FEA nonlinear analysis verification

[upzheng]

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?

 

[GregLocock]

1) yes, if you and your customers can live with 30% errors. I doubt they will. It is very common for FEA models to overestimate the stiffness of solid bodies. The reasons are many.

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

http://eng-tips.com/market.cfm?

 

[corus]

I'd be suspicious about your results as the contours around the maximum stress position appear to be irregular, rather than smooth contours that you'd expect. Your absolute maximum stress might be due to badly shaped elements, which will remain badly shaped the more you refine the mesh. Try meshing it so that the mesh is smooth and regular.

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.

 

[rb1957]

1) the FEA result shows a stiffer model than reality. personally, i think the test result reasonably matches the FE prediction (i'd ask what's the measuring accuracy of the test result ?, maybe 0.01" ? ... a large proportion of the difference)

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

 

[GregLocock]

A 30% error in static stiffness is a 15% error in natural frequencies - not acceptable in my neck of the woods.

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

http://eng-tips.com/market.cfm?

 

[upzheng]

Thank your reply, guys.

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--support/Technical-Tools/Steelfacts/Steelfacts/.

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.

 

[btrueblood]

The stress-strain curve you linked to is for the rolling direction, but your part will have areas loaded transverse to the rolling direction, i.e. you may have fairly anisotropic material properties. I don't know if it's part of the problem here or not, the people who have already replied are more better experts than me at nonlinear stuff.

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.

 

[rb1957]

i interpret your results as max principal stress = 135 ksi, vM =171 ksi ... which you get with tension-compression principal stresses.

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

 

[upzheng]

I tried solid/contact modeling with HEXA8 elements, I can do static linear analysis. the maximum stress lowered to 88.6ksi from 101 ksi (yield strength 110)obtained by using shell/beam elements. but the deflection decreased as well, which is .041 instead of 0.05. It seems that the transverse deflection is included when solid/contact model is used, but the deflection is even farer from the test result.

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".