After getting the solution you need to use the /POST1 processor : its menu is easier to list any result or graphics or animations at exact locations. If it is a dynamic analysis use READ RESULTS, FIRST SET or other set until LAST SET. Use also RESULTS VIEWER, PLOT RESULTS, ANIMATE. Several data can be listed from the main menu : points, elements, nodes and corresponding displacements, strains, stresses. I suggest that youselect from these values the searched data and save them in a file.

Let me describe my understanding from your question first. You are trying to automate an analysis in workbench, basically manipulate an input parameters first, solve the analysis and extract the result to Matlab and loop over again. If you just want to extract the last substep result from WB, then it is not required to use Matlab and you can just follow the same methodology that described in the attached files. This is a good example of manipulating WB using Excel. You can do the same thing with Matlab in conjunction with Python programming, however it will be a lot complicated and required advance scripting capability. Also, for both of these methodes it is not required to use "Write Input Files" command and later on change the text for reflecting the new input parameter. Using this method make your script a lot more complicated for nothing!!

Thanks all for the input.

This is the command snippet I have inserted in the solution section

*cfopen,timedata.txt ! timedata.txt created in working folder

*VWRITE,time(1),Dy(1)

(F10.0, F10.0) ! number Format

*cfclose

I expected this to print out a 2 column table in the text file "timedata.txt" with the first column being time and the second column being deflection data at the probe. However, it does not print anything.

Possible reasons:

1. time, Dy are not valid variables to use. If so how can I check under what variable names they are stored?

2. I am not reading the valid variables first. As suggested by Mohammed Lamine Moussaoui, however I do not know how to do that.

3. I am not looping through all the time instances, again I do not know how to do that. I read examples that "time(1)" is sufficient to tell APDL that this is a vector of values and needs to be looped through

Thanks once again.

Dear Punnag Chatterjee ,

The commands that I have cited are available in Ansys interactive mode corresponding to the first window when you launch the apdl software.

Hello all,

I have found the solution to write the command snippet that would print the table to file. However, it does not print the probe data but it can print a "named selection" nodal point's displacement vs time data. Which also works for my case. Thanks to a friend of mine from Bajaj Auto Limited, Mr. Manoj Sharma who helped me with this.

Probe_pt is the named selection of a meshed nodal point.

!***********APDL code snippet*************

set,last

*get, nsets,active,0,set,nset

*dim, data_store,,nsets,2

*do,i,1,nsets

set,next

*get,t,active,,set,time

cmsel,s,Probe_pt

*get,node_id,node,0,num,max

*get,displ,node,node_id,U,sum

data_store(i,1) = t

data_store(i,2) = displ

*enddo

*cfopen,try,txt   !filename is try.txt which is a 2 column table of time & disp

*vwrite,data_store(1,1), data_store(1,2)

%g %g

*cfclos

!************END of APDL code ***************

This works and I have verified this.

Claudio Pedrazzi

This is a transient solution with large deflection "on", and there is an equation based body acceleration acting on the entire beam (for simulating shaker table base excitation experiment).

The equation is acc = A0*sin(2*pi*f*time) [m/s^2]

where,

A0 - constant amplitude (for now) [m/s^2]

time - simulation time vector/array [s]

f - excitation/forcing frequency [Hz]

I am looking at running a sweep of 'f' automatically (say from 2- 50 Hz with steps of 0.1 Hz)and automatically write the tabular data to a text file, using ANSYS mechancial APDL GUI.

I have been able to completely realize the automation I had wished. I am tabulating this down so that any person in the future facing these issues can look into this. Also, this would bring a formal closure to this topic of discussion.

Thanks to all for helping me here.

TASK OUTLINE: Mechanical + piezo transient analysis to capture geometrically nonlinear system response and voltage output due to base excitation at high amplitudes (acceleration loading force). The acceleration value is a function entered in ANSYS GUI with the format : 0.1*9.8*sin(2*pi*10*time) [9.8*A*sin(2*pi*f*time)] I want the automation to :

(1) sweep across a range of frequencies, f

(2) to change the excitation amplitude, A

(3) output a table with time, displacement at center of structure, voltage as its 3 columns

1. I created the entire simulation required in ANSYS workbench 18.1. I also used the 'Piezo and MEMS v1' extension which is free to download from the ANSYS website, provided one has the university licensing, which I was lucky to have via our university.

2. From Mechanical GUI (Workbench) I clicked tools>write input file. This converted my workbench model into a *.dat file which is basically a series of text lines converting my GUI work into ANSYS APDL readable code. This is one of the 1st steps towards automation.

3. Open the *.dat input file to locate the line numbers where the base excitation and the excitation amplitude frequencies are written. Use MATLAB to change these values. Additionally, the name of the output table is also changed for every frequency sweep(check attached command snippet). These modified ANSYS input files are saved with appropriate names in *.dat format. MATLAB is also used to create a *.bat files for sequentially executing each of the different frequency simulations. Example: If I am sweeping through 20 frequencies for a single A value my *.bat files have 20 lines in it. TIP: In GUI enter a unique value of 'f' and 'A' such that its easily searchable. For example f = 9.6969 and A = 1.414469. Entering a generic value like f = 5 and A = 1 might give you multiple search hits in incorrect locations!

4. Once the *.bat file is generated by MATLAB, just double click that file and voila, APDL will run in the background sequentially!

P.S. A snapshot of my generated batch file is attached here. I wish to do a Youtube video as I have not really found one which addresses this issue of automating transient analysis via frequency sweeping. The blue color of the commands in the snapshot is due to the fact that the file is edited with notepad++.

I have also attached the command snippet created in solutions section of Workbench mechanical GUI to extract the displacement, voltage vs time data and write it to a text file.