Force vs displ

[nomi9]

Hello Users,
I am simulating a tensile test of CFRP shell coupon in Abaqus.
Aluminums tabs are attached to the CFRP shell sample on both the edges from top and bottom and they are modeled with solid elements. Two Aluminium tabs on the fixed edge are Encastred with all DOF's=0 and the other two Aluminums tabs on the loading end has one DOF not equal to zero i.e. U3 as I am pulling from this end. For load, I have defined surface traction and have selected the two Aluminums top surfaces on the loading edge. I want to plot Force vs Displ. in order to validate the model with the experiment one.
I created a set consisting of two elements which are on the loading edge and requested RF3 and U3 in the history output request. The simulation ran successfully with the U magnitude to be around 2.4 mm, but there is no data to be seen in the history output in the visualization module in order to plot, it is completely blank!!
Can you please suggest me what wrong I have done here? Also can you suggest other simpler option to extract the Force vs Displ. curve (on a Global level of model)?

Best Wishes

 

[SWComposites]

what is a "shell" coupon?
if you are trying to correlate FEM displacements to test machine head travel displacements,. well, it won't work well as you are not modelling the test machine and grip compliance.
in your test data, you should measure displacement or strain in the specimen gage section between the tabs, and then compare that to a FEM.
you should then extract element strain vs load in the gage section from the FEM.

 

[nomi9]

what is a "shell" coupon?
if you are trying to correlate FEM displacements to test machine head travel displacements,. well, it won't work well as you are not modelling the test machine and grip compliance.
in your test data, you should measure displacement or strain in the specimen gage section between the tabs, and then compare that to a FEM.
you should then extract element strain vs load in the gage section from the FEM.

Hi,
Thank you for your answer. By coupon, I mean CFRP with a size of 250*25 mm. To make it less computationally effective, I used shell as an element type for CFRP and wrote a shell coupon. I understand I will have to measure displacement in the gauge section, i.e., in the middle part of the CFRP. For that, should I have to use History or field output request?

 

[FEA way]

Even if you don’t request history output, you can create XY data from field output. Either way, make sure that you sum the reaction forces from all fixed nodes. Of course, it’s easier to apply BCs via coupling or rigid body constraints so that you only have a single node for output.

 

[nomi9]

Hi,
Taking reaction forces summation of the nodes on the loading edge would be a better choice right? I mean they are the one who are getting pulled? I selected the nodes on the top surfaces of the aluminium tabs on the loading edge and will take summation of those nodes.
For plotting the displacement, I selected the nodes in the mid-section of the CFRP.
Both requested from History o/p.
Best regards

 

[FEA way]

Taking reaction forces summation of the nodes on the loading edge would be a better choice right? I mean they are the one who are getting pulled?

Reaction forces (RF) are written only for nodes having boundary conditions applied in given directions (DOFs). So it will work if you pull one side with a prescribed displacement but not if it’s loaded with force.