Nodal Solutions 1

[navash]

Hi All,

1) Can we define "Nodal Solutions Table" similar to that of "Element Table" and save the results in ".lis" file or ".xml" format

2) Can we automate or write a script to save Nodal solutions parameters in all substeps in the directory with some naming convention(can be .lis format)

Thank you so much,

Regards,
-N

 

[cbrn]

Hi,
1), yes. PRNSOL command prints nodal solution(s)
2) yes. Requires APDL programming.

Regards

 

[navash]

Thanks Cbrn,

1) I will read more about PRNSOL command and get back to you.

2) I have 4 load steps and each has 11 substeps.
Now I manually (in GUI) list nodal solutions and save with naming convention (1 1 1), (1 1 2) and so on until (4 11 3), which means (Loadstep, Substep, Filenum), without parenthesis.

Can you give me an idea of the key commands to do something like this.

Basically I need to save .lis files with SX, SY, SZ, SXY, SYZ, SZX, S1, S2, S3, SEQV, HPRE, EPEQ values and then convert .lis files to XML spreadsheets

Thank you
Regards,
-N

 

[navash]

Regarding 1)

Basically I need to save .lis files with SX, SY, SZ, SXY, SYZ, SZX, S1, S2, S3, SEQV, HPRE, EPEQ values.

For elements, I can define an Element Table in GUI with all components in one table and save the listing as .lis file

So I was asking if we could have one table with all these values for Nodal solution.

Sorry for the confusion

Thanks
-N

 

[cbrn]

Hi,
well, yes, you can ask for more than one ETAB to be printed out in a file, but there is a limitation in their number, I can't recall how many, and most likely the ones you need are far more.
You can incorporate in the APDL all the directives you give by picking in the GUI, and even many more.
Each GUI command has its "APDL-equivalent", e.g. "Plot Results -> Nodal Results -> X Displacement" is trivially "PRNSOL,...,UX". Many times you see in the dialog boxes the names of the APDL commands. In addition, each time you issue a GUI command, have a look in the Output Window: it will print the execution of the APDL command underlying...
Managing filenames parametrically from within an APDL script is possible, but it will require formatting strings etc. The Help is not very clear and user-friendly about this subject, but you can find it.
However, if you know "a priori" the names of the files, the numbers of the steps and substeps, etc, then everything will become trivial (a long list of repeated commands).
Bear in mind that ANSYS Classical doesn't even know what xml is. Only plain-text, fixed-width.

Regards

 

[navash]

Now I am looking for simpler options.

Is it possible to write "PRNSOL, S, Comp" to a file "s.dat"
on my system.

I have tried typing this in command window

/output, s,dat
prnsol, s,comp

and then it pops-up
PRNSOL is not a recognized begin command

How do I go about it..
I am a beginner on ANSYS..its getting interesting,

Regards,
-N

 

[cbrn]

Hi,
it's because Ansys is organized in "modules", or "ambients":
"BEGIN" is the first "gateway" to Ansys. If you use Unigraphics, then you may be familiar with the "Gateway" concept. It's the "ambient" where you setup the generic configuration options. You are in the "BEGIN" whenever you start a new job or whenever you finish (NOT exit !!!) operating with another module (via the command FINISH).
"PREP7" is the preprocessor. Please note that even in Workbench, if you wanted to insert a Commands snippet you might need to re-enter the preprocessor and it would be called exactly the same. There are a lot of commands which are PREP7-specific, they do NOT work with ANY other module. In APDL, you call the preprocessor with the command "/PREP7".
"SOLU" is the solution module (the solver ambient). Once again, there are commands which work only within SOLU.
"POST1" is the "single-step post-processor", the one where you can access ALL nodal and element results of any kind, for ALL the nodes at the same time, but ONE substep (timestep) at a time. Some commands are valid only in POST1, of course, AND THIS IS THE CASE OF THE PRNSOL, PLNSOL, ETC COMMANDS !!!
"POST16" is the "time-history post-processor", the one where, when applicable, you can retrieve results for SOME selected nodes only, but over the whole timesteps in your analysis.
There are also some minor modules, such as the "Auxiliary" ones which serve principally for 3D-solid models import, etc...
Of course, there are lots of commands which work indifferently in all the modules.

The structure of ANSYS should be very well described in the Help, please have a thorough reading of the Manual before attempting "semi-advanced" operations such as the ones you are trying...

However, the solution (!) to the error you get is simply to enter the post-processor POST1, either by GUI pick, or by adding the /POST1 command in the APDL before issueing the PLNSOL command. Please also note that you must be sure to have the results file loaded in memory. This is automatic after a SOLVE command, otherwise you have to load the results file AND read-in the loadstep (SET) you need.

Regards

 

[cbrn]

... sorry, in the second-last line, I wanted to write "PRNSOL", not "PLNSOL".

 

[navash]

I got it. It prints to file. Thank you so much
I will keep working on this to make it better.

Thanks again.
-N