"Workbench" Contact tool results plotting vs length

  • 1.9K Views
  • Last Post 03 January 2019
  • Topic Is Solved
Mirghani posted this 02 January 2019

Hello Ansys Community

In ANSYS Workbench how can I plot the Contact tool results (frictional stress, sliding distance...etc) Vs "length" (500mm for example) in the "x-axis" instead of default "by time" option???. the "Path" method can not be used with this type of results. I tried all the possible solution using path, named selection, user defined results ...etc. However, I found the easiest way is:Go to Contact tool-> frictional stress ->Then right click the mouse and select Export -> Export text file -> Use Excel software to draw the frictional stress with node locations not the time using probes. Using probes is a time consuming process because I need to select each node and read the corresponding contact tool value. (any other easier and more direct way??)  

Any help or suggestions will be highly appreciated.

 

 

    

 

 

 

Order By: Standard | Newest | Votes
SandeepMedikonda posted this 02 January 2019

Hi Mirghani,

You might have to do this using an APDL command snippet.

A colleague of mine put this together for a couple of simple blocks touching each other.

The key here is to define a Path and define coordinate systems at the start and end of that path.

Then using the following APDL script:

! Create a coordinate system at the start and end of your path
csys_start=12
csys_end=13

/triad,off
/view,1,1,1,1
/show,png

set,last

csys,csys_start
node1=node(0,0,0)

csys,csys_end
node2=node(0,0,0)

csys,0

esel,s,ename,,174
nsle

PATH,path1,2,30,20, 
PPATH,1,node1
PPATH,2,node2

PDEF,p_pres,CONT,PRES

/PBC,PATH,,1 
/REPLOT 

PLPATH, p_pres

plnsol,cont,pres

you should be able to generate the plot you are looking for:

Regards,
Sandeep
Guidelines on the Student Community

  • Liked by
  • Mirghani
  • jackhero
Mirghani posted this 03 January 2019

Hi Sandeep

Thank you very much for your answer (thank your colleague for me as well), I inserted the command and its working fine. however, do you have any idea how can I get the path data itself. I mean in a table kind of thing or a text file. in addition, this command gives the results only for 1 set (last Set), how can I retrieve the results for multiple sets with its data on the same time.

I changed the contact pressure PRES to SFRIC & SLIDE to get the frictional stress and sliding distance respectively.

PS: I am a beginner when it comes to APDL commands but am learning.

Thank you.   

 

jpasquerell posted this 03 January 2019

Mirghani:

 

POST1 only holds one set of results at a time so a path plot will always only show one set of results.  See the SET command to read other sets of results. There is a PAGET command that can be used to save the path data into an array.  You can export array values to a text file using the *VWRITE command.  There is also a *VPLOT command that can plot up to 8 columns of data in a table array as a line plot with the index column being the distance.  You would need to copy the data from the arrays to a table using the *VFUN,,copy command.

  • Liked by
  • Mirghani
jackhero posted this 03 January 2019

Although the question has been marked as solved, one query I would like to ask here. Within the contact tools we can also use the sliding distance to plot it on x-axis (against frictional stress, load etc on y-axis). How come the sliding distance would be different from the length (here is say 500mm) which we are plotting here from this question?

If we apply displacement controlled loading then I think the maximum displacement or sliding distance will be almost similar. If yes, then why do we need length? Bit confused. It would be easier if one may post the x-axis’s sliding and length comparison for the same model

Mirghani posted this 03 January 2019

Hi jpasquerell

Thank you for your answer. I will try to go through these commands and apply them.

Hi Jack

By length, I mean the overall contact length. The sliding distance is different, simply the sliding distance is the slip of the contact elements as they are being debonded/separated from the target elements (C4 in CZM input). Generally the slip can by calculated experimentally by the means of strain gauges (very small displacement a fraction of mm). Its also different than the total displacement applied because the displacement controlled load applied includes the deformation/ elongation of the bonded material plus it's slip when its being deatached from the other material.

  • Liked by
  • jackhero
Close