Non Linear Analysis of Interference Fit with OptiStruct

This tutorial demonstrates how to carry out non-linear quasi-static analysis in OptiStruct of a 1 mm interference/press fit as well as non-linear quasi-static analysis of the interference fit along with an enforced displacement of 5 mm.'
DOWNLOAD THE FREE ALTAIR STUDENT EDITION HERE: studentedition....

[@antoniomancino8945]

0- I create the block and shaft components
1- I define the Mblocco material
I activate MATS1 to specify that the properties of the material depend on the state of stress.
I select TYPE and put plastic
I set TYPSTRN to 1
2- I define the relationship between stress and strain through an SvS load collector
Card image TABLES1
I enter the number of empirical lines of the relationship between stress and strain and fill in the table (not having the necessary data, I can use a curve generated using the Rambrg-Osgood equation)
3- I go to the Mblocco material and refer to the SvS load collector
in TID I select the SvS load collector
4- I create the Mshaft material
5- Creo 2 properties Pblocco and Pshaft
Both PSOLID, material respectively Mblocco and Mshaft
6- I create the property for the Pcontatto contact area
Card image PCONT
MU1 (coefficient of friction) I recommend 0.2.
7- I assign the Pblocco and Pshaft properties to the block and shaft components
8- I define two contact surfaces Unblock and Sshaft between block and shaft (create> contact surface)
Unlock: Elements> add solid faces, select block internal faces> add
Sshaft: Elements> add solid faces, select shaft outer surface (not the bases)> add
9- I create a Contact Cbloccoshaft in which I refer to the Sblocco and Sshaft contact surfaces and to the Pcontatto property
Property type: property id, PID: Pcontatto, SSID1: Unlock, MSID2: Sshaft, ADJUST3: no,
DISCRETE4: S2S, TRACK: finished
10- I define the boundary conditions through the load collectors SPCshaft, SPCblocco, SPCtotale
I apply the necessary constraints on shaft and block, then in SPCtotale I select the SPCADD card image that allows me to group multiple load collectors, in SPCADD_num_set I select the number of load collectors I want to group (2) and in Data: S I select them.
11- I apply an enforced displacement on the constrained faces
I create a new load collector LCenfdisp, and apply a load type SPCD (the constraints must be the same as the corresponding SPC previously set) on a shaft base.
12- I activate three loadcollectors with three cards required for non-linear analysis
-NLOUT, NINT: active, VALUE: 10, SVNONCNV active, VALUE: yes
-NLMON, ITEM: disp, INT: iter
-NLPARM, NINC: 10, MAXITER: 100
13- I create the loadsteps
-Interferencefit, analysis type: non-linear quasi-static, SPC: SPCblocco, NLParm: select, NLOUT: select. I create a label. NLMON: active and select.
-enforceddisploading, analysis type: non-linear quasi-static, SPC: SPCsum, LOAD: LCenfdisp, NLParm: select, NLOUT: select. I create a label. CNTNLSUB: active.
14- Start simulation.
1 SSID = Slave entity identification number
2 MSID = Master entity identification number
3 ADJUST = Adjustment of slave nodes onto the master surface at the start of a simulation
4 DISCRETE: S2S = Discretization approach type for the construction of contact elements: Surface-to-surface discretization

[@shivanitiwari2112]

Can anyone help where is interference joint made. M not able to understand

[@Ventre82]

Any link to supporting files for this tutorial?

[@alexnewman6227]

Good tutorial for optistruct, thank you. But: it would have made it to "excellent" if information regarding the geometry of the two parts were given AND a comparison between the FEA results and an analytical calculation for the stresses due to interference fit were presented. Otherwise, the outcome might be considered "pictures with colours"...

[@haryakumuda6798]

what if I dont have the stress - strain curve of the material, only have the yield point and ultimate point.

[@noonewillknow123]

Use the Ramberg-Osgood relationship to generate a curve.