XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Transient thermal analysis of SAW
 
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
arpan.mondal
User


Joined: 19 Aug 2013
Posts: 3

PostPosted: Fri Jun 20, 2014 2:50 am  Reply with quote

Hello Everyone

I am working on transient thermal analysis of SAW with gaussian distribution heat source model.I need to move the local CSYS also.I am facing some problems as my heat source is not moving while simulating though the load step files have already been read with a solution.I am getting 2 warning messages.These are :

1)Both solid model and finite element model boundary conditions have been
applied to this model. As solid loads are transferred to the nodes or
elements, they can overwrite directly applied loads.

2)A reference heat flow value times the tolerance is used by the
Newton-Raphson method for checking convergence. The calculated
reference HT FLOW CONVERGENCE VALUE= 2.842665544E-14 is less than a
threshold. This threshold defaults to 1.0e-6 or is specified as
MINREF on the CNVTOL command. Check results carefully

And my code is as follows:

*ask,q,Input the value of Total Heat Input energy of arc,1500
*ask,R,Input the value of Heat Source Radius,0.003
*ask,VELOCITY,Input the value of line velocity,5

Q=((3*q)/3.14*(R**2))*EXP(((-3)*r**2)/(R**2))
nropt,full ! Newton Raphson = full
trnopt,full
lumpm,0
TIME_NOW=0
*do,I,1,15,1
TIME_STEP = 13.33/VELOCITY
LOCAL,11,0,0,(i-1)/70,0,,,
CSYS,11
ALLSEL,ALL

!LS-I
ASEL,ALL
ASEL,S,AREA,,2,2,,0
ESEL,ALL
ESEL,S,ELEM,,608,613
SFE,ALL,,HFLUX,Q,,,
AUTOTS,ON
DELTIM,TIME_STEP/5,,,0
KBC,1
TIME_NOW = TIME_NOW + TIME_STEP
TIME,TIME_NOW
LSWRITE,I
CSDELE,ALL !delete previous coordinate system
ESEL,ALL !select all elements
SFEDELE,ALL,,HFLUX
*ENDDO


Please check and waiting for proper suggestions....
Thank you




-------------------------------------------------------------------------------------
Arpan Kumar Mondal
Research Scholar
Department of Mechanical Engineering
Indian Institute of Technology(IIT),Guwahati
Back to top
View user's profile Send private message
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Fri Jun 20, 2014 7:08 am  Reply with quote

Arpan

I have moved heat fluxes before using the coordinate system, but it was in conjunction with a table. The last parameter in the *DIM connects the table to the coordinate system 11

*dim,hfx,table,3,,,x,,,11
*SET,hfx(1,0),-2,1e-6,2
*SET,hfx(1,1),.001,10,.001

Apply the heat flux to all elements in the path (sf,all,hflux,%hfx%)


When this approach is taken, the cycle is

Move the coordinate system to the new location (local,11,0,new_location)
Time,New_time
Solve

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of arpan.mondal
Sent: Friday, June 20, 2014 5:51 AM
To: xansys@xansys.org
Subject: [Xansys] Transient thermal analysis of SAW

Hello Everyone

I am working on transient thermal analysis of SAW with gaussian distribution heat source model.I need to move the local CSYS also.I am facing some problems as my heat source is not moving while simulating though the load step files have already been read with a solution.I am getting 2 warning messages.These are :

1)Both solid model and finite element model boundary conditions have been applied to this model. As solid loads are transferred to the nodes or elements, they can overwrite directly applied loads.

2)A reference heat flow value times the tolerance is used by the
Newton-Raphson method for checking convergence. The calculated
reference HT FLOW CONVERGENCE VALUE= 2.842665544E-14 is less than a
threshold. This threshold defaults to 1.0e-6 or is specified as
MINREF on the CNVTOL command. Check results carefully

And my code is as follows:

*ask,q,Input the value of Total Heat Input energy of arc,1500 *ask,R,Input the value of Heat Source Radius,0.003 *ask,VELOCITY,Input the value of line velocity,5

Q=((3*q)/3.14*(R**2))*EXP(((-3)*r**2)/(R**2))
nropt,full ! Newton Raphson = full
trnopt,full
lumpm,0
TIME_NOW=0
*do,I,1,15,1
TIME_STEP = 13.33/VELOCITY
LOCAL,11,0,0,(i-1)/70,0,,,
CSYS,11
ALLSEL,ALL

!LS-I
ASEL,ALL
ASEL,S,AREA,,2,2,,0
ESEL,ALL
ESEL,S,ELEM,,608,613
SFE,ALL,,HFLUX,Q,,,
AUTOTS,ON
DELTIM,TIME_STEP/5,,,0
KBC,1
TIME_NOW = TIME_NOW + TIME_STEP
TIME,TIME_NOW
LSWRITE,I
CSDELE,ALL !delete previous coordinate system
ESEL,ALL !select all elements
SFEDELE,ALL,,HFLUX
*ENDDO


Please check and waiting for proper suggestions....
Thank you




-------------------------------------------------------------------------------------
Arpan Kumar Mondal
Research Scholar
Department of Mechanical Engineering
Indian Institute of Technology(IIT),Guwahati






+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| 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
arpan.mondal
User


Joined: 19 Aug 2013
Posts: 3

PostPosted: Fri Jun 20, 2014 10:36 am  Reply with quote

Thank you mike for your suggestion..but I dont want to use table for defining heat flux equation.What I am willing to do is directly apply the heat flux on the selected elements/nodes and make it to move along with the moving coordinate system.

And is node selection is compulsary for providing the heat flux ? or we can select a group of elements and apply heat flux on them ?

Thank You




-------------------------------------------------------------------------------------
Arpan Kumar Mondal
Research Scholar
Department of Mechanical Engineering
Indian Institute of Technology(IIT),Guwahati
Back to top
View user's profile Send private message
mike.yaksh
User


Joined: 05 Feb 2009
Posts: 291

PostPosted: Fri Jun 20, 2014 11:30 am  Reply with quote

Arpan

I use the active nodes to define the surface. There are a number of ways. You could get all the nodes on the surface and then select the elements for that load step and use sf,all,hflux,value. Then before the solve make the entire model active. How are you applying the heat load; KBC,1 or KBC,0?

Mike Yaksh
NAC International
Norcross GA

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of arpan.mondal
Sent: Friday, June 20, 2014 1:36 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Transient thermal analysis of SAW

Thank you mike for your suggestion..but I dont want to use table for defining heat flux equation.What I am willing to do is directly apply the heat flux on the selected elements/nodes and make it to move along with the moving coordinate system.

And is node selection is compulsary for providing the heat flux ? or we can select a group of elements and apply heat flux on them ?

Thank You




-------------------------------------------------------------------------------------
Arpan Kumar Mondal
Research Scholar
Department of Mechanical Engineering
Indian Institute of Technology(IIT),Guwahati






+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| 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
summer.shen
User


Joined: 14 May 2014
Posts: 53
Location: Shanghai, China

PostPosted: Fri Jun 20, 2014 6:59 pm  Reply with quote

Hi Mike,

I guess I am doing a similar job as you described above. Here is how I do it:
1), define a center point (xc,yc,zc) of the heat flux.
2), define a table for the gaussian distribution around (xc,yc,zc)
3), apply boundary conditions and solve
4), move the point xc=xc+xstep, yc=yc+ystep, zc=zc+zstep
5), re-define the heat flux table around new center (xc,yc,zc)
```
To define the heat flux distribution, I use a coordinate attached to the center point (using the LOC command). So if the center points moves, the table need to be updated for each step.

Basically, the program looks like this:
xc=x0
yc=y0
zc=z0 !origin

*do,istep,1,n,
loc,11,1,xc,yc,zc !cylindrical coordinate
*dim,xarr,array,nxx !for hflux table
*dim,yarr,array,nyy !for hflux table
*dim,fluxtable,table,nxx,nyy,,x,y,,11 !hflux table
...apply other boundary conditions and constraints...
time,loadtime
solve
xc=xc+xstep
yc=yc+ystep
zc=zc+zstep
...
*enddo

Hope this can help.




arpan.mondal wrote:
Thank you mike for your suggestion..but I dont want to use table for defining heat flux equation.What I am willing to do is directly apply the heat flux on the selected elements/nodes and make it to move along with the moving coordinate system.

And is node selection is compulsary for providing the heat flux ? or we can select a group of elements and apply heat flux on them ?

Thank You




-------------------------------------------------------------------------------------
Arpan Kumar Mondal
Research Scholar
Department of Mechanical Engineering
Indian Institute of Technology(IIT),Guwahati

_________________
Summer Shen
--
MSc,Shanghai Jiao Tong University
Dongchuan Rd. 800, Shanghai, China. 200240
Laser cladding
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