Diference between pure APDL and pyansys

[wmpjrufg]

I modeled the same 2D structure using both APDL commands and PyAnsys (MAPDL). The structure consists of a rectangular element (b × h) with an internal "knot" region (assigned a significantly lower elastic modulus).

Problems:
Stress Distribution:

• Only the boundary between the two materials shows different stresses.
• All other points exhibit equal stress values.

Discrepancy in Results:

• Using PyAnsys, the element stresses returned zero for all elements.
• In pure APDL, the stresses were non-zero (as expected).

I’m sharing both files for reference:
apdl.txt
Python file pyansys.txt

Could you help identify why PyAnsys reports zero stresses and stress difference when compare APDL?

I'm using mechanical APDL 2024 R2

[mikerife]

Hi @wmpjrufg The PyMAPDL script is trying to post process while still being in the Solution processor.

Also...why use "run" so much? And why use shell63? Shell181 replaced shell63 years and years ago.

[wmpjrufg]

Thanks @mikerife

Your script PyAnsys works fine, but I wrote a pure APDL script. When running PyAnsys, the step max(w) returns 37.21078545588245 MPa, whereas in APDL Ansys, max(w) returns 49.41 MPa. Can you help me?

FINISH
/CLEAR

! Parameters
b = 100
h = 100
espessura = 50

e_mod = 11889
v = 0.4
g_mod = 560

e_mod_no = 0.00000001
v_no = 0.4
g_mod_no = 560

no_dim = 10
refinamento = 5
press = -1000

! Preprocessing
/PREP7

! Element types and sections
ET,1,SHELL181
SECTYPE,1,SHELL
SECDATA,espessura

ET,2,SHELL181
SECTYPE,2,SHELL
SECDATA,espessura

! Material properties
MP,EX,1,e_mod
MP,PRXY,1,v
MP,DENS,1,g_mod

MP,EX,2,e_mod_no
MP,PRXY,2,v_no
MP,DENS,2,g_mod_no

! Geometry
CYL4,b/2,h/2,no_dim

! Create rectangular area
K,5,0,0,0
K,6,b,0,0
K,7,b,h,0
K,8,0,h,0

LSTR,5,6
LSTR,6,7
LSTR,7,8
LSTR,8,5
AL,ALL

! Meshing - Circular area (Material 2)
ASEL,S,AREA,,1
TYPE,2
MAT,2
SECNUM,2
AESIZE,ALL,refinamento
MSHAPE,1,2D
MSHKEY,0
AMESH,ALL

! Meshing - Rectangular area (Material 1)
ASEL,S,AREA,,2
TYPE,1
MAT,1
SECNUM,1
AESIZE,ALL,refinamento
AMESH,ALL

! Boundary conditions
NSEL,S,LOC,Y,0
D,ALL,ALL

! Pressure load
LSEL,S,LOC,Y,h
SFL,ALL,PRES,press

ALLSEL
FINISH

! Solution
/SOLU
ANTYPE,0
SOLVE
FINISH

! Postprocessing
/POST1
SET,LAST

[wmpjrufg]

When assessing stress at other points, the stress values along the y-axis are equal. However, at the boundary between element 1 and element 2, pure Ansys and APDL show divergent results.

Element stress are equals in the both scripts.

[mikerife]

Hi @wmpjrufg remember that MAPDL has two methods of averaging and presenting result data to be plotted: 'Full' and 'Power' graphics. MAPDL running batch defaults to Full graphics while running interactively defaults to Power graphics. PyMAPDL is a third method of running MAPDL which is a hybrid where inputs are interactive but outputs are batch. So you are comparing the Full to the Power graphics results. The values are expected to be different as the model has two parts (with distinct material, element type etc). So the averaging across the boundary is different.

You can check this by using /graphics,full then replot the Y stress in MAPDL and you should see the plot change where the maximum is 37 etc.

So first you need to decide what you want with respect to averaging at the boundary. Then post process that. The native PyMAPDL post processing is akin to Full graphics. I had a PyMAPDL documentation example model of how to create native PyMAPDL plots that mimic Power graphics...but I see the site has been updated and my example is gone. I'll see what happened there and either get it reposted or track down where I saved the darn thing on my work computer and post it here.

Mike

[mikerife]

@wmpjrufg found it; the Example page layout changed is all. https://mapdl.docs.pyansys.com/version/stable/examples/gallery_examples/00-mapdl-examples/2d_magnetostatic_solenoid-BodyFlux_Averaging.html#sphx-glr-examples-gallery-examples-00-mapdl-examples-2d-magnetostatic-solenoid-bodyflux-averaging-py

[wmpjrufg]

thanks @mikerife

[germa89]

As @mikerife mentioned, the differences between pure APDL and PyMAPDL (PyAnsys) are due to the different averaging method because the choosen graphics.

Hi @wmpjrufg remember that MAPDL has two methods of averaging and presenting result data to be plotted: 'Full' and 'Power' graphics. MAPDL running batch defaults to Full graphics while running interactively defaults to Power graphics. PyMAPDL is a third method of running MAPDL which is a hybrid where inputs are interactive but outputs are batch. So you are comparing the Full to the Power graphics results. The values are expected to be different as the model has two parts (with distinct material, element type etc). So the averaging across the boundary is different.

You can check this by using /graphics,full then replot the Y stress in MAPDL and you should see the plot change where the maximum is 37 etc.

...

Mike

Originally posted by @mikerife in #3928 (reply in thread)

The explanation why this happens is in here: https://mapdl.docs.pyansys.com/version/stable/getting_started/faq.html#listing-results

Example link: https://mapdl.docs.pyansys.com/version/stable/examples/gallery_examples/00-mapdl-examples/2d_magnetostatic_solenoid-BodyFlux_Averaging.html#analysis-of-a-2d-magnetostatic-solenoid

[wmpjrufg]

@mikerife @germa89

As you can see the PowerGraphics is plotting as intended. However, we should be able to extract the SMX = 49.41; Even after defining "mapdl.graphics("POWER")" and running the command mapdl.post_processing.nodal_stress_intensity() or mapdl.post_processing.nodal_principal_stress('1') the result is still 37. Is there any way to extract the 49.41 value via output?

I need this result in a variable to use in other functions (optimziatioon and reliability analysis)

[mikerife]

Hi @wmpjrufg the PyMAPDL post_processing method is native to PyMAPDL and does not 'respect' commands to set up graphics etc from MAPDL. So the mapdl.graphics('power') has no effect on mapdl.post_processing.nodal_principal_stress('1'). If you want to stick with the post_processing method but match the MAPDL power graphics result, you need to gather the results on a part-by-part basis. Since we know that the model only has two parts; each part defined by a unique material and element type ID; and are meshes that share nodes (as opposed to connected by contact or some other element based method) we can simply loop over the unique IDs. A more generic version would be something like this...

import numpy as np

mapdl.post1()
mapdl.set('last')
mapdl.allsel()
result_value = []
for mat in np.unique(mapdl.mesh.material_type):
    mapdl.esel('s', 'mat', '', mat)
    mapdl.nsle()
    result_value.append(max(mapdl.post_processing.nodal_principal_stress(1)))
mapdl.allsel()
print(np.max(result_value))

Mike

[germa89]

PyMAPDL uses *VGET to obtain the nodal_principal_stress (and other results).

ansys/pymapdl-reader#185 (comment)

[germa89]

Eventually we are going to have to provide a more consistent API, or better docs that explain the differences.

[wmpjrufg]

Folks, thank you so much! I will finish this topic...bye bye.