Learning Forum

[Ahmed_Safty]

Hi i am s student and i am doing my final year project on a screw connection with simplified screw geometry. I have been able to simulate this test but my equivalent stress doesn't seem logical. What i think that depends on the steel plate material property but what i am using is grade 550 steel and the yield strength and ultimate strength should be 550 MPa. how can fix it or improve it. And i don't know how to make this model fail in which there is going to be damage in the steel plate and screw.

[ciema]

Hello Ahmed_Safty, the first question is what kind of analysis it is: static structural? What type of material model do you use? Is it linear elastic behavior?

[Ahmed_Safty]

Hi Ciema, It is static structural analysis and the materials stiffness behavior is Flexible. The materials used that I require to input are:
Zinc Aluminum Alloy with G550 Grade for steel plates
AISI C 1022 Steel for the screw
and I use non-linear option to achieve my results.

[ciema]

You have to go to Project Schematic and set properties in Engineering Data cell. If this is linear analysis you will need only density, youngs modulus and poisson's ratio to determine each material. You can try to add also properties for checking Safety Factors - in default material like Structural Steel there are four materials data included: tensile yield strength, compressive yield strength, tensile ultimate strength, and compressive ultimate strength.
Then you should go to To Mechanical and Add Insert - Stress Tool - Max equivalent Stress. And this result can help you to analyze your system.
Different aspect is that you should check all contacts status via Contact Tool and all boundary conditions (check their influence on your model). If you want to analyze Life of your parts, you have to input Fatigue data and use Fatigue Tool.

[Ahmed_Safty]

Hi Ciema, If i may can show u my material properties and setting that i have input it would be easy to pinpoint the problems that i don't know. I have tried applying and tweaking with the settings but still the same result appears to me in the equivalent stress solution.
Material Properties:
Contact between screw and plates are frictional of 1 as the screw is simplified and contact friction is 0.2 between steel plates:
My analysis settings (Using fixed and nodal displacement BCs):
Thank you

[peteroznewman]

In Engineering Data, expand the Plasticity category. Drag the Bilinear Kinematic Hardening material model and drop it on your 550 steel material. This model requires two inputs: Yield Strength and Tangent Modulus. Make sure the units are set to MPa and type in 550 on the Yield Strength line, and type 0 for the Tangent Modulus. This is called an elastic perfectly plastic material model.
I recommend you change the mesh on the plates. Right click on Mesh in the outline in Mechanical and Show Sweepable Bodies. The two plates should highlight. If so, add a Mesh Method and set that to Sweep. Set the number of divisions to 4. That should put 4 elements through the thickness of the steel plates.
When plasticity is in the model it is best to use a displacement BC for the load, which you are using, and not a Force which some people use.
I see you have 20 steps, which is helpful for plasticity to converge, but you may find you need more substeps in some of the later steps to help convergence.

[Ahmed_Safty]

I have used the Bilinear Kinematic Hardening , edited the mesh and Analysis settings, so it gave me quite desirable results but still not the results that is expected:

as i have seen other articles and tests looks like this for ES Mises:

[peteroznewman]

See in the example you are trying to recreate, they have 2 elements through the thickness. I repeat what I said above, I recommend you change the mesh on the plates. Right click on Mesh in the outline in Mechanical and Show Sweepable Bodies. The two plates should highlight. If so, add a Mesh Method and set that to Sweep. Set the number of divisions to 4. That should put 4 elements through the thickness of the steel plates.
Also, change the Contact between the head and the top plate to Frictional, and also the contact between the shaft and the hole in the top to Frictional.

[Ahmed_Safty]

I have changed the mesh through Show Sweepable Bodies, but it only chooses the bottom plate to be sweeb for the mesh method. I have tried to choose the top and bottom to be sweepable but Ansys crashes.
I also have a friction between the head and the top plate to be frictional of factor 1 and the shaft contact between the two holes of the plates to be frictional of factor 1.


Thanks

[peteroznewman]

For the top plate, try Multizone method instead of Sweep.
Or go into Geometry and make sure that the geometry is sweepable.

[Ahmed_Safty]

It half-succeeded after i followed your instructions, but i have another problem. I put the nodal displacement 20mm in the +ve x-axis direction and it reaches to 2.79mm and then it fails to reach the 20mm. I have done this experiment in the lab and the specimen handled until 19mm. what could i do to make it similar to my lab experiment?