Learning Forum

[2020221038]

Can you tell me how to extract the strain at the integration point of a shell element in ANSYS APDL?

[Akshat Gupta]

Hello,

You can use the command ERESX,no to copy the integration-point results to the nodes.

Reference:

https://ansyshelp.ansys.com/public/account/secured?returnurl=/Views/Secured/corp/v251/en/ans_cmd/Hlp_C_ERESX.html?q=eresx

Best,

Akshat

Introducing Ansys Assistant a 24/7 AI-powered virtual assistant for active Ansys academic customers.

[2020221038]

Thank you for your answer! This command copies the integration point results to the node. I want to see the strain of five integration points on the single shell element, not one.

[Akshat Gupta]

Hello,

Please have a look at the article mentioned below:

https://innovationspace.ansys.com/knowledge/forums/topic/how-can-i-get-displacements-stresses-and-plastic-strains-at-the-integration-points-for-a-shell-model-with-5-integration-points-through-the-thickness-2/

This should serve the purpose.

Thanks,

Introducing Ansys Assistant a 24/7 AI-powered virtual assistant for active Ansys academic customers.

[2020221038]

Based on what you and the article say, the results should be output. The list will only show the result for the top center bottom side (KEYOPT(8)). I can extract the top-bottom surface via shell command. But at the moment I can't extract the results for the other integration points.

[2020221038]

Thank you very much for your answer. The result of integration points can be obtained by OUTPR,ESOL command and ERESX command. I have output the result with outres,esol,last; OUTPR,ESOL ; ERESX,no command but how can I extract the result of integration point like beam element? The beam element can be used to extract the integration point results by using the following.
*GET, Par, SECR, n, Item1, IT1NUM, Item2, IT2NUM

[Akshat Gupta]

Hello,

With the 'OUTPR,ESOL,LAST', I am able to get the stresses as the integration points.

Sample Below.

Best,

Akshat

[2020221038]

Wow, you are showing this correctly, you have what I want. Can you send me the relevant commands to learn? I'm still not getting it right here.

FINISH$/CLEAR

/filname,00 SHELL

/PREP7!!

R0=1.0$H0=0.3$LH=2.0

ZJBH=0.05$GJJJ=0.1

ET,1,SHELL181

keyopt, 1, 8, 2

ET,2,MESH200,2 

MP,EX,1,3E10

MP,PRXY,1,0.2

MP,EX,2,2.1E11

MP,PRXY,2,0.30

MP,EX,3,2.06E11

MP,PRXY,3,0.3

 

!===============

SECTYPE,1,SHELL$SECDATA,H0, , , 5

K,1,R0-H0/2$K,2,R0-H0/2,,LH

K,3$K,4,,,LH$L,1,2

AROTAT,1,,,,,,3,4,90

AATT,1,,1,,1$ESIZE,0.04$AMESH,ALL

!----------

AG20=ACOS(-1)/4*20*20*1E-6!!!

AG6=ACOS(-1)/4*6*6*1E-6!!!

SECTYPE,2,REINF,DISC!!!!

SECDATA,2,AG20,MESH!!!!

SECTYPE,3,REINF,DISC!!!!

SECDATA,3,AG6,MESH

!----

LSEL,NONE!!!!!

K,1001,R0-H0+ZJBH,0,0

K,1002,R0-H0+ZJBH,0,LH

L,1001,1002!!

LGEN,2,ALL,,,H0-2*ZJBH

CSYS,1$LGEN,7,ALL,,,0,15

LATT,,,2,,,,2$LESIZE,ALL,,,1!!!

LMESH,ALL!-!!!

!----

LSEL,NONE$CSYS,1

K,2001,R0-H0+ZJBH

K,2002,R0-H0+ZJBH,90

K,2003,R0-ZJBH

K,2004,R0-ZJBH,90

L,2001,2002$L,2003,2004

CSYS,0

LGEN,1,ALL,,,0,0,GJJJ,,,1

LGEN,19,ALL,,,0,0,GJJJ

LATT,,,2,,,,3

ESIZE,0.10$LMESH,ALL

!--

ESEL,S,TYPE,,1!!--!

ESEL,A,TYPE,,2!!!

EREINF!

!!-----------------

ESEL,S,TYPE,,1!!!!

!/TRLCY,ELEM,0.92$ESEL,ALL

/ESHAPE,1$EPLOT!

 

lsel, s, loc, z, lh

sfl, all, pres, 10e6

lsel, s, loc, z, 0

nsll, s

d, all, all

 

/solu

allsel, all

 

antype,0

!nlgeom, on

outres,esol,last

OUTPR,ESOL 

ERESX,no 

autots,on

nsubst,10,500,10

neqit,100

!stat, inrtia

cnvtol,u,,0.05

cnvtol,f,-1

cnvtol,M,-1

solve

 

/post1

esel, s, , , 1

nsle, s

PRNSOL,S,PRIN   

 

 

OUTPR,ESOL,LAST

[Akshat Gupta]

Hello,

OUTPR is a solu command. So, you need to issue it before the solve.

https://ansyshelp.ansys.com/public/account/secured?returnurl=/Views/Secured/corp/v251/en/ans_cmd/Hlp_C_OUTPR.html?q=outpr

Thanks,

[2020221038]

Thank you very much for your positive answer. As you can see, in my command flow, I have set OUTPR,ESOL before solving

[Akshat Gupta]

Hello,

Yes, but before the solve it is given as OUTPR,ESOL. You should set it to OUTPR,ESOL,LAST.
Then it will print the quantities in the solve.out file.

Thanks,

[2020221038]

Can you tell me how to export the solve.out file? I try to export but I don't have your very perfect result.Thank you very much.

[2020221038]

Hello,but I don't have a solve.out file here.

[Akshat Gupta]

Hello,

You can have a look at jobname.out file in the solver directory. 

Do you see such file with .out extension in the directory?

Thanks,

 

[2020221038]

Thank you for your answer! I've looked at the working directory, but there are no such files with the .out extension.

[Akshat Gupta]

Ideally, due to the second command "/filname,00 SHELL", the jobname becomes 00SHELL, so you should see a file named 00SHELL.out in your directory. It is essentially the output file where we are also requesting printing of the ESOL via OUTPR command.

Maybe you can try removing that command once. What is the job name you have given in the execution line of APDL?

That name can be checked too. By default, APDL launcher takes 'file'.

Thanks,

[2020221038]

I reran it but there is no file in this format, and I have not seen this format during previous runs. Can you send me that command you ran to learn it?

[Akshat Gupta]

Hello,

Please make the following changes to the script.

Remove the /filname command from the second line.

Then add the /ouptut command under /solu.

Then outpr,esol,last and you will get the desired values in your output file (Specified via /Output command).

Example:

Thanks,

[2020221038]

Thank you very much for your reply, I have tested what you said and it still doesn't work. I have tested the /output position as well and it still doesn't work. Does this have anything to do with the High Performance Computing Setup? It seems to me that the previous files with output were using distributed computing.

FINISH$/CLEAR
!/filname,00 SHELL, 1
/PREP7!!

....

/solu
/output
allsel, all
antype,0
!nlgeom, on
ERESX,no 
autots,on
nsubst,10,500,10
neqit,100
!stat, inrtia
cnvtol,u,,0.05
cnvtol,f,-1
cnvtol,M,-1
outres,esol,last
OUTPR,ESOL,LAST
!/output
solve

or

/solu
!/output
allsel, all
antype,0
!nlgeom, on
ERESX,no 
autots,on
nsubst,10,500,10
neqit,100
!stat, inrtia
cnvtol,u,,0.05
cnvtol,f,-1
cnvtol,M,-1
outres,esol,last
OUTPR,ESOL,LAST
/output
solve

[2020221038]

When using distributed computing, there will indeed be out files, just records that can write the base information, but still no result output. There is a big gap with your output.

[Akshat Gupta]

Hello,

Can you try using the commands below with SMP

/CLEAR
/OUTPUT,TEST,OUT
/PREP7!!
R0=1.0$H0=0.3$LH=2.0
ZJBH=0.05$GJJJ=0.1
ET,1,SHELL181
keyopt, 1, 8, 2
ET,2,MESH200,2 
MP,EX,1,3E10
MP,PRXY,1,0.2
MP,EX,2,2.1E11
MP,PRXY,2,0.30
MP,EX,3,2.06E11
MP,PRXY,3,0.3
 
!===============
SECTYPE,1,SHELL$SECDATA,H0, , , 5
K,1,R0-H0/2$K,2,R0-H0/2,,LH
K,3$K,4,,,LH$L,1,2
AROTAT,1,,,,,,3,4,90
AATT,1,,1,,1$ESIZE,0.04$AMESH,ALL
!----------
AG20=ACOS(-1)/4*20*20*1E-6!!!
AG6=ACOS(-1)/4*6*6*1E-6!!!
SECTYPE,2,REINF,DISC!!!!
SECDATA,2,AG20,MESH!!!!
SECTYPE,3,REINF,DISC!!!!
SECDATA,3,AG6,MESH
!----
LSEL,NONE!!!!!
K,1001,R0-H0+ZJBH,0,0
K,1002,R0-H0+ZJBH,0,LH
L,1001,1002!!
LGEN,2,ALL,,,H0-2*ZJBH
CSYS,1$LGEN,7,ALL,,,0,15
LATT,,,2,,,,2$LESIZE,ALL,,,1!!!
LMESH,ALL!-!!!
!----
LSEL,NONE$CSYS,1
K,2001,R0-H0+ZJBH
K,2002,R0-H0+ZJBH,90
K,2003,R0-ZJBH
K,2004,R0-ZJBH,90
L,2001,2002$L,2003,2004
CSYS,0
LGEN,1,ALL,,,0,0,GJJJ,,,1
LGEN,19,ALL,,,0,0,GJJJ
LATT,,,2,,,,3
ESIZE,0.10$LMESH,ALL
!--
ESEL,S,TYPE,,1!!--!
ESEL,A,TYPE,,2!!!
EREINF!
!!-----------------
ESEL,S,TYPE,,1!!!!
!/TRLCY,ELEM,0.92$ESEL,ALL
/ESHAPE,1$EPLOT!
 
lsel, s, loc, z, lh
sfl, all, pres, 10e6
lsel, s, loc, z, 0
nsll, s
d, all, all
 
/solu
allsel, all
OUTPR,ESOL,LAST
 
antype,0
!nlgeom, on
outres,esol,last
ERESX,no 
autots,on
nsubst,10,500,10
neqit,100
!stat, inrtia
cnvtol,u,,0.05
cnvtol,f,-1
cnvtol,M,-1
solve
 

Please try this and let me know.

Thanks,

[2020221038]

Hello! I noticed that the out file results do not include the principal stress results, only the results below, but there is no relevant explanation in the esol documentation.
“S”     Stresses (11,22,33,12,23,13)
“EPTO”  Strains  (11,22,33,12)
“EPEL”  StrainsEL(11,22,33,12)

My structure is cylindrical, and I want to extract the radial strain and principal stress at the integration point.

 

[2020221038]

I ran the command you posted and it automatically generated the out file. In the help it mentions：By issuing the /OUTPUT command before SOLVE, you can divert the output to a file instead of the screen.

However, in the solution phase, performing /output before solving doesn't result in an out file, only in the preprocessor phase?