Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

How to interpret my results....?

sander

New member
I have some experience with FEA software (Cosmos) . I am using Structure now since januari, and I have some basic questions about the interpretation of my results.<?:namespace prefix = o ns = "urn:schemas-microsoft-com:eek:ffice:eek:ffice" />
I thought it would be interesing to doso with help of the picture below.

Material : Aluminium.
I have a vertical load applied at the hole (top left hole)
I have contrained my part as if it were fixated between two washers (see circular pattern bottom right)

At the washers, you can see the stresses are above 230 N/mm2.
My aluminium yield stress would be around 130 N/mm2.

Does Structure/Mechanica (integrated mode) interpret the Aluminium material as lineair, even when exceeding my yield stress ?
(I have applied an alloy from the standard material database. My material has only the Modulus of Elasticity applied, soo I would assume my material is only interpreted as lineair.)

If soo (only lineair) should I let my part fail my test ? Or can I make some assumptions about local deformation, but not total failure of the part, because the stresses are that high only locally ?
(But then I would discard the
 

james.lynch

New member
Sander,


Mechanica is a linear fea package, also if you fully constrained the washer, it's goign to result in stress concentrations,


a possible work around may be to create an actual washer and create surface region on the outside of it (representing the nut) and constrain that. thenuse contact regions between them. the advantage of this is that teh high stress concentration s will occur on your washer and could possibly be excluded.. (BTW contact regions cantake a lot of time to compute)


no I'm by no means an expert in mechanica so this is how I'd probably do it but I'm sure that there are many more ways o going about it.


James
 

Mloew

Moderator
I would first be woried about the boundary conditions. I always make the following demands of my analysts:



Applyboundary conditions that are both correct and realistic. Constraints should be used primarily to model symmetry conditions and to remove rigid body displacements and rotations. A balanced load and moment approach with minimal supports should always be used (i.e. the sum of loads in any global direction equals zero, taking moments about any global axis should also equate to zero, if this is employed correctly then minimal supports can be applied which will prevent rigid body motion and rotation, but will not react any load). When possible, avoid use of constraints to solve for reaction loads. Do not over-constrain models; this often results in misleading stresses and/or displacements. Boundary conditions should match those seen in component/system testing and/or in service.<?:namespace prefix = o ns = "urn:schemas-microsoft-com:eek:ffice:eek:ffice" />
 

bem

New member
I would agree with matthew, but the large deformation option is non-linear in the sense that it takes into account geometric stiffness. Material properties are linear. Geometric nonlinearity is useful where phenomenon like membrane stiffness plays a role
 

pedja666

New member
Your stress around constraint is fictitious and it is not nowhere near 230 MPa.As far as I can see it is rather around80 MPa.<?:namespace prefix = o ns = "urn:schemas-microsoft-com:eek:ffice:eek:ffice" />


Your model is of simple geometry do the hand calculationand verify the stress in the proximity of the constraint (STRESS=F*L/I *THICK/2.It does not seem to be nonlinear to me (What is the max deformation ?)This problem with singularities around constraint will reoccur contently in ProM and you will have to learn how to get around it
 

Mloew

Moderator
Singularities around contraints will be present in any FE method model, P, h, whatever. This is not a MECHANICA specific problem; it like most problems I have seen, has to do with the model and the BC.
 

pedja666

New member
I agree,it is the elasticity theory which all codes use that makes trouble.


BTW there was a mistake in the formula It should have been :


STRESS= (F*L)/W; W=I/(THICK/2) I- Moment of inertia
 

sander

New member
Thanks for all your input !


I allready did some handcalculations, and there I allready concluded my part would be allright.


But I just wanted to see what Pro/E would make of it.
 

Sponsor

Top