questions about computing strain in VUMAT (plane stress condition)

[nwpuheyl]

Dear researchers,
In the example provided in VUMAT, it looks like the strain is computed as strainNew=strainOld+strainInc. However, I want to compute strain using defmation gradient tensor F. The following procedure is applied, but it won't work correctly.

1. Get F matrix from ABAQUS ：
F(1,1)=defgradNew(1)
F(2,2)=defGradNew(2)
F(3,3)=defGradNew(3)
F(1,2)=defGradNew(4)
F(2,1)=defGradNew(5)
The rest components of F is set to be 0.

2.Get stretch tensor U
U(1,1)=stretchNew(1)
U(2,2)=stretchNew(2)
U(3,3)=stretchNew(3)
U(1,2)=stretchNew(4)
U(2,1)=stretchNew(4)
Also the rest components of U is set to be 0

3. Compute R with R=FU-1(U-1 means reverse of U)


4. Rotate F and get Frot using : Frot=RT * F * R( RT measn transpose of R)


5. Calculate strain from Frot

e11=0.5*( Frot (1,1) 2+ Frot (2,1) 2 -1)
e22=0.5*( Frot (1,2) 2+ Frot (2,2) 2-1)
e12=0.5*( Frot (1,1)* Frot (1,2)+ Frot (2,1)* Frot (2,2))

There must be something wrong with the above solution, but I can not figue it out. Please , can anyone help me. Thank you.


Yanli

[matsgd]

Is this a a case of plane stress then?

What strain measure are you trying to calculate? If you are trying to calculate the Green-Lagrange strain, then do it this way:

E=0.5*(U*U - I)=0.5*(F^t*F - I), where I is the identity tensor.

If you are trying to calculate a rotated version of this, e=RT*E*R, then do your rotation on U instead of on F. Or calculate the Green-Lagrange strain as above, and rotate it into e.

Mats

[nwpuheyl]

Thank you Mats, for your kind reply.

Yes, this is a plane stress problem, and I want to calclate true strain in the corotational coordinate system in VUMAT (I assume that U provided in Abaqus is in corotational coordinate system , while F is in global coordinate system ). If I follow as you suggest "calculate the Green-Lagrange strain as above, and rotate it into e", shall I do as this:

1) Get F tensor from ABAQUS with components F(1,1)=defgradNew(1) ,F(2,2)=defGradNew(2),F(3,3)=defGradNew(3),F(1,2)= defGradNew(4),F(2,1)=defGradNew(5), and set the rest components of F to be 0.

2) Use E=0.5*(F^t*F - I) to compute strain tensor( in global Coor sys)

3) Get stretch tensor U from ABAQUS with U(1,1)=stretchNew(1), U(2,2)=stretchNew(2), U(3,3)=stretchNew(3), U(1,2)=stretchNew(4), U(2,1)=stretchNew(4), and set the rest components as 0

4) Compute R using R=F * U^-1. (U^-1 means the inverse of U)

5) Rotate E into e in the corotational coordinate system using e=R^T * E * R.

I remember seeing a post somewhere saying you will get the same result whether you transform F first then calculate strain or calculate strain first then transform strain. So is there any difference between the procedure above and the procedure in my original post? I am not specialized in Mechanics, so please correct me if I mean something wrong.

Thank you for your attention.

Yanli

[matsgd]

Thank you Mats, for your kind reply.

Yes, this is a plane stress problem, and I want to calclate true strain in the corotational coordinate system in VUMAT (I assume that U provided in Abaqus is in corotational coordinate system , while F is in global coordinate system ). If I follow as you suggest "calculate the Green-Lagrange strain as above, and rotate it into e", shall I do as this:

1) Get F tensor from ABAQUS with components F(1,1)=defgradNew(1) ,F(2,2)=defGradNew(2),F(3,3)=defGradNew(3),F(1,2)= defGradNew(4),F(2,1)=defGradNew(5), and set the rest components of F to be 0.

2) Use E=0.5*(F^t*F - I) to compute strain tensor( in global Coor sys)

3) Get stretch tensor U from ABAQUS with U(1,1)=stretchNew(1), U(2,2)=stretchNew(2), U(3,3)=stretchNew(3), U(1,2)=stretchNew(4), U(2,1)=stretchNew(4), and set the rest components as 0

4) Compute R using R=F * U^-1. (U^-1 means the inverse of U)

5) Rotate E into e in the corotational coordinate system using e=R^T * E * R.

I remember seeing a post somewhere saying you will get the same result whether you transform F first then calculate strain or calculate strain first then transform strain. So is there any difference between the procedure above and the procedure in my original post? I am not specialized in Mechanics, so please correct me if I mean something wrong.

Thank you for your attention.

Yanli

I *think* that F is also, in fact, in the local coordinates of the element. You should not use the 33 component of F, I think (not sure what it contains when passed to the VUMAT). Instead, F(3,3) should be a consequence of the plane stress constraint, sigma(3,3)=0. When you calculate the thickness strain, ABAQUS additionally also wants the increment in this strain. (This is for eastimating a stable time step to be used in the global explicit time integration.)

Further, the rotation tensor R, as you define it, has nothing to do with transforming to the local frame of the element. It is just the rotational part of F, as given by the polar decomposition theorem...

M

[nwpuheyl]

I *think* that F is also, in fact, in the local coordinates of the element. You should not use the 33 component of F, I think (not sure what it contains when passed to the VUMAT). Instead, F(3,3) should be a consequence of the plane stress constraint, sigma(3,3)=0. When you calculate the thickness strain, ABAQUS additionally also wants the increment in this strain. (This is for eastimating a stable time step to be used in the global explicit time integration.)

Further, the rotation tensor R, as you define it, has nothing to do with transforming to the local frame of the element. It is just the rotational part of F, as given by the polar decomposition theorem...

M

Thank you Mats. That helps me understand F in VUMAT.