Force vs displ 1

[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.

 

[nomi9]

Hello FEA way,
Thank you for your answer. I found it extremely meaningful. I carried out a few simulations where I could extract force vs displacement curve but recently I have been facing the same problem. I requested RF3 on the loading edge nodes which have displacement BC. The another end is fixed (encastre).
Could you maybe share your insights on what I might be doing wrong? I could extract displacement curve but not RF3!
I appreciate any help you can provide.

 

[FEA way]

Is the prescribed displacement applied as U3 ? Did you choose the nodes with BC on this DOF to get RF3 ? If yes, can you share the file (.cae or .inp) ?

 

[nomi9]

Hi FEA,
I tried another approach now. I created a RP and did a kinematic coupling, coupling the aluminum surfaces on the fixed edge to that RP. In the BC, I applied a displacement BC to that RP. In history o/p I requested RF3 and U3 for that RP.
I hope it will work(fingers crossed). Do you think if it is a correct approach?
I am sorry, but I am not allowed to share the inp file as instructed.
Thanks for your cooperation

 

[FEA way]

Yes, you can use coupling and rigid body constraints. It’s commonly done this way and makes it easier to read the reaction forces as there’s just one node. Of course, it still needs BCs to provide RF.

 

[nomi9]

I did it with kinematic coupling and constrained all DOF's. What difference it would make if Rigid body constraint is used?

 

[FEA way]

Rigid body constraints make faces rigid. Kinematic couplings (equivalent to Nastran's RBE2) also impose rigidity but distributing couplings (equivalent to Nastran's RBE3) allow some flexibility.

 

[nomi9]

Hi,
Thank you for your answer. I could successfully extract the needed information from my simulation.
In the force vs displacement curve, my results are not comparable to the experimental curves. RF3 and U3 I extracted are for the RP which was kinematically coupled to aluminum tab's top surfaces. Could you suggest me how to get close to the experimental one?
Will changing poisons ratio of cfrp play a role?

 

[nomi9]

Rigid body constraints make faces rigid. Kinematic couplings (equivalent to Nastran's RBE2) also impose rigidity but distributing couplings (equivalent to Nastran's RBE3) allow some flexibility.

Hello FEA way,
Could you please let me know how I can make my Force vs Displ. curve similar to the experimental one?
I am using Kinematic coupling and I requested RF3 and U3 for the reference point used for kinematic coupling.

 

[FEA way]

So simulation gave you the black curve while the 3 colored ones are from experiments ? What are the differences ?

 

[nomi9]

Yes. Three colored ones are from experiments. I want to validate my model with an experiment. I am extracting RF and U on the Reference point which is used to kinematically couple the two outer surfaces of the aluminum on the loading edge. Between Aluminium and the CFRP specimen, there is a tie constraint.
I know I will not get 100% match but even the slopes are nowhere near.

Alu: C3D8R
CFRP: S4R

 

[SWComposites]

how and where exactly was the displacement measured in the tests?

some photos of the test setup and specimen would help (post them in line not as attachments).

and then show a picture of the FE model with boundary conditions and loads.

 

[FEA way]

Apparently, the numerical model is not stiff enough. Usually, it’s the opposite. But I would have to see the model to tell more. Some screenshots of the mesh and analysis features may help.