Author 
Message 
danbohlen User
Joined: 18 Aug 2008 Posts: 951 Location: Evendale OH

Posted: Tue Oct 08, 2013 4:50 am 


Hi Guys,
Does anyone out there have a method for estimating the error for a mesh? Not looking for a thesis paper (found plenty of those online – I get whoozy when a see a page of Greek symbols anymore.) – more like using SERR or SDSG in Ansys. We’ve had a conservative method here for years, but now there seems to be some interest in finding a less conservative way to assure one’s mesh error is only a certain % of the stress calculated.
Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis
STAR review chairman, Fan and Booster
GE Aircraft Engines
1 Neumann Way
Evendale, OH 45215
Build 90 Col K1.5 cube 1N152
M/D H110 5132432366
Dial Comm *3322366
Post generated using Mail2Forum (http://www.mail2forum.com) _________________ Dan Bohlen
Senior Staff Engineer
GE Aircraft Engines 

Back to top 


joseph.metrisin User
Joined: 07 May 2009 Posts: 404

Posted: Tue Oct 08, 2013 5:02 am 


Hi Dan,
We just compare the SMX and SMXB values, and try to keep them within a certain percentage of each other.
Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)4276346 Office
(561)4276191 Fax
JMetrisin@fttinc.com
Visit our new website: www.fttinc.com
FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com

Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.

Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Tuesday, October 08, 2013 7:50 AM
To: ANSYS User Discussion List
Subject: [Xansys] Mesh Error Estimation
Hi Guys,
Does anyone out there have a method for estimating the error for a mesh? Not looking for a thesis paper (found plenty of those online  I get whoozy when a see a page of Greek symbols anymore.)  more like using SERR or SDSG in Ansys. We've had a conservative method here for years, but now there seems to be some interest in finding a less conservative way to assure one's mesh error is only a certain % of the stress calculated.
Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH 45215
Build 90 Col K1.5 cube 1N152
M/D H110 5132432366
Dial Comm *3322366
++
 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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


rahul.sangole User
Joined: 28 Sep 2009 Posts: 29 Location: IN

Posted: Wed Oct 09, 2013 5:08 am 


I'm interested in this as well. Sounds like you want a confidence interval on your stress values, as a function of mesh density.
I use a couple of ways to ensure appropriate mesh density in regions of interest (I'm sure you're aware of these). These are just guidelines:
1. PRERR,SEPC < 15% for the entire model
2. PRERR,SEPC < 10% in local stress region
3. PRERR,SEPC < 7% for 2 waves of elements from highest stress/strain node
4. % difference between SMAXB and SMAX, or SMINB and SMIN < 7% for 2 waves of elements from highest stress/strain node
I don't use SDSG as much. _________________ Rahul Sangole
Structural Analysis Group
Cummins Inc 

Back to top 


rod.scholl User
Joined: 22 Oct 2010 Posts: 86

Posted: Wed Oct 09, 2013 7:30 am 


Sounds like we have similar approaches, Rahul. I recently gave some thought
to the "confidence interval" idea. I don't think it is workable
unfortunately:
In terms of statistics, confidence interval assumes some distribution of
variation (such as a "normal distribution")  then using the two data
points (one from node XYZ of element A, and the other from the element B
sharing this node) the idea would be to establish the likelihood (confidence
interval) that the converged value would be less than some selected or
calculated Sig_MAX, for example.
However, the converged stress would be different for a flat surface compared
to a fillet, even though the element A and element B differential might be
the same. This is a simple example of how the potential converged solution
depends on the geometry, and just the two values alone are not enough to
come up with a confidence interval... more information is needed. (which is
why this hasn't been done already).
What *can* be done, is for a given geometry, such as a 90degree fillet for
a 2D model (or unchanging in 3rd dimension) we *do* know how quickly the
mesh converges to the theoretical solution. So a confidence interval can be
calculated for a particular upper bound (be it SMXB or whatever we
choose)... what people have found is that 6 elements through the thickness
demarks a "high" confidence interval and this ruleofthumb is popular I've
found. But as soon as a 2nd order effect enters (like 3D stress state, body
loads, compound fillet, curvature in 3D, etc.) our relationship breaks down
and we're left without confidence interval.
Basically, if one has a well known geometry/load/3D effect we can save
ourselves the node count, mesh it coarsely and then use some previous
convergence study to get a decent prediction of the converged solution using
a fairly coarse model and the discretization difference between the two
elements (and even come up with a confidence interval). But geometry/loads
are rarely that clean/consistent (or we'd just use a KT chart and a radius!)
Hopefully I'm not soundinglecturey, just I went down this road thinking it
could be done, and realized we are stuck with things like PRERR,SEPC energy
comparisons. No simple answer or it woulda been programmed right in
already. We can chalk it up to "job security" :)
______________________________
Rod Scholl
Principal Analyst  Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf
Of rahul.sangole
Sent: Wednesday, October 09, 2013 7:09 AM
To: xansys@xansys.org
Subject: Re: [Xansys] Mesh Error Estimation
I'm interested in this as well. Sounds like you want a confidence interval
on your stress values, as a function of mesh density.
I use a couple of ways to ensure appropriate mesh density in regions of
interest (I'm sure you're aware of these). These are just guidelines:
1. PRERR,SEPC < 15% for the entire model
2. PRERR,SEPC < 10% in local stress region
3. PRERR,SEPC < 7% for 2 waves of elements from highest stress/strain node
4. % difference between SMAXB and SMAX, or SMINB and SMIN < 7% for 2 waves
of elements from highest stress/strain node
I don't use SDSG as much.

Rahul Sangole
Structural Analysis Group
Cummins Inc
++
 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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 


danbohlen User
Joined: 18 Aug 2008 Posts: 951 Location: Evendale OH

Posted: Wed Oct 09, 2013 7:57 am 


Yep, there's no magic bullet. We have a conservative method we use (short of rerunning with a different mesh density.) It does give some false positives (indicating the mesh is not converged  when is actually is). Some of our team took it upon themselves to come up with a new method (easier?, faster?, more accurate???) based on some energy error term (SERR? They didn't really say) and run a bunch of our typical jet motor type locations and come up with some normalized energy error criteria.
My put back to them based on the responses to this posting is why not do the same semiempirical indicator using the what is already in Ansys (SMX SMXB) that was put there as a mesh convergence indicator.
Thanks to all,
Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis
STAR review chairman, Fan and Booster
GE Aircraft Engines
1 Neumann Way
Evendale, OH 45215
Build 90 Col K1.5 cube 1N152
M/D H110 5132432366
Dial Comm *3322366
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf Of Rod Scholl
Sent: Wednesday, October 09, 2013 10:30 AM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] Mesh Error Estimation
Sounds like we have similar approaches, Rahul. I recently gave some thought to the "confidence interval" idea. I don't think it is workable
unfortunately:
In terms of statistics, confidence interval assumes some distribution of variation (such as a "normal distribution")  then using the two data points (one from node XYZ of element A, and the other from the element B sharing this node) the idea would be to establish the likelihood (confidence
interval) that the converged value would be less than some selected or calculated Sig_MAX, for example.
However, the converged stress would be different for a flat surface compared to a fillet, even though the element A and element B differential might be the same. This is a simple example of how the potential converged solution depends on the geometry, and just the two values alone are not enough to come up with a confidence interval... more information is needed. (which is why this hasn't been done already).
What *can* be done, is for a given geometry, such as a 90degree fillet for a 2D model (or unchanging in 3rd dimension) we *do* know how quickly the mesh converges to the theoretical solution. So a confidence interval can be calculated for a particular upper bound (be it SMXB or whatever we choose)... what people have found is that 6 elements through the thickness demarks a "high" confidence interval and this ruleofthumb is popular I've found. But as soon as a 2nd order effect enters (like 3D stress state, body loads, compound fillet, curvature in 3D, etc.) our relationship breaks down and we're left without confidence interval.
Basically, if one has a well known geometry/load/3D effect we can save ourselves the node count, mesh it coarsely and then use some previous convergence study to get a decent prediction of the converged solution using a fairly coarse model and the discretization difference between the two elements (and even come up with a confidence interval). But geometry/loads are rarely that clean/consistent (or we'd just use a KT chart and a radius!)
Hopefully I'm not soundinglecturey, just I went down this road thinking it could be done, and realized we are stuck with things like PRERR,SEPC energy comparisons. No simple answer or it woulda been programmed right in already. We can chalk it up to "job security" :)
______________________________
Rod Scholl
Principal Analyst  Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf Of rahul.sangole
Sent: Wednesday, October 09, 2013 7:09 AM
To: xansys@xansys.org
Subject: Re: [Xansys] Mesh Error Estimation
I'm interested in this as well. Sounds like you want a confidence interval on your stress values, as a function of mesh density.
I use a couple of ways to ensure appropriate mesh density in regions of interest (I'm sure you're aware of these). These are just guidelines:
1. PRERR,SEPC < 15% for the entire model 2. PRERR,SEPC < 10% in local stress region 3. PRERR,SEPC < 7% for 2 waves of elements from highest stress/strain node 4. % difference between SMAXB and SMAX, or SMINB and SMIN < 7% for 2 waves of elements from highest stress/strain node
I don't use SDSG as much.

Rahul Sangole
Structural Analysis Group
Cummins Inc
++
 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 xansysmod@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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) _________________ Dan Bohlen
Senior Staff Engineer
GE Aircraft Engines 

Back to top 


rod.scholl User
Joined: 22 Oct 2010 Posts: 86

Posted: Wed Oct 09, 2013 10:31 am 


There's a definite advantage of PRERR approach over the SMXB (though maybe
not worth the extra snippet). Of course the finer points are that PRERR
uses norms and take into account energy and not just stress value  though
I'll agree that dividing SMX by SMXB gets you most the way there for a
material/regime one is familiar with. The bigger distinction is that SMXB
is based on the worst case discretization at any node in the model (also
note that SMXB does not always correspond to the SMX location!)  whereas
with PRERR you can select a few elements, or a region, or the whole model
and get an assessment of the error in energy for the portion.
The distinction is more important when you consider the ultrafast mesh size
transition rates Mechanical produces (unless you switch to the "aggressive"
shapechecking that the Mechanical APDL uses). Nowadays you can have a very
fine tet mesh at the peak stress  and literally one element away has 10X
the edge length.
I am playing devil's advocate, of course  in most cases I don't look at
either SMXB or PRERR calc's  with 20,000+ hours of doing FEA a plot of the
mesh contours and engineering judgment go a long way. To quote from a
dubious source, "I don't practice what I preach because I'm not the kind of
person I'm preaching to."
______________________________
Rod Scholl
Principal Analyst  Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf
Of Bohlen, Dan (GE Aviation, US)
Sent: Wednesday, October 09, 2013 9:58 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Mesh Error Estimation
Yep, there's no magic bullet. We have a conservative method we use (short
of rerunning with a different mesh density.) It does give some false
positives (indicating the mesh is not converged  when is actually is).
Some of our team took it upon themselves to come up with a new method
(easier?, faster?, more accurate???) based on some energy error term (SERR?
They didn't really say) and run a bunch of our typical jet motor type
locations and come up with some normalized energy error criteria.
My put back to them based on the responses to this posting is why not do the
same semiempirical indicator using the what is already in Ansys (SMX SMXB)
that was put there as a mesh convergence indicator.
Thanks to all,
Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis
STAR review chairman, Fan and Booster
GE Aircraft Engines
1 Neumann Way
Evendale, OH 45215
Build 90 Col K1.5 cube 1N152
M/D H110 5132432366
Dial Comm *3322366
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf
Of Rod Scholl
Sent: Wednesday, October 09, 2013 10:30 AM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] Mesh Error Estimation
Sounds like we have similar approaches, Rahul. I recently gave some thought
to the "confidence interval" idea. I don't think it is workable
unfortunately:
In terms of statistics, confidence interval assumes some distribution of
variation (such as a "normal distribution")  then using the two data
points (one from node XYZ of element A, and the other from the element B
sharing this node) the idea would be to establish the likelihood (confidence
interval) that the converged value would be less than some selected or
calculated Sig_MAX, for example.
However, the converged stress would be different for a flat surface compared
to a fillet, even though the element A and element B differential might be
the same. This is a simple example of how the potential converged solution
depends on the geometry, and just the two values alone are not enough to
come up with a confidence interval... more information is needed. (which is
why this hasn't been done already).
What *can* be done, is for a given geometry, such as a 90degree fillet for
a 2D model (or unchanging in 3rd dimension) we *do* know how quickly the
mesh converges to the theoretical solution. So a confidence interval can be
calculated for a particular upper bound (be it SMXB or whatever we
choose)... what people have found is that 6 elements through the thickness
demarks a "high" confidence interval and this ruleofthumb is popular I've
found. But as soon as a 2nd order effect enters (like 3D stress state, body
loads, compound fillet, curvature in 3D, etc.) our relationship breaks down
and we're left without confidence interval.
Basically, if one has a well known geometry/load/3D effect we can save
ourselves the node count, mesh it coarsely and then use some previous
convergence study to get a decent prediction of the converged solution using
a fairly coarse model and the discretization difference between the two
elements (and even come up with a confidence interval). But geometry/loads
are rarely that clean/consistent (or we'd just use a KT chart and a radius!)
Hopefully I'm not soundinglecturey, just I went down this road thinking it
could be done, and realized we are stuck with things like PRERR,SEPC energy
comparisons. No simple answer or it woulda been programmed right in
already. We can chalk it up to "job security" :)
______________________________
Rod Scholl
Principal Analyst  Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com
Original Message
From: xansysbounces@xansys.org [mailto:xansysbounces@xansys.org] On Behalf
Of rahul.sangole
Sent: Wednesday, October 09, 2013 7:09 AM
To: xansys@xansys.org
Subject: Re: [Xansys] Mesh Error Estimation
I'm interested in this as well. Sounds like you want a confidence interval
on your stress values, as a function of mesh density.
I use a couple of ways to ensure appropriate mesh density in regions of
interest (I'm sure you're aware of these). These are just guidelines:
1. PRERR,SEPC < 15% for the entire model 2. PRERR,SEPC < 10% in local stress
region 3. PRERR,SEPC < 7% for 2 waves of elements from highest stress/strain
node 4. % difference between SMAXB and SMAX, or SMINB and SMIN < 7% for 2
waves of elements from highest stress/strain node
I don't use SDSG as much.

Rahul Sangole
Structural Analysis Group
Cummins Inc
++
 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 xansysmod@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 xansysmod@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 xansysmod@tynecomp.co.uk 
++
Post generated using Mail2Forum (http://www.mail2forum.com) 

Back to top 




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

