Learning Forum

[muhammadaziz.sarwar]

I am working on 11 layer rubber pipe with 4 layers of steel wire arranged at particular helix angle in Mechanical APDL2024.I want to model these wires as reinforcements with other layers as rubber material.I am thinking that smeared reinforcing section would be good,as only one type of steel wire is used and at same distance from each other.I am attaching the 90 sector model of pipe with one end closed.Please recommend which type of reinforcing and options ccould be used to model this pipe. I want to apply reinforcement only on V1 .I am available for more information.I tried different options on reinforcing section .But model is giving same deformation with or without reinforcement.I have also studied REINF263,REINF264 and REINF265.But i have not succeded to apply to my model.Please share more information for applying reinforcement at particular angle for each layer.

[Ashish Khemka]

Hello,

Please see if the following link helps: 14.1. Reinforcing Workflow (ansys.com)

Regards,

Ashish Khemka

[muhammadaziz.sarwar]

Thanks for your information.Unfortunately problem is still there beacuse of contact and particular angle requirements and continuity of the mesh..Could you please expalin any other option ?

 

[wrbulat]

Volume 1 appears to be subdivided (sliced) in such a way that there is a fairly sharp angle between the plane of the cut and the inner cylindrical surface. For what reason is the the geometry subdivided in this way? You mentioned contact. Is there contact between one of the surfaces on the right end of the reinforced pipe, with the pipe subjected to an axial load? Did you end up meshing with tetrahedra? If the subdivision was made to clearly define contact surface, I think you can do away with it... the pressure distribution from the contacting body (if you model it explicity) should be fairly well represented.

There are multiple options for defining smeared reinforcing. I believe that in the option you are using, the location and orientation of the fibers is defined with respect to the order of nodes in each element:

If you have a tetrahedral mesh, with random node number order within each element and multiple layers of elements through the thickness of the pipe wall, you might end up with a corresponspondingly random reinforcing locations and orientations.

I can offer you the following (copy the lines below into a text file and read the text file into MAPDL with the /INPUT command). Try two different values of parameter r_reinf (0.001 & 0.0005). The calculated results should differ substantially. I have the luxury of using very simple geometry (not sliced as yours is). Even with this "unfair advantage", I had to resort to a "trick" to align my SOLID185 elements (initially define them to be layered so I could use EORIENT to renumber the elements in such a way as to get consistent REINF265 orientation in the cylinder wall). I added comments to explain the numerous other settings I used in the setup.

Another option would be to create MESH200 elements and assign the reinf section properties to them.

 

I hope this helps!

Bill

 

 

fini

/cle

 

/sys,del file*.png

 

/vie,1,1,1,1

/vup,1,z

 

 

C********************************************************

C*** PARAMETERS

C********************************************************

pi=acos(-1)

 

r1=0.010 ! CYLINDER INNER RADIUS

r2=0.020 ! CYLINDER OUTER RADIUS

l=0.01 ! CLINDER LENGTH

 

r_reinf=0.001 ! REINFORCING FIBER RADIUS (COMPARE 0.001 & 0.0005)

a=pi*r_reinf**2 ! CORRESPONDING REINF CROSS SECTION AREA

facenum=3 ! FACE NUMBER FOR "ELEF" REINF SECTION PARAMETER

s=0.0025 ! REINF SPACING

thta=30 ! MAGNITUDE OF REINF FIBER ORIENTATION ANGLE

 

E_base=0.05e9 ! BASE ELEMENT ELASTIC MODULUS (~RUBBER)

nu_base=0.20 ! BASE ELEMENET POISSON'S

 

E_reinf=2e11 ! REINF ELASTIC MODULUS

nu_reinf=0.20 ! REINF POISSON'S

 

u_top=0.001 ! MAGNITUDE OF AXIAL DISPLACEMENT IMPOSED ON CYLINDER IN TRIAL SOLVE

f_top=2e3 ! MAGNITUDE OF AXIAL FORCE IMPOSED ON CYLINDER IN TRIAL SOLVE

 

 

/title,R_fiber=%r_reinf%, S_fiber=%s%, E_fiber=%E_reinf%

 

C********************************************************

C*** GEOMETRY & BASE ELEMENT MESH

C********************************************************

wpcs,-1,0 ! CYLINDRICAL ELEMENT COORDINATE SYSTEM

cswp,11,1

 

/prep7 ! GEOMETRY (FOUR 90 DEG SECTORS)

cyli,r1,r2,0,l,0,90

cyli,r1,r2,0,l,90,180

cyli,r1,r2,0,l,180,270

cyli,r1,r2,0,l,270,360

numm,kp ! MERGE COINCIDENT KEYPOINTS

vatt,1,1,1,11 ! ASSIGN ATTRIBUTE NUMBERS (MAT, REAL, TYPE, ESYS)

 

et,1,185,,,1 ! LAYERED SOLID185 ELEMENT TYPE

mp,ex,1,E_base ! ELASTIC MODULUS

mp,nuxy,1,nu_base ! POISSON'S

vmes,all ! MESH VOLUMES

 

 

C********************************************************

C*** REORIENT BASE ELEMENTS

C********************************************************

eorient,lysl,posz ! RENUMBER SO THAT FACE 1 IS PARALLEL +Z ESYS AXIS

 

 

C********************************************************

C*** REINFORCING ELEMENT PROPERTIES

C********************************************************

mp,ex,2,E_reinf ! ELASTIC MODULUS

mp,nuxy,2,nu_reinf ! POISSON'S

 

sect,2,reinf,smear ! REINF SECTION FOR INNER RADIUS

secd,2,A,s,,thta,elef,facenum,0.5

seccontrol,0,1,3 ! REMOVE BASE MATERIAL IN DOMAIN OCCUPIED BY REINFORCING, INCLUDE TRANSVERSE SHEAR & BENDING

 

sect,3,reinf,smear ! REINF SECTION FOR OUTER RADIUS

secd,2,A,s,,-thta,elef,facenum,0.5

seccontrol,0,1,3 ! REMOVE BASE MATERIAL IN DOMAIN OCCUPIED BY REINFORCING, INCLUDE TRANSVERSE SHEAR & BENDING

 

 

C********************************************************

C*** CREATE REINFORCING ELEMENTS

C********************************************************

csys,11 ! DETERMINE INNER/OUTER RADII

*get,rmin,node,,mnloc,x

*get,rmax,node,,mxloc,x

 

nsel,s,loc,x,rmin ! REINFORCE BASE ELEMENTS ON INNER RADIUS

esln

esel,r,type,,1

nsle

secn,2

ereinf

 

nsel,s,loc,x,rmax ! REINFORCE BASE ELEMENTS ON OUTER RADIUS

esln

esel,r,type,,1

nsle

secn,3

ereinf

 

 

C********************************************************

C*** MAKE BASE ELEMENT HOMOGENEOUS, PLOT ELEMENTS

C********************************************************

et,1,185 ! CHANGE BASE ELEMENT TYPE FROM LAYERED TO HOMOGENEOUS OPTION

 

esel,s,type,,1 ! MAKE BASE ELEMENTS TRANSLUCENT

/trlcy,elem,0.9

alls

/psy,layr,-1 ! DISPLAY LAYERS (REINFORCING)

/esh,1

/dev,vect,0 ! RASTER FILL DISPLAY

eplo ! PLOT ELEMENTS

/sho,png $eplo $/sho,close $/wait,2

 

esel,s,type,,2 ! SELECT REINFORCING ELEMENTS

/dev,vect,1 ! WIRE FRAME DISPLAY

eplo ! PLOT ELEMENTS

/sho,png,,1 $eplo $/sho,close $/wait,2

 

/dev,vect,0 ! REVERT TO RASTER FILL

esel,s,type,,1 ! MAKE BASE ELEMENTS OPAQUE

/trlcy,elem,0

alls

 

fini

 

 

C********************************************************

C*** TRIAL SOLVE

C********************************************************

/solu

 

nlgeom,on ! MAY BE NECESSARY TO INVOKE TENSION-ONLY REINF BEHAVIOR

 

autots,off

outr,all,all

 

nsel,s,loc,z ! FIX BASE

d,all,all

 

nsel,s,loc,z,l

cp,1,uz,all

nd_top=ndnext(0)

 

alls

 

!d,nd_top,uz,u_top ! TENSION ON TOP SURFACE

f,nd_top,fz,f_top ! TENSION ON TOP SURFACE

nsub,5

solv

 

!d,nd_top,uz,-u_top ! COMPRESSION ON TOP SURFACE

f,nd_top,fz,-f_top ! COMPRESSION ON TOP SURFACE

nsub,10

solv

 

fini

 

 

C********************************************************

C*** POST PROCESSING

C********************************************************

 

/post26

!rfor,2,nd_top,f,z

nsol,2,nd_top,u,z

/axl,y,Axial Displacement

plva,2

/sho,png $plva,2 $/sho,close $/wait,2

 

 

/post1

set,1

 

esel,s,ename,,265

ples,s,x

/sho,png $ples,s,x $/sho,close $/wait,2

 

esel,s,ename,,185

rsys,1

plns,s,z

/sho,png $plns,s,z $/sho,close $/wait,2

 

[muhammadaziz.sarwar]

Thank you so much. I have applied your model to check .But problem for me is angle of reinforcement should be 54.04 to 54.103. and area of cross section should be 0.02. and i  am not sure about the contact.I have total 11 layers of steel and rubber (among 4 of them were steel reinforcements at particular angle and i am not sure about distance)I want to see as well reinforcement like steel wire at helix.

I believe this approach is really good.It can save simulation cost and can be easily edited fior future use.when i am trying to change the angle and area of cross section it shows different style of reinforcements.

Could you please guide me is this reinforcing method can be applied to hydraulic hoses as shared above.If yes could you please guide me regarding reinforcing sections and data.For meshing any meshing can be used around 6mm thickness of pipe but  because of different material involved we just need contact and correct result for deformation.Thanks again.