unexpected results on a static analysis
Altair EmployeeHello,
I am a master degree student and i'm currently try to solve a finite element problem for a school project.
I want to run a a static analysis about a structure that is supporting concrete blocs. I've linked a picture of the problem to this message.
The concrete blocks contact with the structure is not continuous. I have linked a picture of my Hypermesh model with the contact highlighted in white.
I use a pressure reparted on this white area to model the actions of the concrete blocks on the structure. The concrete bloc is not deformable.
The third picture coresspond to my simulation results.
I am not sure these results represent the reality because as I mentionned before, the concrete block is not deformable so the structure is not supposed to bend that much in the middle area. I suppose the software consider that these pressures are independent, so how should I proceed to make Hyperwork understand that all these pressures belong to a same solid in order to see the 'pillars' of the structure being deformed instead of the middle area ?
For this type of loading (mass that has a complex contact with the structure) should I run a multi-body simulation instead ?
I don't know if my questions are clear, feel free to ask me some more details if you don't understand it.
(i've linked in 4th picture the constraints in the structure)
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
Answers
-
Hi QuentinB
Altair Forum User said:I use a pressure reparted on this white area to model the actions of the concrete blocks on the structure
How did you apply the pressure load. Will it resemble a distributed load along the structure?
0 -
Looks like a standard three point bending response. If you could include a scale that would be helpful.
Could always try using a remote force where the top of the block is
0 -
Altair Forum User said:
Hi QuentinB
How did you apply the pressure load. Will it resemble a distributed load along the structure?
Hi thank you very much for this reply, I used the 'pressures' tool from the analysis panel.
The concrete block is 500 kg
The 'white area' which is the contact between the block and the structure is 34 950 mm2
g=9.81
So by using the relation Pressure= Mass*g/white area
I find that pressure = 0.140 MPa
This is the value of the magnitude I use for the pressure on the entire white area. Should I proceed differently ?
I attached some pictures to show how the pressure is applied on the elements.
<?xml version="1.0" encoding="UTF-8"?>
Altair Forum User said:Looks like a standard three point bending response. If you could include a scale that would be helpful.
Could always try using a remote force where the top of the block is
Hello ! You're right, it is a standard response, but this is not what I expected because the concrete block cant't be deformed like that in its center area.
I might be wrong but the constraint is supposed to be concentrated in the 'pillars' relied to the ground. The following picture shows the case that happens ( case number 1 on the top) and the one I expect to model (case 2, on the bottom). In the second case, the bloc is not deformed, which is what happens in reality (we have some measurement that shows the concrete can't bend in that case.
You asked for a scale. The maximum displacement in the center is around 2 mm while I expect a value 10 times smaller.
<?xml version="1.0" encoding="UTF-8"?>
0 -
Help ?
I still didn't find a way to solve this simulation
0 -
Hi QuentinB
Is there a specific reason why you are applying pressure? or else you can use this suggestion and try out
1. Select all the nodes of the surface area in contact (white color portion) and make it as rigid. You can use the calculate node and multiple node option inside the rigids panel. Input the mass of the block as force into the master node of the rigid. This will equally divide and apply the force exerted by the block to all the nodes, which will give reasonable result
2. Also the contour image will show the deformation according to the scale factor you have provided. So check the actual deformation values of the deformed region and interpret the result; the deformation may be too low
0 -
You made the model complicated.
If concrete block is non deformable, it does not cause bending so I think just devide its mass by 2 and apply to each pillar but not the middle beam - only compression is considered.
0 -
Altair Forum User said:
Hi QuentinB
Is there a specific reason why you are applying pressure? or else you can use this suggestion and try out
1. Select all the nodes of the surface area in contact (white color portion) and make it as rigid. You can use the calculate node and multiple node option inside the rigids panel. Input the mass of the block as force into the master node of the rigid. This will equally divide and apply the force exerted by the block to all the nodes, which will give reasonable result
2. Also the contour image will show the deformation according to the scale factor you have provided. So check the actual deformation values of the deformed region and interpret the result; the deformation may be too low
There was no particular reason why I used pressure so I tried your solution and it worked, the simulation gives me the expected results. I am not sure the magnitude is right but the type of response totally is. Thank you very much.
Altair Forum User said:You made the model complicated.
If concrete block is non deformable, it does not cause bending so I think just devide its mass by 2 and apply to each pillar but not the middle beam - only compression is considered.
You're right, it would work for that case. As I just mentioned previously, Pranav solution also seems to work, I'll compare both results and use the best one for my thesis. Thank you very much for your answer.
0 -
0
