FEA nonlinear analysis verification
FEA nonlinear analysis verification
(OP)
A C shape linkage is investigated for its maximum stress. The stress vs. Strain curve of the material is attached as Fig 1. The working condition and contour result are shown as Fig. 2, where there are two pin in the two end holes, the two centers of the holes are along the Y axis when the C-linkage is pull apart. Different mesh sizes have been tried to get a converged solution. The curve of the distance between the two end holes v.s load are shown in Fig 3.
I have 3 questions:
1. At linear stage, under same load the FEA distance result is less than the experimental distance result. For example, FEA: 0.05in at 1000lbs and experimental: 0.07in at 1000lbs. Is the result valid?
2. At nonlinear stage, the maximum stress exceeds the maximum stress on the true stress v.s. strain curve. And when the mesh become finer, the distance curve get closer to the experimental result, but the maximum stress get higher, for example, the fig. 2 shows the maximum stress of 171ksi at maximum load. Is this normal?
I have 3 questions:
1. At linear stage, under same load the FEA distance result is less than the experimental distance result. For example, FEA: 0.05in at 1000lbs and experimental: 0.07in at 1000lbs. Is the result valid?
2. At nonlinear stage, the maximum stress exceeds the maximum stress on the true stress v.s. strain curve. And when the mesh become finer, the distance curve get closer to the experimental result, but the maximum stress get higher, for example, the fig. 2 shows the maximum stress of 171ksi at maximum load. Is this normal?





RE: FEA nonlinear analysis verification
2)In reality what would happen if the stress exceeded UTS? What effect would that have on the Force/deflection curve?
Cheers
Greg Locock
New here? Try reading these, they might help FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm?
RE: FEA nonlinear analysis verification
Another aspect to consider is the effect of the pin in the hole. A better method would be to use contact so that the hole can deform rather than remain fixed as it appears in the picture.
RE: FEA nonlinear analysis verification
2) your mesh convergency study shows you're getting close to the limit, but still a reasonable difference compared to the test results (the ISE samples, yes?). one question, are you using a standard material curve, or one from the test specimen ?
you're getting a very large displacement (compared to the size of the model) ... i wonder if the real part is necking some ? or if the faces of the part are being distorted by the amount of plasticity we're seeing ??
maybe model with solids ?
Quando Omni Flunkus Moritati
RE: FEA nonlinear analysis verification
I agree that the poor modelling of the pin in the hole is likely to be significant, as shown it behaves like a welded in shaft.
Cheers
Greg Locock
New here? Try reading these, they might help FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm?
RE: FEA nonlinear analysis verification
To Greglocock,
I modeled the pin with certain number of beams weld to the center and the circle.
To corus,
I used the mesh by defining the surface mesh size in FEMAP. I checked the mesh, it not nice in the high stress area. The mesh at the high stress area is attached.
To rb1957:
1. The test is done on a pull test machine, the change of the distance of the two pin and the force are recorded by the computer program.The accuracy is 0.00001".
2. The stress-strain curve is downloaded from: http://www.ssab.com/en/Products--Services/Service-.... I guess its a standard material curve.
3. you are right, the sample is necked at the high stress area when the test is done.
I also have another finding in the results: at the load of 1000 lbs,the maximum stress reach 101 ksi, which is close to the yield point. but the load/distance curve shows this load is less than half way of the linear range. as my understanding of you guy's reply, this maximum stress might be fake. anyway I will try to improve the mesh and use 3D model with contacts to give it a try.
RE: FEA nonlinear analysis verification
I do also wonder why you used beam elements vs. solids - are you modelling the linkage as a 2d stress problem (i.e. fixing or not allowing out-of-plane deformation)? The real part likely does deflect out-of-plane in some areas, thus the 2d restraint can artificially increase the calculated stiffness of the part.
RE: FEA nonlinear analysis verification
it'd be nice to see principal stress plots (max, min) ... i'm sure it's doing the vM calc properly, but it'd be nice to see the components.
if the three (?, not sure if CQUAD4 has thru-thk stress) principals are real then the model is saying the part should fail (if UTS = 135 ksi).
Quando Omni Flunkus Moritati
RE: FEA nonlinear analysis verification
When I use the same solid/contact model to do " 10 nonlinear static analyisis", FEMAP says "Error writing Connection(s). Contact connection not supported by this solution type. Check Translation".