Search
Close this search box.
Notifications
Clear all

Convergence troubles with USERMAT subroutine

19 Posts
7 Users
0 Reactions
2,090 Views
Posts: 10
 Jay
(@Jay)
Active Member
Joined: 17 years ago

Which tangent modulus?

Hi Paul, hi Jorgen,

Paul are you shure, that you are using the right tangent modulus? Which one do you use? Up to my knowledge, ANSYS is using the same one as ABAQUS which is the tangent between the Green-Naghdi rate of Kirchhoff stresses and the rate of deformation tensor.

Jorgen, is that right for ABAQUS?

Thanks,

Armin

Reply
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

According to the ABAQUS manuals the exact consistent Jacobian is given by the variation in Kirchhoff stress with respect to the virtual rate of deformation.

Reply
Posts: 24
 mil
Topic starter
(@mil)
Eminent Member
Joined: 17 years ago

Jorgen, Armin and Marco,

now I know the origin of my (past) convergence problems:

Based on one sample code downloaded from the website I originally supposed that the material jacobian matrix required by ANSYS/ABAQUS is directly the spatial elasticity tensor. Now I know that this is not true and this caused my previous convergence problems. Nowadays I am using numerical perturbation method for Jaumann rate of Kirchhoff stress and everything seems to be OK :-).

Thank all of you for your help!!! I am really thankful for that.

Paul_S

Reply
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

Im glad it now works 🙂

Reply
Posts: 10
 Jay
(@Jay)
Active Member
Joined: 17 years ago

Jorgen,

just one more question: if you talking about the variation of Kirchhoff stress with respect to the rate of deformation tensor, its the so called Lie derivative. Is that right? But that differs from the Jauman rate..

For ANSYS I think the following is true: In the corotational approach, they use the Jauman rate (which is also the needed consistent tangent modulus). However, the corotational coordinate system is rotated by means of the rotation tensor. Therein, ANSYS expects all quantities (stresses, tangent). Up to my knowledge, this approach assumes small strains otherwise the corotated system differs more or less from the rotation tensor.

May be, we can discuss this a little further...

Armin

Reply
Posts: 4
(@abhi.suru)
New Member
Joined: 7 years ago

Hi All,

I defined a new hyperelastic material for Ansys using the USERMAT subroutine. Although it is working well for problems with global coordinate system, it diverges when I use the local coordinate system.:frown:

I would be very grateful if someone could help me to fix this problem.

Reply
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

Are you able to share your ANSYS files?
I suspect that you are not using the correct coordinate frame.

-Jorgen

Reply
Page 2 / 3
Share: