Applying increasing force over time in a specific point

[Deternanna]

Hi everybody,
I have looked and looked and looked and I can't find any examples of where you apply an increasing load to a specific point over a decided amount of timesteps. Is that something you guys could help me with? Here is what I have in my script so far.

I have applied the following boundary conditions to the structure and where the pink arrow is, is where I have added a constant force to my structure. I want to now change that constant force to a force that gets bigger over time (until a certain failure criteria, that I haven't decided on yet). Is there a way I can do that in a "static" analysis?

The force is currently added like so,

mapdl.nsel("S", "LOC", "Y", y3) mapdl.f("ALL", "FY", P)

I have tried adding in substeps like so, but its not really working as intended,

mapdl.run("/SOLU")
mapdl.antype("STATIC")

#Activate non-linear geometry
mapdl.nlgeom("on")

#Request substeps
mapdl.autots(key="on")
mapdl.nsubst(nsbstp=100, nsbmx=10, nsbmn=10)
mapdl.kbc(key=0)
mapdl.outres("all", "all")
mapdl.eqslv("SPARSE")
mapdl.solve(mute=True)

Also, I would really like to be able to plot a force-displacement plot for the node where the force is applied.

Thank you in advance!

[mikerife]

Hi @Deternanna
Well, you are already modeling what you are asking for! KBC=0 is a linear interpolation of the load over the "time" of the sub-step. So since the initial number of sub-steps is 100 the first sub-step takes 1/100 of the time and load. Let's say the second sub-step is another 1/100 of the total time. Then another 1/100 of the load is applied (so total is now 1/50 of the total load). Continues on till the end an 100% of the load applied.

I think what you are asking is can you increase the load at the end of the solution in the case that the load was not large enough for your failure criteria? If so there are a few paths that could be taken: restart vs applying huge load and stopping the solve when some criteria is met. Which to use depends on the end goal.

In a static analysis if we make the end time equal to the applied load, then time history plots are also load history plots. If not that then in the time history post processor the XVAR command sets what the X axis variable is. By default it is time (or frequency if harmonic) but you can point it to use some other variable.

[Deternanna]

Hi Mike,

Thanks for your response! I just don't feel like my model is responding the way you are saying it should. If I make the load bigger, going from -1 N to -10 N, my plot end up looking like this, using the following script, (I am also not aware if I am just plotting the first time step and that is the reason nothing is happening)

mapdl.post1()
mapdl.post_processing.plot_nodal_displacement(
    "Y",
    cmap="jet",  # 'turbo' or 'coolwarm' are also nice
    line_width=3,
    cpos="xy",
    scalar_bar_args={"title": "Displacement", "vertical": True})

Is there a way for me to make this time-history plot, so I can check if the load is in fact applied correctly. The only thing I can manage to get out is the timesteps, where the substep counter is going all crazy in the end.. I don't know if that means anything. Hope you can help.

[mikerife]

Hi @Deternanna So two things; the big one first is that sub-step 999999 means that the solution did not fully converge and the 'non converged' results written to the result file at sub step 999999. Is this structure collapsing? Or intended to collapse?

PyMAPDL has a command to check the convergence of a solve: see here

When post processing using the post1 processor a good practice is to read the results in from the result file to the MAPDL database (in memory). So try:

mapdl.post1()
mapdl.set('last')
mapdl.post_processing.plot_nodal_displacement("Y", cmap="jet", cpos="xy")

Mike

[Deternanna]

Hi Mike,
Thank you! That makes a lot of sense! The idea behind this analysis is to change the geometry of the structure and then apply load until failure to see if the change in geometry will change the rate of deformation in the node where the force is applied. But I think I might try to just pick a load where the result can converge for now. Is it possible you can give me an example of how to make a time-history plot (force over time plot)? Can I access the information on the deformation at a specific point over the time steps as well?

[Deternanna]

Hmm, if I chose to not make my geometry non-linear, it seems like my solution can not be converged.

[mikerife]

@Deternanna that makse sense given how linear and non-linear solutions are done and the definition of converged.

[mikerife]

I should add a P.S. that the native PyMAPDL post processing plots the results on the as-defined geometry and not the deformed geometry. The PyMAPDL Reader has an option to show the deformed mesh on the result plot. Or, as I prefer, we can use the upcoord, mesh.grid, and standard PyMAPDL results to make our own PyVista plot of a result on an deformed geometry.

[Deternanna]

Oh really, is that possible? Could you give me an example of how you would use the upcoord, mesh.grid to make a plot of the results on the deformed geometry? I would love to be able to do that!

[Deternanna]

@mikerife is it possible you can help me out making this?

[mikerife]

Here is a small example using a generic solid model of a cantilever beam.

from ansys.mapdl.core import launch_mapdl
import matplotlib.pyplot as plt
import pyvista as pv

mapdl = launch_mapdl(port=50056)
mapdl.units('bin')
mapdl.clear()
mapdl.prep7()

mapdl.et(1, 185)

mapdl.mp('EX', 1, 1E7)
mapdl.tb('plas', 1, 1, 1, 'biso')
mapdl.tbdata(1, 50_000, 5E6)

mapdl.blc4(0, 0, 24, 0.5, 1)
mapdl.esize(0.25)
mapdl.vmesh(1)

mapdl.nsel('s', 'loc', 'x', 0)
mapdl.cp(1, 'all', 'all')
node_bc = mapdl.queries.ndnext(0)
mapdl.allsel()
mapdl.finish()

mapdl.slashsolu()

mapdl.d(node_bc, 'all', 0)
mapdl.nsel('s', 'loc', 'y', 0.5)
mapdl.sf('all', 'pres', 20)
mapdl.allsel()

mapdl.time(20)
mapdl.nsubst(20, 100, 20)
mapdl.nlgeom('on')
mapdl.outres('all', 'all')
mapdl.solve()
mapdl.finish()

mapdl.post1()
mapdl.set('last')

# standard result plot
mapdl.post_processing.plot_nodal_displacement('NORM', cpos='iso', cmap='jet')

result = mapdl.post_processing.nodal_displacement('NORM')
mesh_1 = mapdl.mesh.grid
mapdl.upcoord(1)
mesh_2 = mapdl.mesh.grid
mapdl.upcoord(-1)
plot = pv.Plotter()
plot.add_mesh(mesh_1, color='b', style='wireframe')
plot.add_mesh(mesh_2, scalars=result, cmap='jet')
plot.show(cpos='iso')

# let's do a XY graph too as why not
mapdl.finish()
mapdl.post26()
mapdl.file('file', 'rst')

mapdl.nsel('s', 'loc', 'x', 24)
node_load = mapdl.queries.ndnext(0)
mapdl.allsel()

mapdl.rforce(3, node_bc, 'f', 'y')
mapdl.nsol(4, node_load, 'u', 'y')
mapdl.vget("FYN", 3)
mapdl.vget("UYN", 4)
plt.plot(abs(mapdl.parameters["UYN"]), mapdl.parameters["FYN"])
plt.xlabel("Displacement inch")
plt.ylabel("Reaction Force lbf")
plt.show()

mapdl.finish()
mapdl.exit()

[Deternanna]

Thank you so much, this was really helpful!