I want to plot load vs Displacement. For this I'm using the "sum" command in abaqus to add the magnitude of all the reaction forces on the fixed nodes but the load value is very low, i.e.,less than 2kN but in actual experiment its about 20kN.
am I calculating the load correctly? is there any better method to calculate the load??
Hi Armin,
Another way of doing that is to create a reference point and couple the BC surface or edge to this reference point. Then apply the BC on the reference point instead. you can then read the reaction force and displacement of the reference point.
Interaction>create Constraint>coupling
By the way, I don't think it makes changes on your results. It is only another way of doing that.
Regards
Amir
Hi Armin,
Another way of doing that is to create a reference point and couple the BC surface or edge to this reference point. Then apply the BC on the reference point instead. you can then read the reaction force and displacement of the reference point.
Interaction>create Constraint>coupling
By the way, I don't think it makes changes on your results. It is only another way of doing that.
Regards
Amir
Hi Armin,
I also agree with Amir Hosein Sakhaei's method.
A quick way to check the Reaction forces in your model is to initially plot the contours of the deformed shape. The default is S (Von Mises stress), you can change it from “S” to “RF” in the Visualization module. “RF” meaning “Reaction Forces”. This gives the range of the reaction forces in the model and thus, you can find out the magnitude of the reaction forces (or total load). Hence, if this is still showing significantly lower results, then you may want to double check your model (i.e. boundary conditions, material properties, unit system, dimensions etc.).
However, if the magnitude of the reaction forces looks about right, then you can create a new “History Output”. From the drop down menu, change the “Domain” from “Whole Model” to “Set”. Then select a predefined set created for the fixed nodes (or area of interest). Afterwards, you can select the appropriate output variables (i.e. Reaction Forces, Displacements). Bear in mind that more output variables selected will result in increased computational time.
When the model is solved, you can find those selected output variables (i.e. Reaction Forces, Displacements) in Visualization > Create XY Data > ODB history output.
Hope that helps. Let me know if you have any other question(s).
Kind regards
Ade
Hi Armin
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.
Good luck
Milad
Hello Armin,
I am currently facing the same problem in my work. Trying to find out the reaction force against a displacement loading at rate 1.5 mm/min.
I too am getting a much lower value as compared to the experiment. If you were able to solve your problem, kindly let me know. Thanking you.
SM
Another very easy way to get forces in displacement-control is to plot the total work done (history variable ALLWK) and then differentiate that wrt the displacement.
create the set at which you need RF2, in abaqus viewer go to xy plot and plot and write the report in some txt file now go to excel and sum up all the rf corresponding to a node.
Hi Armin
I have the same problem. I tried several things, but still the same small values. If you have solved the problem, please share.
Thanks
Aziz
I have the same Problem. The raction force should be about 5 kN im comparison with Experiment but is about 50 N. Let me know if you have solved the problem.
You need to consider the width of your sample in the simulation. if you are using surface cohesive you also need to define width to the cohesive layer.
If you did not define a width for your model you can you can simply time the reaction force to the width.
if the problem is not width then you used the wrong unit system. I used the wrong unit system for this question.
- Badges
- Science topic