have never been able to reach 1, only 0.9999.

For example, when I calculate the Hashin matrix tension failure index using the criterion equation and the stresses in the lamina, I get a damage variable value of 1.661 (which would indicate damage initiation), but ANSYS gives a maximum value of 0.747 (which would indicate no damage initiation). I am seeing a drop in fiber stresses immediately after that particular substep, leading me to believe that damage has occurred.

Is it possible that ANSYS has somehow scaled the damage variable output numbers such that they are appearing lower than what they really are? 

 

Thank you!

[Wenlong]

Hi mpirkle,

 

When damage is larger than 0, it means it has already initiated. When the damage reaches 1, it means the material has totally failed and cannot carry any load. The reason it only reaches 0.99999 but not 1 should be a numerical consideration, because completely changing the material stiffness to 0 (or in other words, make damage = 1) will make the matrix unsolvable. For example, for the following damage model, the damaged compliance matrix has a (1-d) in the denominator, so if the damage is 1, the denominator will be 0 and make the matrix unsolvable. 

Could it be possible that your Hashin matrix tension failure index is a different output than the damage variable? I am not familiar with this material model, but it is always a good idea to check with the manual and each output's meaning. 

 

Regards,

Wenlong

 

[Matthew Pirkle]

Wenlong,

 

What you say makes sense, and I think we are talking about two different things. The Hashin equations use a "failure index, f", and from what I understand, when equal to or greater than 1 this signifies the failure of the fiber or matrix and the initiation of damage within a lamina. This is what I thought ANSYS was displaying when using PLNSOL,PDMG,MT. 

But you are saying that ANSYS is actually displaying the matrix tension damage variable, dm. This is starting to make more sense to me, as to why the value is always much lower than 1, even when the stresses present in the lamina satisfy the Hashin equations, thereby indicating that damage has initiated, and is present in the lamina.

Do you know if ANSYS uses the 2D or the 3D Hashin equations? Below can also be seen the "failure index, f" that the equations use. Again, this is what I thought ANSYS was plotting when using PLNSOL,PDMG,MT. 

Is there a way to get ANSYS to plot the "failure index, f"?

 

 

 

Thank you so very much for your time and help!!

 

[Wenlong]

Hi mpirkle,

 

Then you may want to use "PLNSOL, FAIL, HFIB" for Hashin fiber failure criterion or "PLNSOL, FAIL, HMAT" for Hashin matrix fiber criterion. The reference can be found here: 

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_cmd/Hlp_C_PLNSOL.html%23plnsol.tab.fn9

 

For the Hashin Failure criterion theory, here are the equations from the Ansys help: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_thry/thy_str4.html?q=hashin%20theory I think these are the failure variable you are talking about. 

Hopefully this helps.

Regards,

Wenlong

 

---

Useful Links

---

• How to access Ansys Online Help Document


• How to show full resolution image