Learning Forum

[hajar.rhylane]

Dear community, I need your support about my simulation.

I want to analyse the contact between a rolling wheel and rail as it is shown in the picture using ANSYS APDL but my results are not as was expected like specially the repartition of the stick and slip zones which is given in APDL by contact status. i don't know why there is no stick zone in the contact patch ? the contact status indicates always that the wheel is in sliding status even when the wheel is not moving. Please let me know if you have any suggestions or corrections to my issue ????????????????????????. The contact is frictionnal and symmetric. 

To simulate the rolling motion of a loaded wheel, I defined three steps:

-step1: the bottom side of the rail is fixed and symmetry boundary conditions are applied to the left side of the wheel and rail.

-step2: the symmetry bcs are removed from the left side of the wheel and the the pilot node is free to move in vertical direction . the load (FZ=-75000N) is applied to the pilot node

- step4 : translation velocity (Vx=50km/h) and angular velocity (Omgy)and are applied at the pilot node.

 

Here is the code corresponding to these load steps:

 

!Clamp the rail bottom

asel,s,area,,42

da,all,all  

allsel,all

 

! Constrain symmetrical plane

asel,s,area,,17

asel,s,area,,37

asel,a,area,,40

da,all,UX 

da,all,Uy 

 

!fix the pilot node

D,NODENUMBER+1,all

 

allsel,all

eplot

 

Finish

 

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

/SOLU   

ANTYPE,4

nlgeom,on

TRNOPT,FULL,,,,,NMK

TINTP,HISP!GAMMA = 0.005

KBC,0 

RESCONTROL,,NONE,None 

autots,off

OUTRES,ALL,ALL

 

!step1 charging a static wheel  

Time,0.001 

DELTIM,dt,dt,dt

TIMINT,off   

DDele,NODENUMBER+1,Uz

F,NODENUMBER+1 ,FZ,-Cn 

Allsel  

Solve   

 

!step2 rolling 

!inserting speed values  

Time,0.002 

DELTIM,dt,dt,dt 

TIMINT,on  

asel,s,area,,17

DADELE,all,ALL 

D,NODENUMBER+1,omgy,Wr

D,NODENUMBER+1,velx,V

Allsel  

SOLVE   

 

!pick up solution stage d=115mm

Time,0.00978

DELTIM,dt,dt,dt  

TIMINT,on 

Allsel  

SOLVE  

Please find attached the contact status corresponding to the last set of :

-Charging stage:

- Rolling stage

Best regards,

[mrife]

Hi Hajar

Double check the contact real constants; perhaps the limit frictional stress or contact cohesion values are not set as you intended.  Mike

[hajar.rhylane]

 

Thank you so much sir Mike for your too much important answer.

 

You have recommended to me to check the maximum friction stress (TAUMAX) value considered in the contact settings and i found that TAUMAX was equal to 1 in my simulation. I need to ask you sir what is the formula should be used to calculate the TAUMAX value that i should input in the contact settings?

 

According to the ANSYS manual:

” The program provides one extension of classical Coulomb friction: real constant TAUMAX is maximum contact friction with units of stress. This maximum contact friction stress can be introduced so that, regardless of the magnitude of normal contact pressure, sliding will occur if the friction stress reaches this value. You typically use TAUMAX when the contact pressure becomes very large (such as in bulk metal forming processes). TAUMAX defaults to 1.0e20. Empirical data is often the best source for TAUMAX. Its value may be close to the yield stress of the material being deformed devided by squar(3)”.

 

In the case of my simulation the yield stress of the steel is 489MPA so i defined TAUMAX as follow: RMODIF,3,9,282.324281633727e6. This value is yield stress divided by squar (3). Is this correct sir?

 

I’m really confused about its value please guid me.

 

Thank you so much sir,

Best regards

Hajar