Flexplate assembly under different loads

[consti2005]

I'm trying to correlate test displacements results for a flexplate assembly with static linear FEA results under a concentrated axial load, using ABAQUS Standard. They do not match. The theory shows that ABAQUS is correct in its results. This means my assumptions for FEA are not correct or not taking into account everything.
In testing they are doing a combined axial-torque fatigue test.
Do you have any experience to share and help me find a path to follow?

Thanks

 

[CESSNA1]

CONSTI2005: Since you mentioned fatigue testing, I assume that the test item is operating. You cannot compare commpare a dynamic (operating) results with a static analysis program. What is it specifically you are trying to do?

Regards
Dave

 

[consti2005]

In my simulation:
- modeled flexplate, ring gear, bolts & crank;
- tie (weld) ring gear to the flexplate, tie crank area to the flexplate and bolt heads to the flexplate;
- I'm constraining in all DOF the flexplate at the torque converter lugs and apply the loads in a MPC, at the end (and middle) of the crank.
They are only testing only in a simple load and not in fatigue. The testing conditions seem to be similar to my FEA assumptions.
Abaqus find a good correlation with the theoretical solution, but still far from testing. People from Abaqus tell that should be a limitation in the model itself.
What else I could add or change in my simulation in order to better correlate?

 

[GregLocock]

"tie crank area to the flexplate " looks a bit odd to me.

Modelling bolted joints is complex, and for a flex plate I'd imagine quite critical.

In what area do your test results and FEA disagree?



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[consti2005]

All my previous simulations used contact between al the parts in contact (less of course between ring gear and flexplate). But I found that there is no big difference in displacement when I tied the parts.
So, the big difference between tests and FEA appear in the realm of displacements. For a simple axial load the plate looks much stiffer (less displacement) in FEA than in testing (almost two times). They measured a stiffness of about 30000lbs/inch and I got about 56000lbs/inch in my simulation.
Therefore, the question would be: what else I could add or improve my model, or other type of approach I should make in order to match the results?

Thanks for your input! I have nobody to talk to or to consult, therefore your help is highly appreciated.

 

[GregLocock]

Can you refine your mesh density and see if that changes the stiffness?

Can you get them to measure the deflection at various points rather than just at the rim?

It is usual for FEA to overpedict stiffness, because people use rigid elements, which don't exist, and don't model soft interfaces properly.

I'd look very closely at the bolt/flex plate/crank interfaces



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[consti2005]

Thank you very much Greg!

I feel better, because I'm not "alone in the desert."
I'll try your suggestions.
What I tried until now was the following:
- use 4 solid elements per thickness (flexplate) of first order with 1mm element size;
- use 2 quadratic solid elements per thickness of 2mm size (flexplate) but I got a big model going beyonf of my UNIX machine;
- 1mm quadratic shell for flexplate;
-contact between plate-reinforcement and reinforcement-dummy crank;
-tie the bolt heads to the plate, no contact between bolts and flexplate (holes in the flex and bolts).
-contact between lugs and flex but tie the bolt heads of the lugs to the flexplate.
I did not try to go below 1mm element size for the flexplate, but I think I could go if I'll use shell elements (the size of the model remains in decent limits for my computer).
Are you aware, for the contact in Abaqus, if I should use a particular one, better adapted to this situation?
Do you think that tiing the bolt heads to the flex will significantly affect the stiffness of the flex?

Thanks!

 

[GregLocock]

1mm elements should be small enough. You can use bigger elements for most of the plate, just get the mesh density high around the fixings.

If you look at the axial stiffness as being like a cantilever loaded at the tip, then the biggest effect is likely to be the bending at the root, ie the bolt to crank interface.

I really think you need more test data (or more aalysis of what you have).

How does the axial stiffness comapre with a hand calc?



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.