I met some strange problem.I can not present an exact model dimensions and loads but will try to explain on simple simmilar model.
I have to check some simple anchoring/fixing eye. I had some doubts when performing hand calculations so prepared model with NLS (SOL106). See the below picture with the anchor/padeye/lifting lug.
I fixed it on the bottom and loaded with function "BEARING" on the selected tubular surface with certain load "A" with direction along Z-axis . The angle of loading =180 deg + parabolic distribution.
What is strange, when checked the resutls, the sum of Z-reaction forces on the fixed surface is not exactly equal to the load specified in "BEARING" function. Why is that so, can anyone explain?
The relative difference is not very high (1-2%) but when we compare absolute values, it is about 4-5 kN, which is quite a lot.
In the documentation I didn't found any comments/ limitaitons / explanations regarding this.
thanks waiting for your opinion
I can't tell you whats the method of transfering analytical bearing load onto mesh but I could imagine two reasons for your effects:
1. May be its an effect of accuracy during transfering from analytical surface onto nodes of discretized elements.
- the size of elements, may be its too coarse,
- the mechanical load summary, may be you get already here an differing load sum,
2. May be its an effect of accuracy during transfering into NASTRAN-DAT-file.
- the values in your load description in DAT-file for elected nodes with the those in load display in fully
expanded visualization mode with node values.
May be you will get better results in you special case if you increase the number of significant digits of load value by changing settings in "Advanced Solver Options" Field Length from "Small" to "Large". The size of your DAT -file will be nearly doubled and you get in case of forces may be 10 digits instead of 4 - 5 (depending on number of digits in exponent).
can you check the sum of Z-reaction forces in the BEARGING? They should be exactly the same an in the fixed surface! I don't think that the mechanical equilibrium is wrong by 1-2 %. If they are the same, then maybe applying the load nonlinear in steps doesn't work correctly. If not, maybe you don't get all the nodes that are fixed when summing them up!.
Keep us updated!
Small update and clarification.
@JonkMcCool you were right.
When I put the force value in Bearing function it is not transferred 1:1 to the fem file, meaning if I check the "Applied Force - Z direction " in results it is not exactly the same as the function input, but is exactly the same as "Z- reaction force".
The numerical error of mentioned 'transfer' was also not so big as I previously mentioned, is not less than 0.3% so it seems I just overreacted, but when it comes to absolute value, for big loads (that act for example on offshore structures) it may differ sometimes of few tonnes.
We should be aware of fact that the 'transfer' between GUI and Solver is not always 1:1.
I think now is clear, topic closed