Applynig Pressure To Shell Element

[AltoAuto]

Recently, though, I’ve run into a challenge while working with SHELL181 elements. Since shell elements represent 2D geometry with a defined thickness, I understand that pressure application works differently than with solids. Currently, I’m using the SFE command to apply pressure, but I’m not entirely confident if I’m doing it correctly or if there’s a better approach specific to shell elements.

Here’s the current setup I’m testing (summary only — full code below):

Defined a rectangular shell area using

mapdl.blc4(0, 0, 100, 20)

Assigned SHELL181 with SECTYPE and SECDATA
Applied pressure on the right edge using:

mapdl.asel("S", "LOC", "X", 90, 100)
mapdl.esla("S")
mapdl.eplot()
mapdl.sfe("ALL", 1, "PRES", 1, 25)
and currently eplot doesn't show me anything

UserWarning: There are no elements to plot. warnings.warn("There are no elements to plot.")

What’s the correct or recommended way to apply pressure to shell elements (like SHELL181)?
Should I continue using SFE, or is there a better method (e.g., force-on-nodes or other shell-specific loading strategies)?
Also, any insight into how MAPDL internally interprets these loads on shell geometries would help me better understand how to handle face mapping when automating this through a GUI.

Appreciate your time and any guidance you can share!

Best regards,
Aiden Wang

[AltoAuto]

from ansys.mapdl.core import launch_mapdl

mapdl = launch_mapdl()
mapdl.clear()
mapdl.prep7()

# 1. Define Element Type, Section, Material
mapdl.et(1, "SHELL181")
mapdl.r(1, 2)  # thickness = 2 mm
mapdl.sectype(1, "SHELL")
mapdl.secdata(2)  # thickness again for the section

mapdl.mp("EX", 1, 210000)  # MPa
mapdl.mp("NUXY", 1, 0.3)

# 2. Create Geometry (100 mm x 20 mm)
mapdl.blc4(0, 0, 100, 20)

# 3. Mesh
mapdl.esize(3)
mapdl.amesh("ALL")
print(mapdl.etlist())
# 4. Fix left edge
mapdl.nsel("S", "LOC", "X", 0)
mapdl.d("ALL", "ALL", 0)
mapdl.nsel("NONE") 

# 5. Apply pressure force on right face
mapdl.asel("S", "LOC", "X", 90,100)
mapdl.esla("S")
mapdl.eplot()   
mapdl.sfe("ALL", 1, "PRES", 1, 25)

mapdl.allsel()
mapdl.finish()

# 6. Solve
mapdl.slashsolu()
mapdl.antype("STATIC")
mapdl.solve()
mapdl.finish()
mapdl.post1()
mapdl.allsel()
mapdl.set('last')
mapdl.upcoord(1)
mapdl.eplot(cpos='xy', background='black', color='blue',edge_color='white')
mapdl.upcoord(-1)
# 7. Post-processing
mapdl.post1()
mapdl.set(1)
mapdl.view(1, 1, 1, 1) # Isometric 3D view
mapdl.vup(1, "Y")          # Set view direction (Z is up)
mapdl.shade("ON")

mapdl.plnsol("S", "EQV",2)
mapdl.psf("PRES", "NORM", 2, 0, 1)
mapdl.view(1, -1, 1, 1)
mapdl.eplot(vtk=False)
mapdl.post_processing.plot_nodal_eqv_stress(show_edges=True)

[mikerife]

Hi @AltoAuto accidentally selecting area here instead of elements:

# 5. Apply pressure force on right face
mapdl.asel("S", "LOC", "X", 90,100)
mapdl.esla("S")
mapdl.eplot()   
mapdl.sfe("ALL", 1, "PRES", 1, 25)

Use instead:

# 5. Apply pressure force on right face
mapdl.esel("S", "CENT", "X", 90,100)
mapdl.eplot()   
mapdl.sfe("ALL", 1, "PRES", 1, 25)

MIke

[AltoAuto]

you the goat Mike! Thanks.

One quick question about how MAPDL handles shell thickness. I created a thin plate using SHELL181 (100 × 20 midsurface) and defined the thickness using secdata(2). Then I applied a surface pressure using SFE, and I noticed that my von Mises stress came out about half of what I expected based on solid element results. Why is that? Below is the VM result plot

[mikerife]

Hi @AltoAuto I can't really comment as I don't have access to the solid element script. And the results you posted don't match the input (pressure is normal to the material but the results show a in-plane pulling of the material). Here is a example so we can discuss:

from ansys.mapdl.core import launch_mapdl
import os
path = os.getcwd()
mapdl = launch_mapdl(run_location=path)
mapdl.clear()
mapdl.prep7()

# 1. Define Element Type, Section, Material
mapdl.et(1, "SHELL181")
mapdl.sectype(1, "SHELL")
mapdl.secdata(2)  # thickness

mapdl.et(2, "186")

mapdl.mp("EX", 1, 210000)  # MPa
mapdl.mp("NUXY", 1, 0.3)

# 2. Create Geometry (100 mm x 20 mm)
mapdl.blc4(0, 0, 100, 20)
mapdl.block(0, 100, 0, 20, 10, 12)

# 3. Mesh
mapdl.type(1)
mapdl.esize(3)
mapdl.amesh(1)

mapdl.type(2)
mapdl.vsweep(1)

# 4. Fix left edge
mapdl.nsel("S", "LOC", "X", 0)
mapdl.d("ALL", "ALL", 0)

# 5. Apply pressure force on right face
mapdl.esel('s', 'type', '', 1)
mapdl.esel("r", "CENT", "X", 90,100)
mapdl.sfe("ALL", 1, "PRES", 1, 25)
mapdl.allsel()

mapdl.esel('s', 'type', '', 2)
mapdl.esel('r', 'cent', 'x', 90, 100)
mapdl.sfe('all', '1', 'pres', 1, 25)

mapdl.allsel()
mapdl.finish()

mapdl.slashsolu()
mapdl.solve()
mapdl.finish()

mapdl.post1()
mapdl.set('last')
mapdl.post_processing.plot_nodal_eqv_stress(cmap='jet')