Mesh for hydrostatic pressure
Altair EmployeeHello,
I have to apply hydrstatic pressure onto the lower part of my model. See attached picture. (this is a barge within the water)
-Should I model 2 different blocks? And then mesh both, and apply pressure > equation > hydrostatic pressure?
-Should I model 1 solid block and then split the mesh somehow?
-Should I model 1 solid block and am I able to select nodes/elements up until the waterline?
Thanks in advance.
Best regards,
Joep
<?xml version="1.0" encoding="UTF-8"?>
Answers
-
Hello,
I think this would be the better option
Altair Forum User said:Should I model 2 different blocks? And then mesh both, and apply pressure > equation > hydrostatic pressure?
as splitting the mesh can be a tricky job and you can get different results if you miss some elements.
Thankyou
0 -
For applying hydrostatic pressure, you need split the surface.
0 -
Hello, thanks for the reply.
If I split the surface, and want to apply hydrstatic pressure using an equation I can either select ''face'' or ''elements''. Using elements.
Only using elements I can use the equation option.
How can I select the bottom surface (split surface) by using ''equation'' for hydrostatic pressure?
Best regards,
Joep
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
Here's my test of hydrostatic pressure (entered by equation) over face of solid elements:
0 -
Thanks a lot for the test and picture..!
I can only add either a pressure without equation onto a surface (as seen by the PLOAD4 arrow), either select different elements (as checked in the picture) but then no pressure is seen after clicking create..
Can it be my model is not a solid or something?
Best regards,
Joep
0 -
<?xml version="1.0" encoding="UTF-8"?>
0 -
Hydrostatic pressure is perpendicular to element/surface. While as you define 'Y-axis' (under equation) ???
0 -
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
Thanks for the reply and for helping me! The y-direction was a wrong picture.
The problem is: I can select the entire face/surface using : elelements > faces, but I only want to select the bottom half of the rectangular..
If I use elements > elements I can select each element individual while still using an equation.
Any thoughts?
best regards
0 -
Hello,
As you have split the face and they are in the same component you need to select the bottom elements individually. As these are 2D elements and pressure is applied only on one side i don't think selecting them individually should be a problem.
Thankyou
0 -
Hello,
Thanks for the reply. In this case it is not a problem, since there are not that much elements.
But I have to do this for a very big part with very much element.
What will be the best way to do this then?
Maybe I do not need to split the face, but do this another way?
best regards, thanks for helping me.
Joep
0 -
To define the border of pressure area, you need split your surface/solid.
0 -
Thanks for the reply.
I have finally managed to get hydrstatic pressure.
I also know how to split surfaces.
But now I have to add hydrostatic pressure on this model:
I think I have to do this:
1. split surfaces with a hoorizontal straght line (how can I split the globe with a straight line?)
2. add hydrostatic pressure on the bottom side of the rectangular shape and on the bottom side of the globe, without having to select all elements individually
3 apply constaints and perform SPC with constraint, presure and additional loads in a load collector (with card image LOADADD) and then create a subcase.
Can anyone help me with step 1 and 2?
Best regards,
Joep
<?xml version="1.0" encoding="UTF-8"?>
0 -
Hi,
1) Enter panel geom>surface edit>trim with plane
select all surfs
select plane as 'z-axis' and select base node 'B' at the position you expect (hold down left mouse on the surface until it is highlighted, then you can click to select 'B')
- click 'Split'
2) Automesh your model,
enter analysis>pressure
set the equation of pressure
select elems> by geom> surfs => select surfs that need to apply pressure > add to selection > create
don't think that you have to select elements one by one
0 -
Hello,
As stated in the above post use the by geoms option:
<?xml version="1.0" encoding="UTF-8"?>
Then select the elements by surface
<?xml version="1.0" encoding="UTF-8"?>
As you have already split the surface this will now select only the bottom surface.
Thankyou.
0 -
Hello,
Thanks for the great help! Now I have managed to get a straight split line and I can select the elements using an equation by By geom.
There is only 1 more thing, If I select Add to selection, there is no chenge done, no elements/surfaces selected..
Is this becasue this does not work if I performed tetramesh? Since it did work when using (2D) automesh.
Best reggards,
Joep
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
You have to make :
- Select elements
- Select 'nodes on face'
Hypermesh will combine two these selections to determine the face of your solid elements to apply the pressure.
0 -
Hello,
It is still not possible to select the elements using 'by geoms' and then select 'add to selection''.
It only works when if perform a 2D-mesh.
I performs a tetramesh. Can this be the cause?
Best regards,
joep
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
you need to select the nodes also using the same 'by geom' option
<?xml version="1.0" encoding="UTF-8"?>
Thankyou
0 -
Hello, Thanks for the reply.
I am still unable to select the elements. After clicking ''by geoms'' > add to selection, no elements get selected.
I am able to select the nodes.
Does it really have nothing to do with difference automesh / tetramesh?
Best regards,
Joep
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
You can make element selection manually , approximately.
Combining with an exact selection of nodes (thanks to surface splitting), you will got the correct surface for pressure.
0 -
Have a look at my video:
0
