Learning Forum

[safiana]

Hi everyone,

I am having a 3D model in Ansys APDL solved by transient analysis. I would like to store the summation of nodal forces for a group of nodes for each load step.

Let's say I already have assigned the name "gp" to that group of nodes. Also, I have solved the model with 400 load steps. How can I export nodal forces in Z direction only into an excel file? Can anyone give me a sample code for obtaining Fz for a group of nodes and exporting into an excel file where the first column is the load step (time) and the second column is Fz?

Thank you,

Ali

[Govindan Nagappan]

Create an array to store the results using *DIM command
Then use a *DO loop to loop through each step and save the result to the array
Example:
cmsel,s,gp *do,j,1,400
set,j !select result set
fsum
*get,my_fsum,fsum,,ite,fz !get fz and store it to variable my_fsum
!save my_fsum to the array
!save j(load step number) to the array
*enddo
Use *cfopen to opena text file. Then use *vwrite to write the array to a text file. Use *cfclose to close the text file

[Erik Kostson]

Hi as said that is the basic flow - I had something lying around and took very little change , so wanted to share in case anyone else would need this (have in mind there should not be any empty rows especially between *vwrite and (F20.10,F20.10)). Also the text file is placed in the solver files directory is.


! Allocate arrays
cmsel,s,gp,NODE
*GET,my_NNUM,NODE,,COUNT !GET NUMBER OF SELECTED NODES IN MODEL
*GET,my_numtimes, ACTIVE, 0,SOLU,NCMLS

*dim,fsP,array,my_numtimes,2

! Extract force sum
*do,ii,1,my_numtimes,1
set,ii,last
*get,my_time,time
fsum
*get,my_fsum,fsum,,item,fz
fsP(ii,1) = my_time
fsP(ii,2) = my_fsum
*enddo

*CFOPEN,timefsumz,txt
*VWRITE,fsP(1,1),fsP(1,2)
(F20.10,F20.10)
*CFCLOS

[safiana]

Thank you very much @gnagapp and @ekostson. I really appreciate your help.
Best
Ali