Interference Fit

[harid]

Hello Friends,

I wanted to know wat values do i have to take for stiffness factor and friction in contact wizard to get my force required to cause the pressfit between a slug and receiver(fixed), I am trying to verify empirically and compare with ansys results. Could anyone explain all steps for doin press fit analysis. I used contact tutorial in ansys, but of no use.Please help me with ur tips.

Thank you.
cheers

 

[hwong]

What you need most probably for a start is the friction coefficient.

You already know the interference materials. You can find out from the internet search engine on the friction coefficient for some materials. You may base on experience the similarities of other materials. Else, you need to measure it from experiment.

The CAD models, I presume are already modeled using the worst case interference, so you can just use a simple linear isotropic material model, using only the Young's modulus, Poisson's ratio, density not required but no harm adding.

Constraining is important so check your pushing direction be free and which is fix or moving and any other constraints which may be necessary. If analysis cannot complete, then begin by constraining secondary conditions first, then running by releasing the constraints based on priority.

All the best.

 

[harid]

Actually I have used values of 0.2 for friction coeff and 0.1 for stiffness factor. The problem i have is when i get the reaction force to cause this pressfit found from time-history postprocessing and compare with my experimental force found from Instron machine to do the same press fit.I see they are totally different. Also my ansys stresses show that the parts yield because of pressfit( i mean i am getting high stresses beyond yield strngth of materials). In experiment I dont see any yielding. Please help me find wats goin wrong...

Thank you
cheers
harid

 

[hwong]

By the way, how do you model your material property?
If I may ask. Thanks.

 

[harid]

I have just taken material properties like young's modulus and poisson's ratio(in ansys) for 303 stainless steel, which i have used for the parts to be tested for the force required to do the press-fit on instron machine.I thought the force which i get from instron machine will be atleast closer to wat i get from my reaction force from ansys results. but these are so different. Please help me with ur tips.

Thank you.
cheers
harid

 

[hwong]

For my analysis for the insertion force, it was resonable.
I am wondering if it could be the interference you are using. So what is the total interference you have modeled for your interfering parts?

 

[hwong]

Just share my approach.
After the analysis, I obtained the contact stress between the interfering parts.
I used the highest stress value obtained to calculate the minimum corresponding force to overcome this frictional contact stress.
With the maximum area of interference contact which I obtained from the CAD software for the parts, I determined the maximum force required, based on the formula of stress equals to force divided by area.
Hopes this works for you too.

 

[harid]

Here is the input file for the interference model, I would really appreciate if u could correct this input file, I am just including the 2d model which was given plane 82 axisymmetric mesh. Please help me with the completion of the code for complete analysis and may be the calculation for this particular press-fit. So that i can design a generic press-fit model. Thank you very much for ur tips.

/PREP7
K,1,2.05/2,0,0,
K,2,12.5/2,0,0,
K,3,12.5/2,9,0,
K,4,6.15/2,9,0,
K,5,6.15/2,6,0,
K,6,2.05/2,6,0,
LSTR, 1, 2
LSTR, 2, 3
LSTR, 3, 4
LSTR, 4, 5
LSTR, 5, 6
LSTR, 6, 1
FLST,2,6,4
FITEM,2,6
FITEM,2,1
FITEM,2,2
FITEM,2,3
FITEM,2,4
FITEM,2,5
AL,P51X
K,7,2.05/2,9.5,0,
K,8,6.17/2,9.5,0,
K,9,6.17/2,11.9,0,
K,10,12.5/2,11.9,0,
K,11,12.5/2,17.5,0,
K,12,2.05/2,17.5,0,
LSTR, 7, 8
LSTR, 8, 9
LSTR, 9, 10
LSTR, 10, 11
LSTR, 11, 12
LSTR, 12, 7
FLST,2,6,4
FITEM,2,12
FITEM,2,7
FITEM,2,8
FITEM,2,9
FITEM,2,10
FITEM,2,11
AL,P51X
APLOT
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,1,,193000
MPDATA,PRXY,1,,0.28
!*
ET,1,PLANE82
KEYOPT,1,3,1
KEYOPT,1,5,0
KEYOPT,1,6,0
!*
ESIZE,0.2,0,
MSHAPE,0,2D
MSHKEY,0
!*
FLST,5,2,5,ORDE,2
FITEM,5,1
FITEM,5,-2
CM,_Y,AREA
ASEL, , , ,P51X
CM,_Y1,AREA
CHKMSH,'AREA'
CMSEL,S,_Y
!*
AMESH,_Y1
!*
CMDELE,_Y
CMDELE,_Y1
CMDELE,_Y2
!*
!*
!*
!*
!*
/COM, CONTACT PAIR CREATION - START
CM,_NODECM,NODE
CM,_ELEMCM,ELEM
CM,_LINECM,LINE
CM,_AREACM,AREA
/GSAV,cwz,gsav,,temp
MP,MU,1,0.3
MAT,1
MP,EMIS,1,7.88860905221e-031
R,3
REAL,3
ET,2,169
ET,3,172
R,3,,,1.0,0.1,0,
RMORE,,,1.0E20,0.0,1.0,
RMORE,0.0,0,1.0,,1.0,0.5
RMORE,0,0.5,1.0,0.0,
KEYOPT,3,2,0
KEYOPT,3,3,0
KEYOPT,3,4,0
KEYOPT,3,5,0
NROPT,UNSYM
KEYOPT,3,7,0
KEYOPT,3,8,0
KEYOPT,3,9,0
KEYOPT,3,10,0
KEYOPT,3,11,0
KEYOPT,3,12,0
! Generate the target surface
LSEL,S,,,4
CM,_TARGET,LINE
TYPE,2
NSLL,S,1
ESLN,S,0
ESURF,ALL
CMSEL,S,_ELEMCM
! Generate the contact surface
LSEL,S,,,8
CM,_CONTACT,LINE
TYPE,3
NSLL,S,1
ESLN,S,0
ESURF,ALL
ALLSEL
ESEL,ALL
ESEL,S,TYPE,,2
ESEL,A,TYPE,,3
ESEL,R,REAL,,3
/PSYMB,ESYS,1
/PNUM,TYPE,1
/NUM,1
EPLOT
ESEL,ALL
ESEL,S,TYPE,,2
ESEL,A,TYPE,,3
ESEL,R,REAL,,3
CMSEL,A,_NODECM
CMDEL,_NODECM
CMSEL,A,_ELEMCM
CMDEL,_ELEMCM
CMSEL,S,_LINECM
CMDEL,_LINECM
CMSEL,S,_AREACM
CMDEL,_AREACM
/GRES,cwz,gsav
CMDEL,_TARGET
CMDEL,_CONTACT
/COM, CONTACT PAIR CREATION - END
APLOT
FINISH
/SOL
FLST,2,1,4,ORDE,1
FITEM,2,1
!*
/GO
DL,P51X, ,ALL,0
FLST,2,1,4,ORDE,1
FITEM,2,11
!*
/GO
DL,P51X, ,UX,0
FLST,2,1,4,ORDE,1
FITEM,2,11
!*
/GO
DL,P51X, ,UY,-2.9
!*
ANTYPE,0
ANTYPE,0
NLGEOM,1
NSUBST,10,1000,10
OUTRES,ERASE
OUTRES,ALL,-10
TIME,2.9
FLST,3,1,1
FITEM,3,3514
MONITOR,VAR2,P51X,UY
FLST,3,1,1
FITEM,3,3514
MONITOR,VAR3,P51X,FY



CHEERS
Harid

 

[hwong]

Hi Harid,

I have went through your input.
I am not sure, but why not you model your material property to the stress strain data.
The stresses with strain might be lower than your current analysis.
The material I used for my analysis followed the stress strain as provided by vendor.

 

[harid]

Thank you for answering my questions. I would appreciate ur time if u could help me how to model my material property. Do u want me to figure out the stress-strain curve by testing on instron machine and then get the young's modulus from that...??? I will be thankful to u can explain in detail how do u want me to go abt doing that...

Thanks again

Harid

 

[harid]

Thank you for answering my questions. I would appreciate ur time if u could help me how to model my material property. Do u want me to figure out the stress-strain curve by testing on instron machine and then get the young's modulus from that...??? I will be thankful to u if u can explain in detail how do u want me to go abt doing that...

Thanks again

Harid

 

[hwong]

The following material is a template but may not be the best model. Go to the material property to refine the material with your values.

Values from the instron machine with control test pieces should be good enough.

However, better if material supplier has it.

All the best.

=======================================================

/NOP
/COM,Internal UNITS set at file creation time = USER
TBDEL,ALL,_MATL
MPDEL,ALL,_MATL
MPTEMP,R5.0, 1, 1, 0.00000000 ,
MPDATA,R5.0, 1,EX ,_MATL , 1, 5000.00000 ,
MPTEMP,R5.0, 1, 1, 0.00000000 ,
MPDATA,R5.0, 1,ALPX,_MATL , 1, 6.650000000E-05,
MPTEMP,R5.0, 1, 1, 0.00000000 ,
MPDATA,R5.0, 1,DENS,_MATL , 1, 3.333000000E-08,
MPTEMP,R5.0, 1, 1, 0.00000000 ,
MPDATA,R5.0, 1,PRXY,_MATL , 1, 0.350000000 ,
TB,MISO,_MATL , 1, 13
TBTEM, 0.00000000 , 1
TBPT,, 2.000000000E-02, 1.0000000
TBPT,, 3.000000000E-02, 2.0000000
TBPT,, 4.000000000E-02, 3.0000000
TBPT,, 5.000000000E-02, 4.0000000
TBPT,, 6.000000000E-02, 5.0000000
TBPT,, 7.000000000E-02, 6.0000000
TBPT,, 8.000000000E-02, 10.000000
TBPT,, 9.000000000E-02, 30.000000
TBPT,, 10.00000000E-02, 45.000000
TBPT,, 11.00000000E-02, 55.000000
TBPT,, 12.00000000E-02, 60.000000
TBPT,, 13.00000000E-02, 62.500000
/GO

 

[harid]

Thank you for ur tips. I will try that...appreciate ur time.

thanks
harid