Shear Strain Increment

[ndf9f]

Is the strain increment given by ABAQUS to the Explicit VUMAT
subroutine the increment of engineeing shear strain or simply shear
strain (as in 1/2(u1,2 + u2,1))? The documentation states that
abaqus always uses engineering shear strain, but my VUMAT results
seem to inficate that the shear strain increment is not the
engineering shear strain increment.

Thanks if anyone knows the answer.

Nathan




------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->

[benjamin_hagege]

None of your propositions are right. The strain increment in
Abaqus/Explicit is a Green-Naghdi's one, i.e. it is D times dt in a
rotating frame. This frame is defined by R, the orthogonal part of
the deformation gradient F.

And NO, the documentation does NOT say that Abaqus uses only
engineering strains !!!!!! On the opposite : Abaqus never uses the
engineering strain when there are large deformations, as it is the
case in /Explicit.

BenZ.

Post by ndf9f
Is the strain increment given by ABAQUS to the Explicit VUMAT
subroutine the increment of engineeing shear strain or simply shear
strain (as in 1/2(u1,2 + u2,1))? The documentation states that
abaqus always uses engineering shear strain, but my VUMAT results
seem to inficate that the shear strain increment is not the
engineering shear strain increment.
Thanks if anyone knows the answer.
Nathan

------------------------ Yahoo! Groups Sponsor --------------------~-->
Yahoo! Domains - Claim yours for only $14.70
http://us.click.yahoo.com/Z1wmxD/DREIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->

[pierre_burgers]

VUMAT uses tensor strain values. This is impleied in the
documentation, but is not explcicitly stated. Also, note that VUMAT
uses a Green-Naghdi rate formulation where as some of the material
models (such as Mises plasticity) use a Jauman rate formaulation.

UMAT uses engineering shear strain.

All built-in models in ABAQUS/Standard and ABAQUS/Explicit use
engineering shear strain.

Post by ndf9f
Is the strain increment given by ABAQUS to the Explicit VUMAT
subroutine the increment of engineeing shear strain or simply shear
strain (as in 1/2(u1,2 + u2,1))? The documentation states that
abaqus always uses engineering shear strain, but my VUMAT results
seem to inficate that the shear strain increment is not the
engineering shear strain increment.
Thanks if anyone knows the answer.
Nathan

------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->

[benjamin_hagege]

No, really no dear comrad !

For the continuum elements, lemme remind you (i already posted about
this topic) that in /standard this is a jaumann formulation and
in /explicit it is a green-naghdi formulation. I personnaly proved
these facts with purely orthotropic elastic materials, so i do not
know what happens if plasticity is involved.

So UMAT does NOT use an engineering shear strain, or strain, but a
Jaumann strain, that is really NOT the same !!!

Lemme point out that the strains you postprocess isn't always the
strains really used in the UMAT/VUMAT.

BenZ.

Post by pierre_burgers
VUMAT uses tensor strain values. This is impleied in the
documentation, but is not explcicitly stated. Also, note that VUMAT
uses a Green-Naghdi rate formulation where as some of the material
models (such as Mises plasticity) use a Jauman rate formaulation.
UMAT uses engineering shear strain.
All built-in models in ABAQUS/Standard and ABAQUS/Explicit use
engineering shear strain.

Post by ndf9f
Is the strain increment given by ABAQUS to the Explicit VUMAT
subroutine the increment of engineeing shear strain or simply shear
strain (as in 1/2(u1,2 + u2,1))? The documentation states that
abaqus always uses engineering shear strain, but my VUMAT results
seem to inficate that the shear strain increment is not the
engineering shear strain increment.
Thanks if anyone knows the answer.
Nathan

------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->

[pierre_burgers]

When ABAQUS documentation refers to engineering shear srain, it
almost always is used to indicate that the shear strain component is
2 times the tensor shear strain component. Unless the context
indicates otherwise, it implies no more than this.

See
http://abaqus.custhelp.com/cgi-bin/abaqus.cfg/php/enduser/std_adp.php?
&p_faqid=2052&p_created=1087575169
for the strain rate measures used in ABAQUS/Standard and /Explicit
for the different element types.

Post by benjamin_hagege
No, really no dear comrad !
For the continuum elements, lemme remind you (i already posted

about

Post by benjamin_hagege
this topic) that in /standard this is a jaumann formulation and
in /explicit it is a green-naghdi formulation. I personnaly proved
these facts with purely orthotropic elastic materials, so i do not
know what happens if plasticity is involved.
So UMAT does NOT use an engineering shear strain, or strain, but a
Jaumann strain, that is really NOT the same !!!
Lemme point out that the strains you postprocess isn't always the
strains really used in the UMAT/VUMAT.
BenZ.

Post by pierre_burgers
VUMAT uses tensor strain values. This is impleied in the
documentation, but is not explcicitly stated. Also, note that VUMAT
uses a Green-Naghdi rate formulation where as some of the

material

Post by benjamin_hagege

Post by pierre_burgers
models (such as Mises plasticity) use a Jauman rate formaulation.
UMAT uses engineering shear strain.
All built-in models in ABAQUS/Standard and ABAQUS/Explicit use
engineering shear strain.

Post by ndf9f
Is the strain increment given by ABAQUS to the Explicit VUMAT
subroutine the increment of engineeing shear strain or simply

shear

Post by pierre_burgers

Post by ndf9f
strain (as in 1/2(u1,2 + u2,1))? The documentation states that
abaqus always uses engineering shear strain, but my VUMAT

results

Post by benjamin_hagege

Post by pierre_burgers

Post by ndf9f
seem to inficate that the shear strain increment is not the
engineering shear strain increment.
Thanks if anyone knows the answer.
Nathan

------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->

[chee-kuang kok]

This is the part I really don't understand. In ABAQUS/Explicit user's manual, under CONVENTION, it says: "ABAQUS always reports shear strain as engineering strain, gamma (symbol):
gammaij (indicial notation) = epsilonij + epsilonji"
Would you please explain this? Thank you very much.
Chee-Kuang Kok
Research Assistant, Michigan State University

--

--------- Original Message ---------
DATE: Tue, 15 Jun 2004 10:44:00
From: "benjamin_hagege" <***@yahoo.fr>
To: ***@yahoogroups.com
Cc:

None of your propositions are right. The strain increment in
Abaqus/Explicit is a Green-Naghdi's one, i.e. it is D times dt in a
rotating frame. This frame is defined by R, the orthogonal part of
the deformation gradient F.

And NO, the documentation does NOT say that Abaqus uses only
engineering strains !!!!!! On the opposite : Abaqus never uses the
engineering strain when there are large deformations, as it is the
case in /Explicit.

BenZ.

Post by ndf9f
Is the strain increment given by ABAQUS to the Explicit VUMAT
subroutine the increment of engineeing shear strain or simply shear
strain (as in 1/2(u1,2 + u2,1))? The documentation states that
abaqus always uses engineering shear strain, but my VUMAT results
seem to inficate that the shear strain increment is not the
engineering shear strain increment.
Thanks if anyone knows the answer.
Nathan

[benjamin_hagege]

As you said it, this topic is about CONVENTIONS and not
FORMULATIONS ! The manual states that if you take the shear strains,
you'll get, within small perturbations, the gammaij and not the
epsilonij (that is not obvious if you don't know it before !).
That's all ! Nothing is said (or have to be said) about the nature of
the strain.

BenZ.

Post by chee-kuang kok
This is the part I really don't understand. In ABAQUS/Explicit

user's manual, under CONVENTION, it says: "ABAQUS always reports

Post by chee-kuang kok
gammaij (indicial notation) = epsilonij + epsilonji"
Would you please explain this? Thank you very much.
Chee-Kuang Kok
Research Assistant, Michigan State University
--
--------- Original Message ---------
DATE: Tue, 15 Jun 2004 10:44:00
None of your propositions are right. The strain increment in
Abaqus/Explicit is a Green-Naghdi's one, i.e. it is D times dt in a
rotating frame. This frame is defined by R, the orthogonal part of
the deformation gradient F.
And NO, the documentation does NOT say that Abaqus uses only
engineering strains !!!!!! On the opposite : Abaqus never uses the
engineering strain when there are large deformations, as it is the
case in /Explicit.
BenZ.

Post by ndf9f
Is the strain increment given by ABAQUS to the Explicit VUMAT
subroutine the increment of engineeing shear strain or simply shear
strain (as in 1/2(u1,2 + u2,1))? The documentation states that
abaqus always uses engineering shear strain, but my VUMAT results
seem to inficate that the shear strain increment is not the
engineering shear strain increment.
Thanks if anyone knows the answer.
Nathan

http://groups.yahoo.com/group/abaqus
Yahoo! Groups Sponsor
ADVERTISEMENT
Yahoo! Groups Links
http://groups.yahoo.com/group/ABAQUS/
Your use of Yahoo! Groups is subject to the Yahoo! Terms of

Service.

Post by chee-kuang kok
____________________________________________________________
Find what you are looking for with the Lycos Yellow Pages

http://r.lycos.com/r/yp_emailfooter/http://yellowpages.lycos.com/defau
lt.asp?SRC=lycos10

Post by chee-kuang kok
[Non-text portions of this message have been removed]

------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->

[pierre_burgers]

ABAQUS uses tensor shear strain in VUMAT. Everywhere else, including
UMAT, the shear strain component is 2 times the tensor shear strain
component.

When ABAQUS documentation refers to using engineering shear strain,
it means the shear strain component is 2 times the tensor shear
strain component. It does not normally indicate anything concerning
the type of strain measure being used unless this is clear from the
context.

Post by chee-kuang kok
This is the part I really don't understand. In ABAQUS/Explicit

user's manual, under CONVENTION, it says: "ABAQUS always reports

Post by chee-kuang kok
gammaij (indicial notation) = epsilonij + epsilonji"
Would you please explain this? Thank you very much.
Chee-Kuang Kok
Research Assistant, Michigan State University
--
--------- Original Message ---------
DATE: Tue, 15 Jun 2004 10:44:00
None of your propositions are right. The strain increment in
Abaqus/Explicit is a Green-Naghdi's one, i.e. it is D times dt in a
rotating frame. This frame is defined by R, the orthogonal part of
the deformation gradient F.
And NO, the documentation does NOT say that Abaqus uses only
engineering strains !!!!!! On the opposite : Abaqus never uses the
engineering strain when there are large deformations, as it is the
case in /Explicit.
BenZ.

Post by ndf9f
Is the strain increment given by ABAQUS to the Explicit VUMAT
subroutine the increment of engineeing shear strain or simply shear
strain (as in 1/2(u1,2 + u2,1))? The documentation states that
abaqus always uses engineering shear strain, but my VUMAT results
seem to inficate that the shear strain increment is not the
engineering shear strain increment.
Thanks if anyone knows the answer.
Nathan

http://groups.yahoo.com/group/abaqus
Yahoo! Groups Sponsor
ADVERTISEMENT
Yahoo! Groups Links
http://groups.yahoo.com/group/ABAQUS/
Your use of Yahoo! Groups is subject to the Yahoo! Terms of

Service.

Post by chee-kuang kok
____________________________________________________________
Find what you are looking for with the Lycos Yellow Pages

http://r.lycos.com/r/yp_emailfooter/http://yellowpages.lycos.com/defau
lt.asp?SRC=lycos10

Post by chee-kuang kok
[Non-text portions of this message have been removed]

------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->