Empathy List Archives

RF

Raniero Falzon

Tue, Nov 15, 2016 8:25 AM

Hi,

I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning:

“The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.”

In my code I am in no way changing or creating any coordinate systems.

Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem.

I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences.

This is my first post, so please, notify me of any mistakes I made when posting.

Thanks in advance

Raniero Falzon
University of Malta

Hi, I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning: “The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.” In my code I am in no way changing or creating any coordinate systems. Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem. I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences. This is my first post, so please, notify me of any mistakes I made when posting. Thanks in advance Raniero Falzon University of Malta

DG

David Gross

Tue, Nov 15, 2016 2:48 PM

Raniero,

There are many ways to do this. One of them is to set the ESYS element attribute prior to meshing. See, for example, the AATT command.

Regards,

David Gross
Dominion Engineering, Inc.

-----Original Message-----
From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of Raniero Falzon
Sent: Tuesday, November 15, 2016 3:25 AM
To: xansys-temp@xansystest.info
Subject: [Xansys] [APDL] Shell 181 using different element coordinate system for each element

Hi,

I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning:

“The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.”

In my code I am in no way changing or creating any coordinate systems.

Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem.

I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences.

This is my first post, so please, notify me of any mistakes I made when posting.

Thanks in advance

Raniero Falzon
University of Malta

Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list

Raniero, There are many ways to do this. One of them is to set the ESYS element attribute prior to meshing. See, for example, the AATT command. Regards, David Gross Dominion Engineering, Inc. -----Original Message----- From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of Raniero Falzon Sent: Tuesday, November 15, 2016 3:25 AM To: xansys-temp@xansystest.info Subject: [Xansys] [APDL] Shell 181 using different element coordinate system for each element Hi, I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning: “The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.” In my code I am in no way changing or creating any coordinate systems. Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem. I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences. This is my first post, so please, notify me of any mistakes I made when posting. Thanks in advance Raniero Falzon University of Malta _______________________________________________ Xansys-temp mailing list Xansys-temp@xansystest.info http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day. Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list

MV

Mitch Voehl

Tue, Nov 15, 2016 8:09 PM

Raniero,

Each node in an ANSYS model has a nodal coordinate system associated with it. By default, nodal coordinate systems are parallel to the global Cartesian coordinate system. So, if you have not explicitly modified any nodal coordinate systems, they should all be parallel to the global Cartesian coordinate system (CSYS 0). Note that some symmetry boundary conditions will automatically rotate the affected nodal coordinate systems so you need to check for that. (ANSYS Mechancial (Workbench) may do this quietly behind the scenes.) /PSYMB,NDIR will control whether the nodal coordinate triads are displayed on your graphic plots.

Each element in an ANSYS model has an element coordinate system associated with it. "For area shell elements (such as SHELL63), the default orientation generally has the x-axis aligned with element I-J side, the z-axis normal to the shell surface (with the outward direction determined by the right-hand rule around the element from node I to J to K), and the y-axis perpendicular to the x and z-axes." Since SHELL181 elements provide a faceted approximation to a cylinder, and since the element coordinate systems are oriented with respect to the plane of the element, with Z being perpendicular to the plane of the element (radially inward or outward) the Z direction will vary from one element to its neighbor around the circumference of your cylinder. This is what ANSYS is warning you about.

See sections 2.2 and especially 2.3.1 in the Mechanical APDL Element Reference manual.

As David stated, the ESYS attribute can be used to modify the default orientation of the element coordinate systems. However, note that the ESYS coordinate system is projected onto the element surface, so the actual coordinate system used for calculating element results is still oriented parallel (and Z perpendicular to) each shell element surface.

Perhaps consider using NSOL along with ANSOL in /POST26 and compare the results to see how much effect the averaging is having.

There are many subtleties associated with proper understanding of coordinate systems and result display and averaging in ANSYS. See also

// Basic Analysis Guide // 7. The General Postprocessor (POST1) // 7.4. Additional POST1 Postprocessing

and
// Modeling and Meshing Guide // 3. Coordinate Systems

in the Mechanical APDL help documentation.

--
Mitch Voehl
CEO and Engineering Consultant

Summit Analysis, Inc.
1520 Thomas Lake Pointe Road, Suite 111
Eagan, MN 55122-2537

651-287-2360
www.summitanalysis.com

Specializing in the use of ANSYS (R) finite element analysis software

On November 15, 2016 at 8:48 AM David Gross dgross@domeng.com wrote:

Raniero,

There are many ways to do this. One of them is to set the ESYS element attribute prior to meshing. See, for example, the AATT command.

Regards,

David Gross
Dominion Engineering, Inc.

-----Original Message-----
From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of Raniero Falzon
Sent: Tuesday, November 15, 2016 3:25 AM
To: xansys-temp@xansystest.info
Subject: [Xansys] [APDL] Shell 181 using different element coordinate system for each element

Hi,

I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning:

“The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.”

In my code I am in no way changing or creating any coordinate systems.

Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem.

I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences.

This is my first post, so please, notify me of any mistakes I made when posting.

Thanks in advance

Raniero Falzon
University of Malta

Raniero, Each node in an ANSYS model has a nodal coordinate system associated with it. By default, nodal coordinate systems are parallel to the global Cartesian coordinate system. So, if you have not explicitly modified any nodal coordinate systems, they should all be parallel to the global Cartesian coordinate system (CSYS 0). Note that some symmetry boundary conditions will automatically rotate the affected nodal coordinate systems so you need to check for that. (ANSYS Mechancial (Workbench) may do this quietly behind the scenes.) /PSYMB,NDIR will control whether the nodal coordinate triads are displayed on your graphic plots. Each element in an ANSYS model has an element coordinate system associated with it. "For area shell elements (such as SHELL63), the default orientation generally has the x-axis aligned with element I-J side, the z-axis normal to the shell surface (with the outward direction determined by the right-hand rule around the element from node I to J to K), and the y-axis perpendicular to the x and z-axes." Since SHELL181 elements provide a faceted approximation to a cylinder, and since the element coordinate systems are oriented with respect to the plane of the element, with Z being perpendicular to the plane of the element (radially inward or outward) the Z direction will vary from one element to its neighbor around the circumference of your cylinder. This is what ANSYS is warning you about. See sections 2.2 and especially 2.3.1 in the Mechanical APDL Element Reference manual. As David stated, the ESYS attribute can be used to modify the default orientation of the element coordinate systems. However, note that the ESYS coordinate system is projected onto the element surface, so the actual coordinate system used for calculating element results is still oriented parallel (and Z perpendicular to) each shell element surface. Perhaps consider using NSOL along with ANSOL in /POST26 and compare the results to see how much effect the averaging is having. There are many subtleties associated with proper understanding of coordinate systems and result display and averaging in ANSYS. See also // Basic Analysis Guide // 7. The General Postprocessor (POST1) // 7.4. Additional POST1 Postprocessing and // Modeling and Meshing Guide // 3. Coordinate Systems in the Mechanical APDL help documentation. -- Mitch Voehl CEO and Engineering Consultant Summit Analysis, Inc. 1520 Thomas Lake Pointe Road, Suite 111 Eagan, MN 55122-2537 651-287-2360 www.summitanalysis.com Specializing in the use of ANSYS (R) finite element analysis software > On November 15, 2016 at 8:48 AM David Gross <dgross@domeng.com> wrote: > > > Raniero, > > There are many ways to do this. One of them is to set the ESYS element attribute prior to meshing. See, for example, the AATT command. > > Regards, > > David Gross > Dominion Engineering, Inc. > > -----Original Message----- > From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of Raniero Falzon > Sent: Tuesday, November 15, 2016 3:25 AM > To: xansys-temp@xansystest.info > Subject: [Xansys] [APDL] Shell 181 using different element coordinate system for each element > > Hi, > > I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning: > > “The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.” > > In my code I am in no way changing or creating any coordinate systems. > > Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem. > > I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences. > > This is my first post, so please, notify me of any mistakes I made when posting. > > Thanks in advance > > Raniero Falzon > University of Malta >

MV

Mitch Voehl

Tue, Nov 15, 2016 8:16 PM

Raniero,

P.S. /PSYMB,ESYS can be used to display the element coordinate system triads on your graphic plots, which will help you to understand how the element normal direction will vary around the circumference of your cylinder.

On November 15, 2016 at 2:09 PM Mitch Voehl mitchpublic@voehl.us wrote:

Raniero,

Each node in an ANSYS model has a nodal coordinate system associated with it. By default, nodal coordinate systems are parallel to the global Cartesian coordinate system. So, if you have not explicitly modified any nodal coordinate systems, they should all be parallel to the global Cartesian coordinate system (CSYS 0). Note that some symmetry boundary conditions will automatically rotate the affected nodal coordinate systems so you need to check for that. (ANSYS Mechancial (Workbench) may do this quietly behind the scenes.) /PSYMB,NDIR will control whether the nodal coordinate triads are displayed on your graphic plots.

Each element in an ANSYS model has an element coordinate system associated with it. "For area shell elements (such as SHELL63), the default orientation generally has the x-axis aligned with element I-J side, the z-axis normal to the shell surface (with the outward direction determined by the right-hand rule around the element from node I to J to K), and the y-axis perpendicular to the x and z-axes." Since SHELL181 elements provide a faceted approximation to a cylinder, and since the element coordinate systems are oriented with respect to the plane of the element, with Z being perpendicular to the plane of the element (radially inward or outward) the Z direction will vary from one element to its neighbor around the circumference of your cylinder. This is what ANSYS is warning you about.

See sections 2.2 and especially 2.3.1 in the Mechanical APDL Element Reference manual.

As David stated, the ESYS attribute can be used to modify the default orientation of the element coordinate systems. However, note that the ESYS coordinate system is projected onto the element surface, so the actual coordinate system used for calculating element results is still oriented parallel (and Z perpendicular to) each shell element surface.

Perhaps consider using NSOL along with ANSOL in /POST26 and compare the results to see how much effect the averaging is having.

There are many subtleties associated with proper understanding of coordinate systems and result display and averaging in ANSYS. See also

// Basic Analysis Guide // 7. The General Postprocessor (POST1) // 7.4. Additional POST1 Postprocessing

and
// Modeling and Meshing Guide // 3. Coordinate Systems

in the Mechanical APDL help documentation.

--
Mitch Voehl
CEO and Engineering Consultant

Summit Analysis, Inc.
1520 Thomas Lake Pointe Road, Suite 111
Eagan, MN 55122-2537

651-287-2360
www.summitanalysis.com

Specializing in the use of ANSYS (R) finite element analysis software

On November 15, 2016 at 8:48 AM David Gross dgross@domeng.com wrote:

Raniero,

There are many ways to do this. One of them is to set the ESYS element attribute prior to meshing. See, for example, the AATT command.

Regards,

David Gross
Dominion Engineering, Inc.

-----Original Message-----
From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of Raniero Falzon
Sent: Tuesday, November 15, 2016 3:25 AM
To: xansys-temp@xansystest.info
Subject: [Xansys] [APDL] Shell 181 using different element coordinate system for each element

Hi,

I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning:

“The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.”

In my code I am in no way changing or creating any coordinate systems.

Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem.

I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences.

This is my first post, so please, notify me of any mistakes I made when posting.

Thanks in advance

Raniero Falzon
University of Malta

Raniero, P.S. /PSYMB,ESYS can be used to display the element coordinate system triads on your graphic plots, which will help you to understand how the element normal direction will vary around the circumference of your cylinder. > On November 15, 2016 at 2:09 PM Mitch Voehl <mitchpublic@voehl.us> wrote: > > > Raniero, > > Each node in an ANSYS model has a nodal coordinate system associated with it. By default, nodal coordinate systems are parallel to the global Cartesian coordinate system. So, if you have not explicitly modified any nodal coordinate systems, they should all be parallel to the global Cartesian coordinate system (CSYS 0). Note that some symmetry boundary conditions will automatically rotate the affected nodal coordinate systems so you need to check for that. (ANSYS Mechancial (Workbench) may do this quietly behind the scenes.) /PSYMB,NDIR will control whether the nodal coordinate triads are displayed on your graphic plots. > > Each element in an ANSYS model has an element coordinate system associated with it. "For area shell elements (such as SHELL63), the default orientation generally has the x-axis aligned with element I-J side, the z-axis normal to the shell surface (with the outward direction determined by the right-hand rule around the element from node I to J to K), and the y-axis perpendicular to the x and z-axes." Since SHELL181 elements provide a faceted approximation to a cylinder, and since the element coordinate systems are oriented with respect to the plane of the element, with Z being perpendicular to the plane of the element (radially inward or outward) the Z direction will vary from one element to its neighbor around the circumference of your cylinder. This is what ANSYS is warning you about. > > See sections 2.2 and especially 2.3.1 in the Mechanical APDL Element Reference manual. > > As David stated, the ESYS attribute can be used to modify the default orientation of the element coordinate systems. However, note that the ESYS coordinate system is projected onto the element surface, so the actual coordinate system used for calculating element results is still oriented parallel (and Z perpendicular to) each shell element surface. > > Perhaps consider using NSOL along with ANSOL in /POST26 and compare the results to see how much effect the averaging is having. > > There are many subtleties associated with proper understanding of coordinate systems and result display and averaging in ANSYS. See also > > // Basic Analysis Guide // 7. The General Postprocessor (POST1) // 7.4. Additional POST1 Postprocessing > > and > // Modeling and Meshing Guide // 3. Coordinate Systems > > in the Mechanical APDL help documentation. > > -- > Mitch Voehl > CEO and Engineering Consultant > > Summit Analysis, Inc. > 1520 Thomas Lake Pointe Road, Suite 111 > Eagan, MN 55122-2537 > > 651-287-2360 > www.summitanalysis.com > > Specializing in the use of ANSYS (R) finite element analysis software > > > > On November 15, 2016 at 8:48 AM David Gross <dgross@domeng.com> wrote: > > > > > > Raniero, > > > > There are many ways to do this. One of them is to set the ESYS element attribute prior to meshing. See, for example, the AATT command. > > > > Regards, > > > > David Gross > > Dominion Engineering, Inc. > > > > -----Original Message----- > > From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of Raniero Falzon > > Sent: Tuesday, November 15, 2016 3:25 AM > > To: xansys-temp@xansystest.info > > Subject: [Xansys] [APDL] Shell 181 using different element coordinate system for each element > > > > Hi, > > > > I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning: > > > > “The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.” > > > > In my code I am in no way changing or creating any coordinate systems. > > > > Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem. > > > > I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences. > > > > This is my first post, so please, notify me of any mistakes I made when posting. > > > > Thanks in advance > > > > Raniero Falzon > > University of Malta

CW

Christopher Wright

Wed, Nov 16, 2016 1:45 AM

On Nov 15, 2016, at 2:25 AM, Raniero Falzon wrote:

In my code I am in no way changing or creating any coordinate systems.

The warning message deals with element coordinate systems which are defined relative to the nodes defining the elements. If the component stresses aren't calculated in the same coordinate system the averaging process would be garbage If I recall correctly you can set some option to redefine each element coordinate system as the global system—RTFM. I don't know how accurately I remember if it's an option for all elements or if it'd work in your problem. You need to check your element coordinate systems and how the stress you want is handled—check a few elements first.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania 1864)
http://www.skypoint.com/members/chrisw/

On Nov 15, 2016, at 2:25 AM, Raniero Falzon wrote: > In my code I am in no way changing or creating any coordinate systems. The warning message deals with element coordinate systems which are defined relative to the nodes defining the elements. If the component stresses aren't calculated in the same coordinate system the averaging process would be garbage If I recall correctly you can set some option to redefine each element coordinate system as the global system—RTFM. I don't know how accurately I remember if it's an option for all elements or if it'd work in your problem. You need to check your element coordinate systems and how the stress you want is handled—check a few elements first. Christopher Wright P.E. |"They couldn't hit an elephant at chrisw@skypoint.com | this distance" (last words of Gen. .......................................| John Sedgwick, Spotsylvania 1864) http://www.skypoint.com/members/chrisw/

JJ

James J. Kosloski

Wed, Nov 16, 2016 1:32 PM

Raniero,

This is just a warning, not an error. The key word in the warning is "which MAY not have consistent...", all it is saying is that ANSYS is not going to check the normals, it is just going to average the results. IF the normals are not consistent then the results will be wrong.

-Jim

James J. Kosloski
Director of Engineering Services

CAE Associates, Inc.
1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762
www.caeai.com

P: 203.758.2914 | F: 203.758.2965 | E: kosloski@caeai.com

-----Original Message-----
From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of Raniero Falzon
Sent: Tuesday, November 15, 2016 3:25 AM
To: xansys-temp@xansystest.info
Subject: [Xansys] [APDL] Shell 181 using different element coordinate system for each element

Hi,

I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning:

“The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.”

In my code I am in no way changing or creating any coordinate systems.

Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem.

I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences.

This is my first post, so please, notify me of any mistakes I made when posting.

Thanks in advance

Raniero Falzon
University of Malta

Xansys-temp mailing list
Xansys-temp@xansystest.info
http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list

This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.

Raniero, This is just a warning, not an error. The key word in the warning is "which MAY not have consistent...", all it is saying is that ANSYS is not going to check the normals, it is just going to average the results. IF the normals are not consistent then the results will be wrong. -Jim ________________________________ James J. Kosloski Director of Engineering Services CAE Associates, Inc. 1579 Straits Turnpike, Suite 2B | Middlebury, CT 06762 www.caeai.com P: 203.758.2914 | F: 203.758.2965 | E: kosloski@caeai.com -----Original Message----- From: Xansys-temp [mailto:xansys-temp-bounces@xansystest.info] On Behalf Of Raniero Falzon Sent: Tuesday, November 15, 2016 3:25 AM To: xansys-temp@xansystest.info Subject: [Xansys] [APDL] Shell 181 using different element coordinate system for each element Hi, I am trying to model a tube tensile test with shell 181 using an imported IGES file. I have managed to get a solution and was planning to use TimeHist Postpro to get the relevant stress-strain graph of a particular node or element and also for the entire specimen. When I choose to get nodal or element solution I am getting the following warning: “The averaging done by the ANSOL command together with the RSYS,SOLU command assumes consistent coordinate systems for all elements used in the averaging. Shell elements are present in the selected set which may not have consistent coordinate systems which in turn may lead to incorrectly averaged nodal results.” In my code I am in no way changing or creating any coordinate systems. Following a search on XANSYS, a post suggested that I create the geometry on the APDL itself. This did not solve the problem. I am using ANSYS 17 on Windows 10 but have also tried to run it on ANSYS 16.2 both with university licences. This is my first post, so please, notify me of any mistakes I made when posting. Thanks in advance Raniero Falzon University of Malta _______________________________________________ Xansys-temp mailing list Xansys-temp@xansystest.info http://xansystest.info/mailman/listinfo/xansys-temp_xansystest.info If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day. Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ This email and any attachments may contain privileged or confidential information of Computer Aided Engineering Associates. This e-mail is intended solely for the use of the individual or entity to which it is addressed. If you are not the intended recipient of this e-mail, you are hereby notified that any copying, distribution, dissemination or action taken in relation to the contents of this e-mail and any of its attachments is strictly prohibited and may be unlawful. If you have received this e-mail in error, please notify the sender immediately and permanently delete the original e-mail and destroy any copies or printouts of this e-mail as well as any attachments.

xansys-temp@list.xansys.org

[APDL] Shell 181 using different element coordinate system for each element