Press fit 3

[martin99]

Hi All,
Can I simulate a press-fit in Workbench 8. I'm currently actually modelling the assembly of the 2 components (moving a fixed diameter onto tapers)to get the assembled stresses and contact pressures. Can i get the final results just with contact instead, i know i certainly can in I-Deas.

Many thanks in advance

Martin

 

[pbd999]

Martin,

You can certainly do this in Workbench...I have done it many times. When you bring in the geometry ANSYS will automatically define the contact pair, that is the "Contact" and "target" surfaces between the parts. By default this will be a bonded contact condition but if you select the contact in the project outline, in the details view it can be changed to frictionless or frictional, whatever. There are two ways to go:
1) Model the actual interference in the CAD package. When you say "solve" ANSYS will resolve the the interference so that the parts are in contact with no penetration and you will have the assembly stresses.
2) In CAD model the parts as "just touching". Then in the Details view of the contact region under "interface Treatment" specify an ofset that is equal to the interference. This will offset the contact into the target and simulate the interference.

One thing to think about. Interference analyses using contact are sensitive to the amount of penetration allowed. In the Details view of the Contact Region do a sensitivity study on this by changing the Normal Stiffness Factor. Here's the tradeoff: Low factor (less than 1.0) makes convergence easier but at the cost of more penetration which can give the wrong stress. Higher value (> 1.0) gives more accurate stresses due to less penetration allowed but at the cost of more difficulty converging the nonlinear analysis.

Paul

 

[maxPE]

I assume that you would be using contact elements to simulate the intereference. I have done some work that indicates that the stresses resulting from this type of analyis is highly dependant on type of element and mesh density. Even with a high mesh density the results do not appear to be valid SOMETIMES. Believability and engineering judgement is a big issue here. Ansys corporate has worked on this issue and I suggest that you fall back on hand calcs to check your result. As an alterative, use hand cals to obtain the interference contact pressure at the surfaces and apply these to obtain the stresses from the models (inside and outside). I believe that this will give you more accurat results.

 

[martin99]

Many thanks for the replies on the method and warning.

Both methods work well, but I have one small query.

When solved, the contact data (separation, contact pressure etc) is only available for one component i.e. for only one side of the contact pair. Stresses and deformation are calculated for both sides but any ‘contact derived’ results give a zero value for one side. Solving after changing from asymmetric to symmetric gives the contact results for the other side. Any ideas on this, or an explanation of why this happens?

Also thanks for the warnings about contact and FEA. With regard to hand calcs, the problem I have is that it is not a true press-fit and the deflection of one component conforms to fit the other changing the area of contact. I’m not experienced in a hand calc of this of non-linear type. Can you suggest any good texts with regard to the hand calculations for the contact pressure.?

thanks again

Martin

 

[ifegermany]

you get ‘contact derived’ results on both components for symmetric
as this option generates contact faces on both components,
while asymmetric creates them on one components faces only - target faces have no such results available.

Frank Exius
IFE Deutschland

http://www.ife-ansys.de

Telefon ++49\2642\980409
Germany

Dienstleistung in ANSYS
FEM Berechnung Simulation
Digital/virtual Prototyping