Small equation pivot terms

[Sephiroth79]

Hi all.
I a m running a static stuctural simulation on a simple metal frame on which there's a front load and a constrain on the back.
As i am simulating ansys wb11 tells me that there are 5 small equation solver pivot terms.
As far as I know it means that large displacements are going on in the model.
I can't solve the problem also with "large deformation on" and with "gravity acceleration on".
Any suggestion on how to fix the problem?

Thanks.

Andrea

 

[cbrn]

Hi,
the message is a warning, not an error, so you should obtain a solution anyway; if your solution is misconverging then you have at least two possibilities:
- there is an improper (ill-conditioned) set of restraints
- you are running into some kind of instability (buckling?)

In order to check for the first, it's easy: run a modal analysis and see if you find any (at least one) rigid body mode (should have frequency extremely near to zero).

The check of the second is harder and mainly need the knowledge of what's happening to your frame, so without further info I'm not able to say more.

Regards

 

[Sephiroth79]

Thank you for your reply.
I Know that the message wb gives me is a warning and not an error, but the solution does not converge after at time 1 on 4 seconds so i am guessing that there's a problem on my model.
I am going to run a modal analysis and i'll try to post some picture of my frame with the constrains I have applied.
I am going to try to run a simulation in which the load is just 1/10 of the real one. If it runs fine it means that for efforts greater than 1/10 of F the structure go in insyability (maybe buckling).

 

[Sephiroth79]

Just to understand: the purpose of the test you propose me 'bout running a modal analysis is to understand if the If the modal analysis gives as an answer that one or more bodyes have frequency around zero it means that this bodyes are completely constrained?

 

[Sephiroth79]

Here it is the image of my simulation.


Shot at 2007-08-10

The red arrow is the effort, the violet ones are the constrains (fixed support), and the yellow one is the gravity acceleration.
I am still having problems with "small equation solver pivot terms".
In the first run i've made i was trying to simulate the floor (as the machine is on the floor) and for this I was using only compression supports on the faces under the structure and the fixed support where you can see the B in the image.
However in both cases i have the same problem and finally I have a non converging solution.

 

[cbrn]

Hi,
1- yes, as the structure is made there MAY be an instability problem (the load vector is not colinear with the neutral axis of the structure)
2- if the modal analysis reports a rigid body mode, it means that at least one component is NOT completely restrained.

...The temptation to write in Italian is strong, but the rules here don't allow to ;-)

Regards

 

[Sephiroth79]

Are u from italy too?
However thank u fro your quick reply.
In my structure the center of gravity lies on the axis on which pass the efforts so I am expecting no buckling.
Is it correct to simulate the effect of the floor giving to the surface of the machine wich touches the floor a "compression only" constrain?

 

[cbrn]

Hi,
sì, it's correct. Only looking to the picture doesn't really make easy to understand what's going wrong...

Regards

 

[Sephiroth79]

Yeah I know.
I am supposing that the mesh is not correct as my system has not much memory (2 gb) and I am actually working with windows xp 32 bit.
The dimension of the strucuture is something like 1000*1100*6000 (mm) so i have a lot of elements and if I refine the mesh the system tells me that there's not enough memory to run the simulation.
I really would like to understand why it's not running!!

 

[cbrn]

Hi,
I would reverse the problem and, first of all, run a simulation with a VERY coarse mesh. Accuracy is not a goal for the moment, you have to try and understand what is wrong with the numerical model. Think thoroughly about the boundary conditions (restraints in particular), think about the effect(s) of the contacts you are using (if any), if in doubt run the modal analysis to see if there still is something unrestrained (or ill-restrained).
By the way: your structure is of the gendre which would far better be modeled with beams and plates (shells, thick shells).

Regards