Hydrostatic simulation problem

Out of category
1

Hello

I need to model a hydrostatic pressure and I am having problems with inconsistent results.

I modeled a 15mm thick steel tank, 1000x1000x1000 => 1m3 => 1000kg of water

I made 2 calculations

- 1 or I model the non-uniform pressure by following what you find on the internet

9810 N/m²

Equation 1*"y"

I get an astronomical deformation of 214mm!!

- I do a 2nd calculation where I just put a force of 10000N or a pressure of 10000N/m² or a distributed mass of 1000Kg on the bottom of my tank.

There I get a reasonable deformation of 0.34mm

I don't understand this inconsistency.

Can anyone help me?


Part1.SLDPRT
2

Hello@phiphi_38

Would you be so kind as to complete your profile please  ;-) In particular teaching in what and where please, ditto for trainer ;-)

Moreover, for your results from what I see on the images, I read 2.14 mm and not 214 as you indicate in the body of the text and 3.45mm and not 0.34 mm.

In addition, when you open your file, you have no materials for the tank. You have not submitted the results of your simulations l(the results are empty).

Can you send your file back using pack and go so that the simulation results are also transmitted.

Kind regards

1 Like
3

Hello,

I quickly redid the calculation 

  • 15 mm shell mesh
  • Variable pressure depending on the water level
  • I added gravity

I checked the reaction forces: It's correct (9810N + 5900N)

If I haven't made a mistake, the max deflection at the bottom of the tank is about 0.3 mm

Cdlt

Alan


image_273.png
4

Hello Alain;-)

Can you post your file with the results of the STP simulation.

Kind regards

5

Hello Zozo

The values are in scientific notation 2.14 10+2 and 3.45 10-1

There are the materials in the simu if not we can't calculate

I don't put the results files because it's very very large. it's faster to restart the calculation on your computer than to load a 40MB zip

6

Hello Alain,

Thank you for your answer.

Can you attach your file so that I can look at the values you put for your variable pressure.

Personally I relied on this link to fill in the values: https://www.visiativ-solutions.fr/pression-hydrostatique-modeliser-solidworks-simulation/

In fact I looked at my reaction forces too and I have a factor 1000 error.

I have 9.81 10+6 N instead of 9.81 10+3 N

 

7

I was the one who wrote this article smiley .... a long  time ago

The interface has changed since then 

We must pay attention to the unit of pressure and the unit of the equation 

To check, at the bottom of the tank (1m) we must have 0.1 bar or  about 10000N/m2

You also always have to check the reaction forces!

I put a rar file attached: It's sw 2020!

 

 


calcul.rar
1 Like
8

Thank you Alain!!

It was indeed the "m" unit that you circled that I hadn't seen.

Now it's all good.

Bonus question:

Pressure loading applies pressure to the walls but does it also apply mass to the fixing points?

9

Good evening Philippe

Answer YES since you have gravity and mass.

On the other hand, with the constraints put on the edges, it's not famous compared to reality because you blocked if I saw all the DDLs.
In real life, your upper edges would be deformed because the angles are more robust and the sides should swell like the middle of the tank. But we agree that as long as we don't know how the top of the tank is fixed and especially on what, we can only make a remark without more ;-)

Kind regards