SimScale CAE Forum

Force plot of a structure


#1

Hello, i’m a learner of SimScale, and i’m working in a project involving a concrete structure, the objective is to:
Calculate the upward (lifting) force caused by typhoon,

There are my design constraints:

  1. I would like to make the entire structure less than 200kg,
  2. The structure consist of 2 concrete base (each of them <90kg), and a 20 to 25 kg panel on top of the bases,
  3. The top panel must be at least 10 degree.

this is my project link:
https://www.simscale.com/projects/gkwok/concrete_base_02_1/

Here is my mesh, strong wind is blowing towards the back of structure (y-direction):
as you can see, panel (the flat surface at the top of the structure) is 10 degree inclined:

The Results control “forces and moments”:
Lower Panel:


Upper Panel:

The simulation results:
Upper Panel:


Lower Panel:

as you can see, the wind is blowing in y-direction (as shown from the picture above),
from the force plot:
the average force acting on the upper panel is about 2100 N in Z-direction,
the max. force acting on the lower panel is about -750N in negative Z-direction,

My problem is:

  1. Is that means the force acting on the panel is upward force? with net upward force 1350N??
  2. Actually, the back of the structure is sealed, why there is still a huge upward force acting on the panel?
  3. Is there anything wrong with my understanding or system setting?

thank you


#2

Hi @gkwok!

Might take a bit of time to delve into this project - will have a look at it later on and let you know my thoughts on it. @DaleKramer & @Retsam, feel free to add your thoughts here as well.

Best,

Jousef


#3

Thank you for your help,
actually, i only used the default simulation settings, because i don’t know which solver / what setting is suitable for this case.


#4

Hi @gkwok,

You should not be surprised by roofs lifted by wind even weaker than your. If you look into pressure field in ‘Solution Fields’, it will explain the lifting force.

However you still have ‘face3229’ missing from definition of Lower Panel, so actually lifting force from strong front pressure will be much bigger. In your case Z+ means lifting force, but now you possibly grasped it.

Some hints:

  • Your ‘house’ is really small, perhaps for a dog: Turbulence will develop in a dozen of seconds, so no need to run simulation for 1000 seconds.
  • Your big Background Mesh Box is an overkill: you can reduce it 100 times for you tiny house (but keep the mesh resolution).
  • In open air, for reduced tunnel size, I suggest to NOT use slip walls. Instead, use: Custom > U and P Zero Gradient > k and omega Fixed value, set respectively to k = 0.00375, omega = 3.375. That way the walls become ‘transparent’ and will not reflect pressure drop or whatever due to turbulence or wind direction. That kind of ‘transparent’ tunnel allows one to change inlet wind direction: when you try to do that in normal ‘slippy walls’ tunnel, simulation will go awry.

Retsam


#5

Thank you for your advice,
i’m now doing some modifications:

  1. In simulation control: reduce the “end time” and “write interval” to 500s
  2. Reduce the size of mesh box
  3. Change the settings of the walls

and check the results later.

But in the Numerics, is the default solvers and settings suitable for my current situation?
Also, if i want to find out the total upward force acting on the entire structure, should I include all the faces (select the entire structure) in the Result Control - Forces and moments?


#6
  1. Time of simulation seems still big compared to object size: observe forces on time scale, the same for convergence. After 300 seconds nothing special happens.
  2. Seems OK: check in Solution Fields how it behaves.

Default solvers are good enough for your sandbox. Now, as time on simulation is about 5 core-hours, you can experiment with different solvers. However @DaleKramer may have different opinion.

Now, tha last part of your question: You can avoid that hassle with faces if bottom line is to find total upward force on the whole structure. How to do it?

  • If you have (or make) only one solid in your drawing software, export it in STL format.
  • Load new geometry in the same project. You will find only one object (solid) to handle.
  • Create a copy of the simulation.
  • Go to simulation copy and change the Geometry to new uploaded geometry. You will loose the current mesh in that simulation copy.
  • Click on mesh, than again on mesh in the open frame and select the original mesh used before.
  • Refine what you want, etc and create new mesh.
  • Now, for simulation, you select that unique object as a target for Forces and Moments. That’s all.

Not yet: think twice if you believe more processors are better for you budget of core-hours. You may reduce time of calculation, but you core-hours will be doubled or tripled.


#7

Yes, I think that works. Right now your geometry is imported as 1 solid so I am unsure of @Retsam suggestion…

But, this is a very small concrete structure, are you sure you 1mx1,6mx0.4m are the correct dimensions?


#8

Dale: short answer about geometry is that AFTER meshing the STEP format or PARASOLID are ‘exploded’ into flat structure of many faces. This is not the case of STL format: you have, after meshing, still one solid (but its name is lost).

By the way, elsewhere you proposed to change the naming convention for meshed faces: I would agree, but it is not enough. Why meshing does not preserve naming of entities, present in STEP files, for instance? Then the structure of the mesh will be easier to navigate. Perhaps we can join forces to propose that?


#9

Ahhh, but I don’t have much luck exporting good stl from Rhino, I just stick with importing Rhino .3dm files and I don’y know if Rhino has entity naming.

I am not sure I am much of a force to join with :wink: , and I definitely have my own opinions on a lot of things but I will post this as one of my ‘Dale’s Feature Polls’ and you can vote and comment on it there :wink:


#10

OK, keep me posted about that topic: I can elaborate later on.


#11

Hi, i’ve got the result:


It seems the little tail on the top left of the picture is the major cause of uplift force.
Perhaps I need to eliminate this little tail and try the simulation again.

Actually, this CAD model was imported from Onshape.
Onshape can export the model to STL, or other format, but is it necessary to do that in my case?


#12

Hello, yes, the dimensions are correct,

There are my design constraints:

  1. I would like to make the entire structure less than 200kg,
  2. The structure consist of 2 concrete base (each of them <90kg), and a 20 to 25 kg panel on top of the bases,
  3. The top panel must be at least 10 degree.

I have selected the entire structure in the force plot, the above picture is the total uplift force of the entire structure, the max. is about 1604N, which should be able to meet my design target,

The power of the wind is much bigger than I imagine. I’m still trying to modify the design, as strong wind can lift the panel. So, putting a cover at the back may reduce the uplift force.


#13

Looks like you have things under control now and it looks like this is a concrete structure that just sits on the ground…

Don’t forget to take into account the moments results that would let you obtain the lifting force on the windward wall with respect to the actually weight on that windward wall (from c of g location and weight of structure).

And to confirm that the structure drag will be significantly less than the friction created between the concrete structure and the surface it is sitting on.

Have fun from here!
Dale


#14

Thanks for your advice,
Just a question, every time when i finish mesh generation, a message appear:
“Simulation assignment on the geometry is not supported for the currently selected mesh. Try to regenerate your mesh or use the mesh as simulation domain”

so what’s the problem with the mesh?


#15

Please ‘use the mesh as simulation domain’ and everything will fit in place.