Someone explain to me some methods to get the Force-displacement curve from Abaqus for whole model .
Hello,
In the step module, specify the number of increments you want.
Then, in the visualization module, go to Create XY data -> odb field output -> in the variables tab specify the variable(s) you want to plot and in the element/node tab specify the elements or nodes in which you want the results. E.g.:
i)if you want the displacement at a specific node, select unique nodal and displacement in the variables tab, then in the element/node tab select the node the displacement of which you want.
ii)if you want the force at a specific node in a similar way select CF and unique nodal, then the node the force of which you want.
Then you can combine force and displacement data by
go to tool then create xy data then operate on xy data..then select combine
option.
Hope this will help you.
Hello,
In the step module, specify the number of increments you want.
Then, in the visualization module, go to Create XY data -> odb field output -> in the variables tab specify the variable(s) you want to plot and in the element/node tab specify the elements or nodes in which you want the results. E.g.:
i)if you want the displacement at a specific node, select unique nodal and displacement in the variables tab, then in the element/node tab select the node the displacement of which you want.
ii)if you want the force at a specific node in a similar way select CF and unique nodal, then the node the force of which you want.
Then you can combine force and displacement data by
go to tool then create xy data then operate on xy data..then select combine
option.
Hope this will help you.
Ahmed!
Just watch this tutorial and you should be able to get it..good luck
https://www.youtube.com/watch?v=vA1UUmea06E
Hello Ahmed,
I usually like to automate the post processing and using the GUI is time consuming. Therefore, I usually write the nodal outputs to the .dat file.
For instance, if you have a reference node kinematically coupled to a surface that's being compressed in the Z direction, you are interested in U3 and RF3 of this node:
*NODE PRINT, NSET=REF_NODE, FREQUENCY=1, SUMMARY=NO
U3,
RF3
Then, simply use a script (python or matlab) to parse the .dat file, extract U3 and
RF3 and plot.
Regards,
Ghislain
Update:
I realised that I never replied to the example request. Here it is: an input file with this feature, the resulting .dat file, the python script for reading the .dat file, and the related publication. Please realise that this is just an example and that you will not be able to run the input file withouth the UMAT for interpreting the material cards.
Article Head-Neck Osteoplasty has Minor Effect on the Strength of an...
Hello,
I applied a compression displacement to a one element case and I'm certain of my model parameters. However, in the visualization module when I plot the stress vs strain curve or any curve, I get only two data points, so my curve is always linear. I'm using a plasticity model so this doesn't make sense. Please advise on the two data-point issue. Thanks!
Hi Dr Maquer
I run my parametric study in abaqus through matlab, now i want to save the each iteration under different job name and find the reaction in each job.
Please can you help me in this matter.
Thank you
Regards
The matlab tool 'Abaqus2Matlab' can used to read and save force displacement response of multiple simulations in a parametric study or optimisation in abaqus
Check this youtube tutorial.
https://www.youtube.com/watch?v=VpQUtwzz0Q0
I use the "combine" operator but it says "X value is not monotonic and interpolation is not defined". The "interpolation" operator can be applied successfully for displacement curve but I get error applying that for Stress curve. It again says "X value is not monotonic". Does anyone know why?
* Update: This error occurs when the number of arrays in load is not the same as displacement.
- Badges
- Science topic