'Parachute' simulation project by jhorv_th


#1

I created a new simulation project called 'Parachute':

Parachute test v is 4mps


More of my public projects can be found here.


Seemingly overly large drag values, unsure why
#2

Hi @jhorv_th - super interesting application! Eager to help if you’re running into troubles with the sim!

Best,

David


#3

Hi @dheiny,

first of all thanks for your interest in my project!

I’m quite new with SimScale and with CAE applications in general so I’m trying to use my little knowledge about the topic based on a Drone prop simulation tutorial to determine the drag force applied on the canopy at 4m/s descent rate.

My first run was not a real success, because the Force plot showed 0.0 N. Now I’m making a new mesh that seems to be stucked and I’m not really sure that this one would work better.

Anyway, I’d appreciate any tips tricks comments or hints so that I’d succeed sooner.

BR,
János


#4

Hi János @jhorv_th,

I had a quick look at your project - great work! Two things I noticed:

  • Boundary Condition setup: The reason why the force is zero is that you’re not forcing any flow. So a flow field that solves your constraints is simply zero velocity everywhere, which is why the force also is zero. If you force a flow to happen e.g. via an inlet BC at the bottom, this will change immediately.

  • Mesh: This might be a bit trickier to fix. Your mesh contains illegal faces, see meshing log:

The surface of the parachute is changing the angle to Cartesian directions constantly, so that can be a challenge for meshing but this can be fixed as well. A first few hints:

  • Cell height is considerably larger then cell with, see this image (I know, I’ve got mad drawing skills :wink: ):

Throw in more cells in z direction, than this should get better. I’m pretty sure that the edges on the parachute are the region where the illegal faces occur:

Here you could turn up the surface refinement by one more level.

Check each time the meshing log, if the illegal faces have gone. Once they are, with the new boundary condition setup, this will give you the force acting on the parachute.

Hope that helps.

David


#5

@jhorv_th,

one additional hint: The second mesh you generated approached more than 30 million cells, which is probably a bit overkill to this type of application. I’d turn down a bit the overall bounding box discretization and start with one level lower in terms of surface refinement and start iterating from there.

Let me know, how it goes.

Best,

David


#6

Hi @jhorv_th,

I see the new mesh finished without illegal faces/cells but it does not reflect nicely the CAD model anymore. Indeed a tricky geometry.

@Ali_Arafat - could you take a look here? The continuously changing curvature seems to be challenging, specifically at the edges. Could you hint to a proper mesh setup?

Thanks.

David


#7

Hi David @dheiny and Ali @Ali_Arafat,

wow, you really follow this project. Thanks, I highly appreciate it! Your tips and tricks helped me a lot! :slight_smile:

I think the progress is so far so good. At least I have some cool colorful pictures which is nice! :smiley:

I am not really worrying about the exact shape. I know my CAD model is not optimised for CFD. What I’m interested in is to get a result (Pressure force z?) for the drag force.

According to my simple calculation, the force should be around 26N:

It means that with SimScale this value should be 1/4 of 26N -> 6.5N because only 1/4 of the canopy is modelled. Unfortunately this hasn’t been approached with my simulations. I’m sure I set something wrong by the simulation.

I set 4m/s in the Z direction on the Inital Conditions/Velocity tab, and a boundary conditions of Velocity inlet with 4m/s also. Maybe it is overdefining? Or should I add a 0Pa surface at the inlet?

My last run seems to be wrong, so I’ll keep on trying to figure out what was wrong.

Anyway, any other tips, comments and hints are welcome!

Thank you in advance! :slight_smile:

BR,
János


#8

Hi, @jhorv_th nice geometry. Well you are unable to run the simulation because you have defined multiple boundary conditions for the same faces. You have defined inlet condition at inlet face and also you have included this same face in the slip walls. Same is with the outlet. Remove the inlet and outlet from slip walls then you will be able to run the simulation. Once you have force results with this setup then we will be able to comment regarding the validation of results. If you need any help feel free to contact. Have ffun

Cheers :slight_smile:


#9

Hi @AsadAli,

thanks for the hint. I’ll give it a shot. :slight_smile:
It’s kinda embarassing for me to make such a mistake… :smile:
I’ll inform you about the results.

Cheers


#10

@AsadAli, @dheiny,

It looks like the result is still not similar to the calculated one. May you please have a look on it, what can be wrong?

Thank you in advance! :slight_smile:

Best,
János


#11

Hi @jhorv_th

Good to know that now you are able to run the simulations. I have looked into your results first very obvious mistake we are making is that we are using symmetry. By this we will have unbalanced forces in horizontal directions, as you can see from force plots. For this case we have to make a mesh of complete body. SimScale calculates pressure forces by integrating pressure over the given surface (Pressure over normal surface), which is slandered way of calculating the pressure forces on the given patches. These forces almost always agree with the analytical calculation(depending on the mesh quality). Try to run the simulation for full mesh and lets see what we get. If you are still unable to find the correct results then this will be an interesting case for us as well. Also double check your analytical results since we do not know the exact geometry description so cannot figure out the calculations. If you need any help, feel free to contact. Have fun

Cheers :slight_smile:


#12

Hi @AsadAli,

first of all, it’s quite a shame but my calculations were wrong! The projected area of the canopy was not right so the drag force. I’ll introduce my calculations later.

With the new value the error between SimScale and my calculations is 37% at 1/4 of canopy simulation which is not too good but not bad either.
I’d like to note that when I say 37% error I mean it is a speculation of mine, does not grade SimScale at all! I’m not a professional so please consider this when reading!

So then I made a full mesh simulation excepting a much better result. Unfortunately it got 62% error. The strange thing I noticed is that the speed distribution is quite assymetrical and the highest velocity is 25m/s. Probably there are some problems with meshing at the edges or something.

This first run with full mesh lasted for 5000s and I saw on the Convergence plot that the force remains constant from 2500-5000s so I made a second run to make it more detailed in the 0-2500s interval. That’s when the confusing part came. The forces and velocities got extremely high and the convergence plot got funny:

I did not change anything else but the time interval. What could cause this?

At last but not least here are my calculations:


#13

Hi @jhorv_th nice work

Well due to certain meshing defects, simulations can diverge after long time, so if you know your simulation is converging early then no need to elongate the simulation time. Also velocity can increase in the middle of parachute due to small opening there. We made a simulation run for you using two different meshes, and we got the drag force of 4.96N for both cases, which is -if you consider the exact drag coefficient for this shape- in a good match with exact calculations. You can find this project here. If you need any further assistance, feel free to ask. Have a nice day.

Cheers :slight_smile:


#14

Hi @AsadAli, nice work too!

The convergence plots and flow patterns of your simulations are much nicer than mines. I need to compare from step to step what you changed. I’m sure it will be very useful for me. :slight_smile:

Indeed the coefficient is just an approximation. And maybe with a bigger scale “real life” canopy the results would converge more to the calculated one. Anyway I’m quite happy with your results.

One question: the box’s walls are set to be slip walls but the velocity drops near them. Shouldn’t it be also 4m/s at the walls? I think that command simulates like there were no walls at all around.

Have a nice day to you too!

P.s.: I made an other simulation (of a completely different project) and there there was only 2% error between the calculated and simulated results. Pretty impressive! :slight_smile:
Project can be found here: https://www.simscale.com/workbench?publiclink=1168ad96-5ae6-4def-93cb-e0d137b44c0d

Cheers!


#15

@jhorv_th Good to know that you simulations are working. Well the slip BC on the walls, ensures that velocity won’t be effected by walls. If the velocity fluctuates within the domain, say due to geometry or turbulence, then this effect will also be projected to walls if walls are close to the disturbance region. In my case I kept the no slip on walls, because walls are far enough from geometry so they won’t effect the flow. Simply if walls are far enough from the body, its safe to use no slip at walls. If they are close to to the body then use slip. Have fun :slight_smile:


#16

@jhorv_th and @AsadAli, I’ve really enjoyed watching the progress on this project - great work :smile: