XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[Xansys] Bilinear analysis fro beam188
 
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
Author Message
juan.carlos.peteiro
User


Joined: 11 Aug 2014
Posts: 13

PostPosted: Tue Aug 12, 2014 2:40 am  Reply with quote

Hi all,

In order to check buckling for the entire model of an offshore leg, I need to use a bilinear stress-strain curve. Before that I make a simple model of a single beam with all dof constraint in one end and I apply bending moment in the other end. In material I put the properties of E, v, and tangent modulus. The results show that the software is no reading the bilinear curve. I get no plastification in the beam section as the hand calculation shows. Can anybody please help me?.

Thanks,

Juan Ceballos
Structural Engineer
Houlder
----------------------------------------------------------------------------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com
-----------------------------------------------------------------------------------------------------------------------------------------


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Aug 12, 2014 3:25 am  Reply with quote

Dear Mr. Peteiro:

wouldn't you also need to specify yield stress?

Have you checked your units?

Have you compared the cross-section properties (area, moment of inertia
about weak and strong axis) from Ansys (see the commands slist and
secplot) with the values that you use for your hand calculation (taken
from commercial tables)? They may have some differences, because the
commercial profiles have rounded corners and the Ansys sections haven't.


Best regards,

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain

El 12/08/2014 11:40, Juan Carlos Peteiro escribió:

Quote:
Hi all,

In order to check buckling for the entire model of an offshore leg, I need to use a bilinear stress-strain curve. Before that I make a simple model of a single beam with all dof constraint in one end and I apply bending moment in the other end. In material I put the properties of E, v, and tangent modulus. The results show that the software is no reading the bilinear curve. I get no plastification in the beam section as the hand calculation shows. Can anybody please help me?.

Thanks,

Juan Ceballos
Structural Engineer
Houlder
----------------------------------------------------------------------------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com [1]
-----------------------------------------------------------------------------------------------------------------------------------------

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [2] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [3] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://www.mimecast.com
[2] http://www.xansys.org/forum
[3] http://www.padtinc.com
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
juan.carlos.peteiro
User


Joined: 11 Aug 2014
Posts: 13

PostPosted: Tue Aug 12, 2014 3:34 am  Reply with quote

Hi Jose,

Thank you for your reply.

The information used:

- Material: E = 200000 MPa, v = 0.3, Yield = 250 MPa, bilinear with Tangent modulus = 2000 MPa.
- Section: rectangular 10x100 mm.
- Load: moment = 5 e6 Nmm
- Beam188

The stress I am getting = M/w = (5e6)/(10*100*100/6) = 300 MPa.

I would expect the stress not to go higher than around 250 MPa

Thanks,

Juan C.

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of mfernan@us.es
Sent: 12 August 2014 11:25
To: ANSYS User Discussion List
Subject: Re: [Xansys] Bilinear analysis fro beam188



Dear Mr. Peteiro:

wouldn't you also need to specify yield stress?

Have you checked your units?

Have you compared the cross-section properties (area, moment of inertia about weak and strong axis) from Ansys (see the commands slist and
secplot) with the values that you use for your hand calculation (taken from commercial tables)? They may have some differences, because the commercial profiles have rounded corners and the Ansys sections haven't.


Best regards,

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain

El 12/08/2014 11:40, Juan Carlos Peteiro escribió:

Quote:
Hi all,

In order to check buckling for the entire model of an offshore leg, I need to use a bilinear stress-strain curve. Before that I make a simple model of a single beam with all dof constraint in one end and I apply bending moment in the other end. In material I put the properties of E, v, and tangent modulus. The results show that the software is no reading the bilinear curve. I get no plastification in the beam section as the hand calculation shows. Can anybody please help me?.

Thanks,

Juan Ceballos
Structural Engineer
Houlder
----------------------------------------------------------------------
------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com [1]
----------------------------------------------------------------------
-------------------------------------------------------------------

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [2] | The Online Community for
| users of ANSYS, Inc. Software | Hosted by PADT - www.padtinc.com [3]
| | Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://www.mimecast.com
[2] http://www.xansys.org/forum
[3] http://www.padtinc.com
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
----------------------------------------------------------------------------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com
-----------------------------------------------------------------------------------------------------------------------------------------
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Tue Aug 12, 2014 3:57 am  Reply with quote

On 12/08/2014 11:34, Juan Carlos Peteiro wrote:
Quote:

The information used:

- Material: E = 200000 MPa, v = 0.3, Yield = 250 MPa, bilinear with Tangent modulus = 2000 MPa.
- Section: rectangular 10x100 mm.
- Load: moment = 5 e6 Nmm
- Beam188

The stress I am getting = M/w = (5e6)/(10*100*100/6) = 300 MPa.

I would expect the stress not to go higher than around 250 MPa

I don't think you have said what sort of cross section you are using but
have you specified enough cells so that the stresses at the integration
points are above yield?

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
juan.carlos.peteiro
User


Joined: 11 Aug 2014
Posts: 13

PostPosted: Tue Aug 12, 2014 4:00 am  Reply with quote

Hi Martin,

It is a rectangular section of 10 mm x 100 mm.

Please help me to understand what you mean by " enough cells so that the stresses at the integration points are above yield ".

I appreciate your help.

Cheers,

Juan C.

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Martin Liddle
Sent: 12 August 2014 11:57
To: xansys@xansys.org
Subject: Re: [Xansys] Bilinear analysis fro beam188

On 12/08/2014 11:34, Juan Carlos Peteiro wrote:
Quote:

The information used:

- Material: E = 200000 MPa, v = 0.3, Yield = 250 MPa, bilinear with Tangent modulus = 2000 MPa.
- Section: rectangular 10x100 mm.
- Load: moment = 5 e6 Nmm
- Beam188

The stress I am getting = M/w = (5e6)/(10*100*100/6) = 300 MPa.

I would expect the stress not to go higher than around 250 MPa

I don't think you have said what sort of cross section you are using but have you specified enough cells so that the stresses at the integration points are above yield?

--
Martin Liddle, Tynemouth Computer Services, Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
----------------------------------------------------------------------------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com
-----------------------------------------------------------------------------------------------------------------------------------------

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Aug 12, 2014 4:25 am  Reply with quote

Dear Mr. Peteiro:

please, check the ansys help on BEAM188 element. The cross-section is
meshed with cells. By default, a 2x2 mesh is used for rectangular
cross-sections.

"When the material associated with the elements has inelastic behavior
or when the temperature varies across the section, constitutive
calculations are performed at the section integration points". The
integration points (Gauss points) are located inside the cells, and
therefore their stress will be lower that on the edges. If you are using
the default mesh, those integration points will be quite far from the
edge, and they will not yield until much higher bending moments than
your hand calculations.

If you want to accurately capture the initiation of yielding, you need
to improve the mesh of the cross-section, by increasing the number of
elements and refining them (making them smaller) near the boundaries. By
doing so, your integration points will be very close to the edges.

You can control the cross-section meshing with two commands:

SECTYPE, SECID, Type, Subtype, Name, REFINEKEY

(modify the value of REFINEKEY, from the default of 0, no refinement,
to 5, high level of refinement)

SECDATA,B,H,Nb,Nh

For a rectangular cross-section, you can indicate the number of cells
along width (Nb, default 2) and along height (Nh, default 2). You will
have to increase those values.

With the command secplot,1 you will be able to plot the beam
cross-section mesh that Ansys generates.

You can try with several meshes and refinements, until you get an
acceptable agreement with your hand calculation for the onset of
plasticity.

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
juan.carlos.peteiro
User


Joined: 11 Aug 2014
Posts: 13

PostPosted: Tue Aug 12, 2014 5:17 am  Reply with quote

Hi Jose,

Many thanks to you and Martin. It worked as you predicted.

Most appreciated.

Juan Carlos

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of mfernan@us.es
Sent: 12 August 2014 12:25
To: ANSYS User Discussion List
Subject: Re: [Xansys] Bilinear analysis fro beam188



Dear Mr. Peteiro:

please, check the ansys help on BEAM188 element. The cross-section is meshed with cells. By default, a 2x2 mesh is used for rectangular cross-sections.

"When the material associated with the elements has inelastic behavior or when the temperature varies across the section, constitutive calculations are performed at the section integration points". The integration points (Gauss points) are located inside the cells, and therefore their stress will be lower that on the edges. If you are using the default mesh, those integration points will be quite far from the edge, and they will not yield until much higher bending moments than your hand calculations.

If you want to accurately capture the initiation of yielding, you need to improve the mesh of the cross-section, by increasing the number of elements and refining them (making them smaller) near the boundaries. By doing so, your integration points will be very close to the edges.

You can control the cross-section meshing with two commands:

SECTYPE, SECID, Type, Subtype, Name, REFINEKEY

(modify the value of REFINEKEY, from the default of 0, no refinement, to 5, high level of refinement)

SECDATA,B,H,Nb,Nh

For a rectangular cross-section, you can indicate the number of cells along width (Nb, default 2) and along height (Nh, default 2). You will have to increase those values.

With the command secplot,1 you will be able to plot the beam cross-section mesh that Ansys generates.

You can try with several meshes and refinements, until you get an acceptable agreement with your hand calculation for the onset of plasticity.

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
----------------------------------------------------------------------------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com
-----------------------------------------------------------------------------------------------------------------------------------------

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
juan.carlos.peteiro
User


Joined: 11 Aug 2014
Posts: 13

PostPosted: Tue Aug 12, 2014 8:24 am  Reply with quote

Hi There,

I need one more clarification to move forward. I am actually using a not standard section that I am drawing in Ansys. For that not standard section I need to increase the integration points to take into account the plasticity. Please could anyone help me how to do it?.

Thanks,

Juan C.

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of mfernan@us.es
Sent: 12 August 2014 12:25
To: ANSYS User Discussion List
Subject: Re: [Xansys] Bilinear analysis fro beam188



Dear Mr. Peteiro:

please, check the ansys help on BEAM188 element. The cross-section is meshed with cells. By default, a 2x2 mesh is used for rectangular cross-sections.

"When the material associated with the elements has inelastic behavior or when the temperature varies across the section, constitutive calculations are performed at the section integration points". The integration points (Gauss points) are located inside the cells, and therefore their stress will be lower that on the edges. If you are using the default mesh, those integration points will be quite far from the edge, and they will not yield until much higher bending moments than your hand calculations.

If you want to accurately capture the initiation of yielding, you need to improve the mesh of the cross-section, by increasing the number of elements and refining them (making them smaller) near the boundaries. By doing so, your integration points will be very close to the edges.

You can control the cross-section meshing with two commands:

SECTYPE, SECID, Type, Subtype, Name, REFINEKEY

(modify the value of REFINEKEY, from the default of 0, no refinement, to 5, high level of refinement)

SECDATA,B,H,Nb,Nh

For a rectangular cross-section, you can indicate the number of cells along width (Nb, default 2) and along height (Nh, default 2). You will have to increase those values.

With the command secplot,1 you will be able to plot the beam cross-section mesh that Ansys generates.

You can try with several meshes and refinements, until you get an acceptable agreement with your hand calculation for the onset of plasticity.

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
----------------------------------------------------------------------------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com
-----------------------------------------------------------------------------------------------------------------------------------------

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Aug 12, 2014 9:48 am  Reply with quote

Dear Mr. Peteiro:

for that non-standard cross-section, you will be defining a 2D solid
model of your cross-section geometry, and then you use the command
SECWRITE. Ansys creates a mesh of your 2D solid model. With the command
SECREAD you read the mesh of your cross-section.

Instead of using the initial mesh, you can refine it. You can also
assign different materials to different elements.

Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up>
Refine Mesh

After modifying the mesh of the cross-section, you will have to write it
to a file (SECWRITE). Later, use the command SECREAD to create a cross
section with the refined mesh.

Check the ansys manual (Structural Guide / Beam Analysis and Cross
sections/ Creating Custom Cross Sections with Mesh Refinement and
Multiple Materials)

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain

El 12/08/2014 17:23, Juan Carlos Peteiro escribió:

Quote:
Hi There,

I need one more clarification to move forward. I am actually using a not standard section that I am drawing in Ansys. For that not standard section I need to increase the integration points to take into account the plasticity. Please could anyone help me how to do it?.

Thanks,

Juan C.

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of mfernan@us.es
Sent: 12 August 2014 12:25
To: ANSYS User Discussion List
Subject: Re: [Xansys] Bilinear analysis fro beam188

Dear Mr. Peteiro:

please, check the ansys help on BEAM188 element. The cross-section is meshed with cells. By default, a 2x2 mesh is used for rectangular cross-sections.

"When the material associated with the elements has inelastic behavior or when the temperature varies across the section, constitutive calculations are performed at the section integration points". The integration points (Gauss points) are located inside the cells, and therefore their stress will be lower that on the edges. If you are using the default mesh, those integration points will be quite far from the edge, and they will not yield until much higher bending moments than your hand calculations.

If you want to accurately capture the initiation of yielding, you need to improve the mesh of the cross-section, by increasing the number of elements and refining them (making them smaller) near the boundaries. By doing so, your integration points will be very close to the edges.

You can control the cross-section meshing with two commands:

SECTYPE, SECID, Type, Subtype, Name, REFINEKEY

(modify the value of REFINEKEY, from the default of 0, no refinement, to 5, high level of refinement)

SECDATA,B,H,Nb,Nh

For a rectangular cross-section, you can indicate the number of cells along width (Nb, default 2) and along height (Nh, default 2). You will have to increase those values.

With the command secplot,1 you will be able to plot the beam cross-section mesh that Ansys generates.

You can try with several meshes and refinements, until you get an acceptable agreement with your hand calculation for the onset of plasticity.

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [1] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [2] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
----------------------------------------------------------------------------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com [3]
-----------------------------------------------------------------------------------------------------------------------------------------

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [1] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [2] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://www.xansys.org/forum
[2] http://www.padtinc.com
[3] http://www.mimecast.com
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
juan.carlos.peteiro
User


Joined: 11 Aug 2014
Posts: 13

PostPosted: Tue Aug 12, 2014 10:01 am  Reply with quote

Hi Jose,

That worked!.

Cheers,

Juan Carlos

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of mfernan@us.es
Sent: 12 August 2014 17:48
To: ANSYS User Discussion List
Subject: Re: [Xansys] Bilinear analysis fro beam188



Dear Mr. Peteiro:

for that non-standard cross-section, you will be defining a 2D solid model of your cross-section geometry, and then you use the command SECWRITE. Ansys creates a mesh of your 2D solid model. With the command SECREAD you read the mesh of your cross-section.

Instead of using the initial mesh, you can refine it. You can also assign different materials to different elements.

Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-up> Refine Mesh

After modifying the mesh of the cross-section, you will have to write it to a file (SECWRITE). Later, use the command SECREAD to create a cross section with the refined mesh.

Check the ansys manual (Structural Guide / Beam Analysis and Cross sections/ Creating Custom Cross Sections with Mesh Refinement and Multiple Materials)

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain

El 12/08/2014 17:23, Juan Carlos Peteiro escribió:

Quote:
Hi There,

I need one more clarification to move forward. I am actually using a not standard section that I am drawing in Ansys. For that not standard section I need to increase the integration points to take into account the plasticity. Please could anyone help me how to do it?.

Thanks,

Juan C.

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
mfernan@us.es
Sent: 12 August 2014 12:25
To: ANSYS User Discussion List
Subject: Re: [Xansys] Bilinear analysis fro beam188

Dear Mr. Peteiro:

please, check the ansys help on BEAM188 element. The cross-section is meshed with cells. By default, a 2x2 mesh is used for rectangular cross-sections.

"When the material associated with the elements has inelastic behavior or when the temperature varies across the section, constitutive calculations are performed at the section integration points". The integration points (Gauss points) are located inside the cells, and therefore their stress will be lower that on the edges. If you are using the default mesh, those integration points will be quite far from the edge, and they will not yield until much higher bending moments than your hand calculations.

If you want to accurately capture the initiation of yielding, you need to improve the mesh of the cross-section, by increasing the number of elements and refining them (making them smaller) near the boundaries. By doing so, your integration points will be very close to the edges.

You can control the cross-section meshing with two commands:

SECTYPE, SECID, Type, Subtype, Name, REFINEKEY

(modify the value of REFINEKEY, from the default of 0, no refinement,
to 5, high level of refinement)

SECDATA,B,H,Nb,Nh

For a rectangular cross-section, you can indicate the number of cells along width (Nb, default 2) and along height (Nh, default 2). You will have to increase those values.

With the command secplot,1 you will be able to plot the beam cross-section mesh that Ansys generates.

You can try with several meshes and refinements, until you get an acceptable agreement with your hand calculation for the onset of plasticity.

Jose M. Galan

Constr. Engin. Dept.

Univ. Sevilla

Spain
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [1] | The Online Community for
| users of ANSYS, Inc. Software | Hosted by PADT - www.padtinc.com [2]
| | Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
----------------------------------------------------------------------
------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com [3]
----------------------------------------------------------------------
-------------------------------------------------------------------

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [1] | The Online Community for
| users of ANSYS, Inc. Software | Hosted by PADT - www.padtinc.com [2]
| | Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://www.xansys.org/forum
[2] http://www.padtinc.com
[3] http://www.mimecast.com
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
----------------------------------------------------------------------------------------------------------------------------------------
This email message has been delivered safely and archived online by Mimecast.
For more information please visit http://www.mimecast.com
-----------------------------------------------------------------------------------------------------------------------------------------
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Aug 12, 2014 10:11 am  Reply with quote

Dear Juan Carlos:

Don't forget to include your full name and affiliation (company name) on
all your xansys post. Those are xansys rules, and there are consequences
for not complying them.

You can automate signatures in your email application and Forum profile.


You can find the rules at the "Announcements" at the top of the forum or
in the following link (http://www.xansys.org/RULES.html).

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
Display posts from previous:   
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
All times are GMT - 7 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum
You cannot attach files in this forum
You cannot download files in this forum


Powered by phpBB © 2001, 2005 phpBB Group

sleek template created by Andrew Charron