-
-
August 25, 2023 at 8:09 pmMaralllSubscriber
Hello All,
My model is a 2d hollow semisphere. By writing an apdl code in ansys workbench, I defined the elastic modulus changes radially along the thickness of the hemisphere. Now I need to write a code to show me the contour of varaiation of elastic modulus along the thickness in my model. I would aprreciate any help!
Thank You,
Maral
-
August 29, 2023 at 2:21 pmAshish KhemkaForum Moderator
Hi,
Please see if the following link helps: variation of young modulus with the change in density of material? (ansys.com)
Regards,
Ashish Kumar
-
August 29, 2023 at 3:21 pmMaralllSubscriber
Thank you for your reply, Ashish.
I'm afraid this link doesn't help because I already applied the variable elastic modulus along the thickness through an APDL command in Ansys WB and I was able to get the results. However, I don't know how to PLOT the contour of variable elastic modulus on the body. When I use Material Plot, it showed me the default material properties (constant elastic modulus) instead of the variable elastic modulus. The code which is written under material, deletes the default material and assigns the variable elastic modulus to the elements (the valuse of elastic modulus varies radially). I need to see the contour plot of the values of the variable elastic modulus on the model.Â
I would appreciate any help.
Regards,
Maral
Â
-
August 29, 2023 at 4:56 pmdloomanAnsys Employee
There's no direct way. Two generic examples of an indirect way are below. Â
Method 1:
/post1Â
*get,ecount,elem,,count
emin=0
*do,iii,1,ecount,1
emin=elnext(emin)
!!! retrieve numerical value of EX for element emin as exval
detab,emin,EX_,exval
*enddo
pletab,EX_
2nd method based on temp-dep EX:
Â
!
set,last
!
*get,ecnt,elem,,count
*get,emax,elem,,num,max
*del,emmm,,nopr
*dim,emmm,'ARRAY',emax
etab,etemp,'BFE','TEMP'
ei=0
*do,i,1,ecnt
 ei=elnext(ei)
 *get,emno,'ELEM',ei,'ATTR','MAT'
 *get,itemp,'ELEM',ei,'ETAB',etemp
 *get,emmm(ei),'EX',emno,'TEMP',itemp
*enddo
*vput,emmm(1),'ELEM',1,'ETAB',etemp
eplot
/triad,lbot
/VIEW,1,1,1,1 Â Â
/ANG,1 Â
/auto,1
!
/SHOW,PNG,,0
/GFILE,1200,
Plet,etemp
/SHOW,CLOSEÂ -
September 6, 2023 at 6:20 pmMaralllSubscriber
Dear Dave,
Thank you for sending me this code.
I tried to apply the second method under solution but the result that I got is a contour plot of  variable elastic modulus which the maximum in the outer layer with the value which is obtained from the default value of the elastic modulus (that I had to defined in engineering data). However, I had added the command macro under the geometry to overwrite the default material data and the solution were done based on those new values of material data ( the elastic modulus as a function of radius(. So, I need to show those values of overrided elastic modulus on a contour plot-The values are changing from 0.02 to 0.25 MPa. How can I modify your code to make ansys to get the new material data not the default one? I would appreciate if you could help.
And, here is the code that solve the problem with the elastic modulus as a linear function of radius.
MPDELE, elastic,all
TBDELE,elastic,all
 csys,1
 esel, all
cm,remainingelem,elem
matid=1
*Do,ee,1,100000
*get,nextElem,ELEM,0,nxth
*get,elemxposition,ELEM,nextElem,cent,x
esel,r,cent,x,elemxpositionÂ
cm,elementXgroup,elem
*SET,x_pos,elemxposition
E_X=0.46*x_pos-2.74
 Tb,elastic,matid,,2,Isot
Tbdata,1,E_X,0.49
MPCHG,matID,all
*get,count_control,elem,,count
 cmsel,s,remainingelem
cmsel,u,elementXgroup
cm,remainingelem,elem
 *get,Element_count,elem,,count
 *if,element_count,eq,count_control,exit
 matid=matid+1
 *enddo
matid=matid+1
 *get,nextElem,ELEM,0,nxth
*get,elemxposition,ELEM,nextElem,cent,x
esel,r,cent,x,elemxpositionÂ
cm,elementXgroup,elem
 *SET,x_pos,elemxposition
E_X=0.46*x_pos-2.74
 Tb,elastic,matid,,2,Isot
Tbdata,1,E_X,0.49
 MPCHG,matID,all
esel,all
Â
Â
-
- The topic ‘Contour plot of elastic modulus’ is closed to new replies.
- Battery Simulation – Cannot access User-defined scalar (UDS) diffusivity
- Chemkin requires HPC
- acoustic structure coupling
- ANSYS Advanced Composite Cure Simulation full simulation Workshop issues
- Regarding the modal analysis of the hyperelastic material
- Doubt clarification on seed generation using ANSYS ADPL
- S-N (Wohler Graph) for steel X153CrMoV12 / D2 / NC11LV / K110 or similar
- Damping
- Material Designer: Meshing difficulties
- Calculate heating of an assembly for a given ambient temperature?
-
476
-
231
-
203
-
200
-
162
© 2024 Copyright ANSYS, Inc. All rights reserved.