XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[other] An observation in Thermal/Strl transient analysis !!
 
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
debabrata.podder
User


Joined: 21 Feb 2013
Posts: 51
Location: NIT Meghalaya, India

PostPosted: Mon Oct 07, 2013 4:39 pm  Reply with quote

Dear experts,
I am doing an arc welding analysis. The material properties in the thermal analysis I have taken in a range of 20 - 3500 deg C. After completion of the thermal analysis, the maximum temperature is generating around 2500 deg C. To do the structural analysis, I have imported (LDREAD) thermal loads to structural. For structural analysis, I have taken a material property range of 20 -1500 deg C. Interestingly, if I consider the structural material properties in a range of 20 - 3500 deg C, the programme is crushing, saying some elements have highly distorted ! But if I consider the structural material property in a range of 20- 1500 deg C, then the programme is running without any disturbance. And after running my structural model I have compered my results with the experiment, and they are quite similar. Is my approach of doing structural analysis is wrong !! One more thing, when I am importing the thermal loads to structural, the maximum temperature there is around 2500 deg C, but when I am doing the structural analysis I am using material properties only upto 1500 deg C. What about the other elements which have gained temperature more than 1500 deg C ?? What structural material properties are assigned to them !!! Is it forcefully assigning structural material properties upto 1500 deg C range (which I have taken) on those higher (>1500 deg C) temperature elements also ??? Why the program is crushing then, if I use a range of structural material properties of range 20 - 3500 deg C ??? Can anyone explain !! Thanks in advance.

Regards-
_________________
Debabrata Podder(PhD)
Assistant Professor
NIT Meghalaya
India
Back to top
View user's profile Send private message
Martin Liddle
User


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

PostPosted: Tue Oct 08, 2013 3:53 am  Reply with quote

On 08/10/2013 00:39, debabrata.podder wrote:
Quote:
when I am doing the structural analysis I am using material properties only upto 1500 deg C. What about the other elements which have gained temperature more than 1500 deg C ??

Material properties for elements with a temperature higher than the
maximum provided temperature dependent material property will be
determined by extrapolation using (I think) the last two specified data
points.


--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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
debabrata.podder
User


Joined: 21 Feb 2013
Posts: 51
Location: NIT Meghalaya, India

PostPosted: Tue Oct 08, 2013 5:19 am  Reply with quote

Thank you Mr. Martin for your time. According to your explanation, if my obtained temperature from thermal analysis is 2500 deg C, and if the last two data points in structural analysis is 800 deg C and 1500 deg C, then it will be extrapolated from this two. Then my question is, if it can calculate (program not crushing !)in the range of 2500 deg C, then why it can't (program crushing !) in the range 3500 deg C ?? In both the cases, though the value of thermal strain (alpha* delta-t) will be the same (I think) though (because in both cases obtained temperature from thermal is same,2500 deg. So in both cases, thermal strain will be, alpha * (2500-20); Only the supplied temperature range is more than the obtained one !!). Is it because of the alpha value (is the extrapolated alpha value is less than my provided value @ higher temperature !!!)Why it is crushing then !!!
Thanks in advance.
_________________
Debabrata Podder(PhD)
Assistant Professor
NIT Meghalaya
India
Back to top
View user's profile Send private message
Martin Liddle
User


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

PostPosted: Tue Oct 08, 2013 6:42 am  Reply with quote

On 08/10/2013 13:19, debabrata.podder wrote:
Quote:
According to your explanation, if my obtained temperature from thermal analysis is 2500 deg C, and if the last two data points in structural analysis is 800 deg C and 1500 deg C

If you read Joe Metrisin's comment you will see that what I said was wrong.


--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Oct 08, 2013 10:00 am  Reply with quote

On Oct 8, 2013, at 7:19 AM, debabrata.podder wrote:

Quote:
Thank you Mr. Martin for your time. According to your explanation,
if my obtained temperature from thermal analysis is 2500 deg C
Were you aware that the liquidus of the iron-carbon system is less
that 2000C? Your thermal analysis indicates that part of your model
should be dripping to the floor.

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/

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


Joined: 21 Oct 2008
Posts: 91

PostPosted: Tue Oct 08, 2013 11:35 am  Reply with quote

But when you look at the plot it's not dripping. Must be a bug.

David Stapp
Peregrine Consulting, Inc.

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf
Of Christopher Wright
Sent: Tuesday, October 08, 2013 1:00 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] [other] An observation in Thermal/Strl transient
analysis !!


On Oct 8, 2013, at 7:19 AM, debabrata.podder wrote:

Quote:
Thank you Mr. Martin for your time. According to your explanation, if
my obtained temperature from thermal analysis is 2500 deg C
Were you aware that the liquidus of the iron-carbon system is less that
2000C? Your thermal analysis indicates that part of your model should be
dripping to the floor.

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/



+-------------------------------------------------------------+
| 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
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Oct 08, 2013 11:39 am  Reply with quote

On Oct 8, 2013, at 1:35 PM, David S Stapp wrote:

Quote:
But when you look at the plot it's not dripping. Must be a bug.
One of those ANSYS problems that actually turns out to be an
engineering problem.

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/

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


Joined: 31 Jul 2009
Posts: 23

PostPosted: Tue Oct 08, 2013 12:07 pm  Reply with quote

Debabrata,

I assume that when you derived properties at 3500C, the coefficient of thermal expansion (Alpha) is higher than that at 1500C? ANSYS does not limit the import temperature (T) values, nor does it extrapolate properties that exceed the input range.

So with the same Delta_T, the thermal strain would be higher for the 3500C property set than the thermal strain for the 1500C property set. This may be the reason for the excessive element distortion when using the 3500C property set.


Francis Ku
Senior Consultant
Structural Integrity Associates, Inc.
San Jose, CA
USA



-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of debabrata.podder
Sent: Monday, October 07, 2013 4:39 PM
To: xansys@xansys.org
Subject: [Xansys] [other] An observation in Thermal/Strl transient analysis !!

Dear experts,
I am doing an arc welding analysis. The material properties in the thermal analysis I have taken in a range of 20 - 3500 deg C. After completion of the thermal analysis, the maximum temperature is generating around 2500 deg C. To do the structural analysis, I have imported (LDREAD) thermal loads to structural. For structural analysis, I have taken a material property range of 20 -1500 deg C. Interestingly, if I consider the structural material properties in a range of 20 - 3500 deg C, the programme is crushing, saying some elements have highly distorted ! But if I consider the structural material property in a range of 20- 1500 deg C, then the programme is running without any disturbance. And after running my structural model I have compered my results with the experiment, and they are quite similar. Is my approach of doing structural analysis is wrong !! One more thing, when I am importing the thermal loads to structural, the maximum temperature there is around 2500 deg C, b ut when I am doing the structural analysis I am using material properties only upto 1500 deg C. What about the other elements which have gained temperature more than 1500 deg C ?? What structural material properties are assigned to them !!! Is it forcefully assigning structural material properties upto 1500 deg C range (which I have taken) on those higher (>1500 deg C) temperature elements also ??? Why the program is crushing then, if I use a range of structural material properties of range 20 - 3500 deg C ??? Can anyone explain !! Thanks in advance.

Regards-

------------------------
Debabrata Podder
Research Scholar
IIT Kharagpur
PIN NO.: 721302
India






+-------------------------------------------------------------+
| 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
debabrata.podder
User


Joined: 21 Feb 2013
Posts: 51
Location: NIT Meghalaya, India

PostPosted: Tue Oct 08, 2013 5:21 pm  Reply with quote

@ Mr. Francis:
Quote:
ANSYS does not limit the import temperature (T) values, nor does it extrapolate properties that exceed the input range.


Thanks Mr. Francis for your time. If Ansys can't extrapolate the properties that exceeds the input range, then what properties are assigned to those elements, which have temperature more than the provided value !!!

@ Mr. Wright: Thanks Mr. Wright for reply. Yes I am aware that the iron-carbon system has liquids temp less that 2000C .
Quote:
Your thermal-analysis indicates that part of your model should be
dripping to the floor.
What you meant by this !!

Regards-
_________________
Debabrata Podder(PhD)
Assistant Professor
NIT Meghalaya
India
Back to top
View user's profile Send private message
francis.ku
User


Joined: 31 Jul 2009
Posts: 23

PostPosted: Wed Oct 09, 2013 7:39 am  Reply with quote

ANSYS uses the properties at the last temperature point, for the 1500C set it will be at 1500C.


Francis Ku
Senior Consultant
Structural Integrity Associates, Inc.
San Jose, CA
USA



-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of debabrata.podder
Sent: Tuesday, October 08, 2013 5:22 PM
To: xansys@xansys.org
Subject: Re: [Xansys] [other] An observation in Thermal/Strl transient analysis !!

@ Mr. Francis:
Quote:
ANSYS does not limit the import temperature (T) values, nor does it extrapolate properties that exceed the input range.


Thanks Mr. Francis for your time. If Ansys can't extrapolate the properties that exceeds the input range, then what properties are assigned to those elements, which have temperature more than the provided value !!!

@ Mr. Wright: Thanks Mr. Wright for reply. Yes I am aware that the iron-carbon system has liquids temp less that 2000C .

Quote:
Your thermal-analysis indicates that part of your model should be
dripping to the floor.
What you meant by this !!

Regards-

------------------------
Debabrata Podder
Research Scholar
IIT Kharagpur
PIN NO.: 721302
India






+-------------------------------------------------------------+
| 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
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Wed Oct 09, 2013 10:17 am  Reply with quote

On Oct 8, 2013, at 7:21 PM, debabrata.podder wrote:

Quote:
Quote:
Your thermal-analysis indicates that part of your model should be
dripping to the floor.
What you meant by this !!

The material becomes liquid at the liquidus, and no longer behaves as
a solid. In particular it no longer supports tension or shear. As a
result it runs something like melted wax. Your model is nonsense at
such temperatures.

At the risk of repeating myself, you might get a lot more help if
you'd explain what result you're trying for and what your physical
understanding of the behavior might be. Just saying that you're
'doing an arc welding analysis' is pointless.

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/

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


Joined: 21 Feb 2013
Posts: 51
Location: NIT Meghalaya, India

PostPosted: Wed Oct 09, 2013 10:55 am  Reply with quote

Thanks again for your time Mr. Wright. So as per your explanation, if my model drips to the floor in liquid-temperature, then simply what-is-happening ? Am I not getting the right calculation (by ANSYS) at that moment ? But how I am getting a similar pattern-of-residual-stress with the experiment data !! Is the error of margin is very less then !! If not, then how to rectify that ? I am also curious to know, if my provided temperature range in-mechanical-analysis is less than the obtained temperature, then what material property ANSYS is using for those-high-temperature elements!!
By the way I am using a double ellipsoidal Goldak heat source to generate the heat and using element-birth-and-death to simulate the weld metal deposition. I am assuming that the weld bead materials are comming to live in the zone of heat flux radius. But that should not be the real logic I feel. They should come to live if their temperature reaches less than solid temperature (1495 deg C).
Thanks in advance.
_________________
Debabrata Podder(PhD)
Assistant Professor
NIT Meghalaya
India
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