Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Problem with spring -- ansys APDL

  1. Feb 15, 2017 #1
    Hi,
    could you help me with my parametric model please? I have a problem with the end of spring. At the end of load (displacement) is problem with solve stress because there is concentrated stress and it shouldn't be. I didn't define contact between coils yet. I need to repair this fail at first. So if you could help me with to solve this problem it will be fine.

    Here is the code of the spring:

    !-----------------------
    ! POCATECNI PODMINKY
    !-----------------------
    finish
    /clear


    RADIUS=5 !Polomer pruziny [mm]
    ELEV=3 !Stoupani pruziny [mm]
    D=1.2 !Prumer dratu [mm]
    DIV=150 !Deleni pri sweepu
    YOUNG=210000 !Modul pruznosti v tahu [MPa]
    G=81500 !Modul pruznosti ve smyku [MPa]
    PI=3.141592653589793
    n=5 !Pocet cinnych zavitu [-]
    POSUV=500 !Stlaceni pruziny [mm]
    !FORCE=100 !Zatizeni pruziny [N]

    P=ELEV/(2*PI) !Stoupani na 1 rad
    P2=D/(2*PI)
    FI=atan(ELEV/(2*PI*RADIUS)) !Uhel stoupani pruziny [rad]
    PSI=atan(D/(2*PI*RADIUS)) !Uhel natoceni prurezu [rad]
    /prep7
    !--------------------
    ! PRVEK A MATERIAL
    !--------------------
    et,1,solid186 !Definuje prvni element
    et,2,plane183 !Definuje druhy element
    et,3,solid187 !Definuje treti element
    mp,ex ,1,YOUNG !Younguv modul
    mp,prxy,1,(YOUNG-2*G)/(2*G) !Poisson
    !---------------------------------------------------------------------------------------------------------
    ! TVORBA TELESA
    !---------------------------------------------------------------------------------------------------------
    !---------------------------------------
    !TVORBA POCATECNIHO ZAVERNEHO ZAVITU
    !---------------------------------------
    local,11,cylin,0,0,0,0,0,0,0,0 !Vytvori valcovy souradnicovy system pruziny
    csys,11 !Prepnuti do souradnicoveho systemu pruziny
    wpcsys,1,11 !Posune pracovni rovinu do souradneho systemu pruziny

    *do,i,1,8 !Vytvori body pro pocatecni uzavreny zavit
    k,i,RADIUS,(i-1)*45,P2*((i-1)/4)*PI
    *enddo

    *do,i,1,7 !Pospojuje body do sroubovice
    l,i,i+1
    *enddo

    lcomb,all !Vytvori strednici zaverneho zavitu

    local,12,cart,,,,,PSI*(180/PI)+90 !Vytvori system pro prurez dratu
    wpcsys,1,12 !Vytvori system pro prurez dratu

    cyl4,RADIUS,0,D/2 !Vytvori kruhovy prurez
    extopt,attr,0,0,1 !Zpusobi ze prurez se potahne kolmo ke strednici
    vdrag,1,,,,,,1 !Potahne prurez po sroubovici

    local,13,cart,0,0,(D/4)*cos(PSI) !Vytvori system pro srazeni zavitu
    wpcsys,1,13 !Vytvori system pro srazeni zavitu
    cyl4,0,0,RADIUS+D, , , ,-D !Vytvori valec

    vsbv,1,2, ,DELETE,DELETE !Provede rozdil teles
    ldele,1 !Odstrani puvodni strednici
    !---------------------------------------
    !TVORBA CINNYCH ZAVITU
    !---------------------------------------
    local,14,cylin,0,0,P2*(7/4)*PI,-45,0,0,0,0 !Vytvori valcovy souradnicovy system pruziny
    wpcsys,1,14 !Posune pracovni rovinu do souradneho systemu pruziny

    *do,i,1,2 !Vytvori body pro dokonceni zaverneho zavitu
    k,i+20*(n+3),RADIUS,(i-1)*45,P2*((i-1)/4)*PI
    *enddo

    *do,i,1,(n*8) !Vytvori body tvorici cinne zavity
    k,20*(n+3)+2+i,RADIUS,(i+1)*45,P*((i)/4)*PI+P2*(1/4)*PI
    *enddo

    k,20*(n+3)+3+n*8,RADIUS,(n*8+2)*45,P*(2*n)*PI+P2*(2/4)*PI

    *do,i,20*(n+3)+1,20*(n+3)+2+n*8 !Pospojuje body tvorici sroubovici
    l,i,i+1
    *enddo

    lsla,u !Odstrani z vyberu cary lezici na carach
    lcomb,all !Vytvori jednu sroubovici

    extopt,attr,0,0,1
    vdrag,6,,,,,,1 !Vytvori cinne zavity pruziny
    ldele,1 !Odstani puvodni strednici
    !---------------------------------------
    !TVORBA KONCOVEHO ZAVERNEHO ZAVITU
    !---------------------------------------
    local,15,cylin,0,0,n*ELEV+4*P2*PI,0,180,0,0,0 !Vytvori valcovy souradnicovy system pruziny
    csys,15 !Prepnuti do souradnicoveho systemu pruziny
    wpcsys,1,15 !Posune pracovni rovinu do souradneho systemu pruziny

    *do,i,1,8 !Vytvori body pro pocatecni uzavreny zavit
    k,i+30*(n+3),RADIUS,(i-1)*45,P2*((i-1)/4)*PI
    *enddo

    *do,i,1+30*(n+3),30*(n+3)+7 !Pospojuje body do sroubovice
    l,i,i+1
    *enddo

    lsla,u !Odstrani z vyberu cary lezici na carach
    lcomb,all !Vytvori jednu sroubovici

    local,16,cart,0,0,n*ELEV+4*P2*PI,180,-PSI*(180/PI)+90,180,0,0
    wpcsys,1,16
    cyl4,RADIUS,0,D/2 !Vytvori kruhovy prurez
    extopt,attr,0,0,1 !Zpusobi ze prurez se potahne kolmo k sroubovici
    vdrag,7,,,,,,1 !Potahne prurez po sroubovici

    local,17,cart,0,0,n*ELEV+4*P2*PI-(D/4)*cos(PSI),0,,180,0,0
    wpcsys,1,17 !Vytvori SS pro dokonceni zakonceni
    cyl4,0,0,RADIUS+D, , , ,-D !Vytvori valec
    vsbv,2,4, ,DELETE,DELETE !Provede rozdil teles
    nummrg,kp,1e-5 !Pospojuje keypointy
    !-------------------
    ! ZESITOVANI
    !-------------------
    vsel,s,,,1 !Vybere cinne zavity
    latt,1,,2
    extopt,esize,DIV,0 !Nastavi velikost elementu
    vsweep,1,6,5 !Provede sweep cinnymi zavity

    vsel,inve !Vybere zaverne zavity
    vatt,1,,3
    mopt,tetexpnd,1 !Definuje podminky pro mesh
    desize,3,1,50,8,13 !Nastavi velikosti
    vmesh,all !Provede zesitovani zavernych zavitu

    !-------------------
    ! KONTAKT
    !-------------------

    !-------------------
    ! OKRAJOVE PODMINKY
    !-------------------
    da,28,all,0 !Na konec pruziny definuje vetknuti
    da,16,uz,-POSUV !Na konec pruziny definuje deformacni podminku
    !-------------------
    ! RESENI
    !-------------------
    csys,1 !Prepnuti do cylindrickeho SS
    wpcsys,1,1 !Prepnuti do cylindrickeho SS
    /solu
    antype,static !Definice analyzy
    allsel,all !Vybere vsechno
    solve !Spusti reseni
    finish
    /post1

    plnsol,s,eqv,0,1.0 !Vykresli napeti podle podminky HMH
     

    Attached Files:

    • 1.png
      1.png
      File size:
      103.9 KB
      Views:
      45
    • 2.jpg
      2.jpg
      File size:
      46.7 KB
      Views:
      49
  2. jcsd
  3. Feb 15, 2017 #2

    Mech_Engineer

    User Avatar
    Science Advisor
    Gold Member

    It looks as though the geometry you have specified has a single point in the mesh near your boundary condition, which is in turn causing a stress discontinuity. I recommend re-visiting your mesh geometry or geometry creation to make sure you don't have any sharp corners or points, but even in that case if you're applying a fixed deformation at that surface your maximum stress will probably continue to show up in that region near the boundary condition.
     
  4. Feb 16, 2017 #3
    I tried to set a finer mesh but the maximum of nodes which I can use is only 32 000 because I have only student licence. I worked only with beams yet so I'm little bit confused. It's my first solid model which I need to my bachelor thesis. I tried to apply without fixed deformation a pressure but the solution was same. Someone said me that I should to turn on a midside nodes but when I tried it so I get only error. Is there any other way to define compression of spring? I know a lengths of spring like L0, L1, L8 and L9 so I need to define compression.
     
  5. Feb 17, 2017 #4

    Mech_Engineer

    User Avatar
    Science Advisor
    Gold Member

    What element type are you using? You'll need to use the appropriate element to allow use of mid-side nodes.

    Keep in mind that FEA models (especially ones with limited node/elements) will have both "real" and "artificial" stress concentrations. It's your job as an engineer to understand which is which, and have some justification as to why that is the case.
     
  6. Feb 17, 2017 #5
    Yes, I understand. But in my opinion in this area shouldn!t be stress concrentrations. For sweep I used solid 186 and last coil is meshed with solid187. I tried to mesh with mesh200 but it's not possible.
     
  7. Feb 17, 2017 #6

    Mech_Engineer

    User Avatar
    Science Advisor
    Gold Member

  8. Feb 17, 2017 #7
    Yes, I have. The sweep mesh is only on the portion of the spring which has a constant cross-section. Only the coil which have not a constant cross-section is meshed by free mesh.

    This is my mesh.
    a.png
     
    Last edited: Feb 17, 2017
  9. Feb 17, 2017 #8

    Mech_Engineer

    User Avatar
    Science Advisor
    Gold Member

    Nice work. What kind of boundary conditions are you applying to the spring to compress it?
     
  10. Feb 17, 2017 #9
    On one side I set all DOFS as zero and on second side I defined only uz. I can't apply pressure because I don't know but displacement I know.
     
  11. Feb 17, 2017 #10

    Mech_Engineer

    User Avatar
    Science Advisor
    Gold Member

    Your stress concentration in your mesh is expected, as it is a result of the flat grind on the end of the spring. Because the DOF's are set to zero at all nodes on that surface, the flexible element nearest the flat surface sees an abnormal amount of stress; in essence, it's like being welded to another infinitely rigid surface. A few options to reduce or eliminate this stress are:
    1. Get rid of the flat ground surfaces, constrain at the wire ends instead
    2. Use a flexible body to compress the spring with potentially non-linear boundary conditions
    3. Utilize a "compression only" support at the flat surfaces and then separately constrain rigid body motion using nodal supports at a few key vertices
    No amount of mesh optimization will completely eliminate this stress concentration, only increase the precision at which you're calculating the stress there. Does this make sense?
     
  12. Feb 17, 2017 #11
    Thank you for your tips, will try them out. Yes, it does.
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook

Have something to add?
Draft saved Draft deleted



Similar Discussions: Problem with spring -- ansys APDL
Loading...