stress and strain input 1

[balu25]

If i have the value of the stress and strain of a material, how can i define a material with this characteristics in ANSYS?
Thanks

 

[cbrn]

Hi,
look for "tabular data", "material properties" ("TB" family of commands - 8.4 of Structural Guide)

Regards

 

[balu25]

thanks, but i have 100 values for stress and strain just for one material type...so i need to make a fail, from whome i can read this and input it.
and tb command just MKIN and BKIN Specifications seems to fit for me with their Stress-strain options.
What should be the Lab so i can make a stress-strain input?

 

[cbrn]

Hi,
1- *DIM-ension a TABLE (see help) to have 100 rows and 2 columns, format your data points file as needed by ANSYS (see help) and then read-in the data from file into the table. Let's say your table is named "DATA_PT", and that the first column contains the total strain whether the second column contains the stress.
2- Use non-linear kinematic hardening material model, as follows (indicatively):
TB,KINH
TBTEMP,...
*DO,i,1,100,1
TBPT,DEFI,DATA_PT(i,1),DATA_PT(i,2)
*ENDDO

You can write these commands in a text file and then "Read Input From..." this file. This APDL file may also include the table declaration (*DIM,...) and the data reading from file (*TREAD,...).

Regards

 

[balu25]

Thanks a lot for the help!!!

 

[Struct71]

To my knowledge a tb,kinh table only
accepts 19 points or so. But realistically this should be more than enough...