No SMISC result, model specific

[mikerife]

Hi @ShaileshFle
Regarding the modle and results from this Discussion

The input file defined a table array that seems to be used to apply a +/- 0.5 displacement. But the commands to actually apply the displacement, and use the table, were missing. So there was not load on the model; hence no results; so retrieving smisc 13 failed as there was no data to retrieve.

Also select logic had been used to select a sub-set of the model prior to solving. So the whole model was not solved for. Be sure to include a ALLSEL prior to solving.

Mike

[germa89]

Why a new discussion and not replying in the previous one?

[ShaileshFle]

Hi, I had removed everything below /SOLU as it was not solving and someone in the forum suggested to remove and solve. Even when I keep those, I am getting the same error. I have also attached the file for your reference.
model1_input09.txt

[mikerife]

Hi @ShaileshFle Which forum? That is very wrong advice! Or very incomplete advice: you will need to add to the PyMAPDL script to replace what was deleted from the inp file that which is needed. Like the creation of the node component that is then used to define the applied displacement. And that applied displacement command. Then the solves at the different time points. Do you use a commercial license?
Mike

[ShaileshFle]

Hi, Yes I have enterprise and premium license. I got this advice on Ansys Pyansys Forum not on GitHub forum. I have a good experience with python, but I am very new to pyansys, so I am not very familiar with and hence struggling to carry out and understand things here. Is it possible for you to arrange any call to discuss, it would be easier that way?

[mikerife]

Hi @ShaileshFle
Ok - if the TECS is current on any of the licenses then next time go ahead and open an technical support call in the typical manner. On the support case make it clear that while you are using PyMAPDL, you have a MAPDL question.

Here is the modified input file for you to review:

model1_input09.txt

And the PyMAPDL script to do what you want:

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

mapdl = launch_mapdl(run_location = path)

mapdl.clear()
_ = mapdl.input(r"model1_input09.txt")

mapdl.allsel()
mapdl.finish()
mapdl.slashsolu()
mapdl.outres('erase')
mapdl.outres('all', 'all')
for i in range(1,5):
    mapdl.time(i)
    mapdl.solve()

mapdl.finish()

Now the kind of tricky part: if the contact element is not in far open state then nothing is written for it in the result file with respect to results. If you try to retrieve a result for a contact element in an far open state with *GET then it will fail with the "SMISC data is not stored...." message. So instead of looping over all the contact elements we can get a list of contact elements that have something other than a far-open state with the PRESOL command (NMISC 41 is the state) and use a modifier to dump it to a list. Then loop over that list and retrieve the contact pressure for the element IDs in the list:

mapdl.post1()
mapdl.set('last')
mapdl.esel('s','ename','',174)
mapdl.nsle()
list_elements_ids = mapdl.presol('nmisc',41).to_list()
mapdl.allsel()

pres_list = []
for id in list_elements_ids:
    pres_list.append(mapdl.get_value('elem',id[0],'smisc',13))
pres_list, list_elements_ids

Give that a shot and if you have any MAPDL questions then please do open a technical support case.

mike

[ShaileshFle]

Hey, Thanks it works. I have just one thing, by technical support case do you mean Ansys support because last time when I asked them for support they replied that "Ansys does not support on pyansys and to refer to forum".

[mikerife]

Hi @ShaileshFle yes I do mean Ansys support; and why I ask you to make it clear to them that you have a MAPDL issue i.e. properly editing a WB Mechanical input file for later use.

[ShaileshFle]

Ok, Thanks!