General Mechanical

General Mechanical

Why does the structure not affect the results in a tensile test?

    • ISSAMAZERTY
      Subscriber

      I did a tensile test in a static structural :

      I defined the substance (young modulus, Poisson's ratio, multilinear stress-strain curve).

      For the structure, I used the lattice structure.

      The problem with the results, when extracting the curve stress-strain keeps the same values of the material you entered earlier. In the sense that it does not take into account the impact of the structure.

    • peteroznewman
      Subscriber
      You input a material Stress-Strain curve into a model that has the geometry in a lattice structure and when you plot material Stress-Strain results, you get back the input, is that what you are saying?
      Say your Lattice Structure is 80% void and 20% material, you might expect that the Effective Stress vs Strain curve would be reduced to about 20% of the material stress value.
      To measure this, you can't plot the material Stress value, you have to request the Tension Force and divide by the Area of the cross section (counting both the void and the material) to get the Effective Stress.
    • ISSAMAZERTY
      Subscriber
      Thank you so much for your answer.
      I got the right results.

    • ISSAMAZERTY
      Subscriber
      It's got a high-stress value.
      I use symmetry in the three directions.
      When extracting the value of the force, multiply it by 4 to get the true value. Then divide it by the area of the cross-section.
      Is this method correct?
      With that, I got a high-stress value.


    • ISSAMAZERTY
      Subscriber

      Also in the experimental data file, when I extract the cross-sectional area, I find that it changes with the change in the applied force.
      Will it be variable when I need to calculate stress?
    • peteroznewman
      Subscriber
      The definition of Engineering Stress is Force/Initial Cross-Sectional Area. In a tensile test of a solid material, the cross-sectional area changes with applied force.
      There is another definition for True Stress, which accounts for the change in cross-sectional area so the True Stress is higher than the Engineering Stress after some plastic strain has built up.
      You say you got a high-value stress, compared to what?
      How exactly did you calculate the cross-sectional area?
      For what reason are you calculating stress?
      I suggest you use the Force-Displacement data to characterize the structure. That is both easy to measure and meaningful.

    • ISSAMAZERTY
      Subscriber
      I have data to test the tensile test that was done.
      I apply displacement to the structure and extract the value of the force as you told me, after that, I try to convert it into stress-strain values.
      When I compare the experimental values with the Ansys values, I find that the simulation values are very large.
      I want to know if the method I used is correct or I have another problem.
    • ISSAMAZERTY
      Subscriber
      I want to compare the stress-strain curve, between experimental and Ansys simulation
    • peteroznewman
      Subscriber
      You mean you have experimental data to compare with the simulation? Good. Get the Force vs Displacement experimental data and overlay the simulation Force data. Show us that graph.
      Don't try to convert your simulation data to stress-strain data.
      Do you know how the experimental data was converted from Force to Stress? Find out the details, or just plot the force.
    • ISSAMAZERTY
      Subscriber
      I don't know how the experimental data was converted.
      I only have stress-strain and displacement values, so I need this conversion.
    • ISSAMAZERTY
      Subscriber
      When using symmetry in three directions, must the force be multiplied by 4 to find the correct value of the force?
    • peteroznewman
      Subscriber
      Yes, multiply the force by 4 to get the total from a 1/4 symmetry model.
      If you don't know how the experimentalists converted Force to Stress then you are completely in the dark.
      You may as well take the Stress value they provided at a known Strain/Displacement and compute the value of area that turns your force into their stress, then you will get exactly the stress they show at least at that one point.
    • ISSAMAZERTY
      Subscriber
      Thank you so much for your answers.
      I have one question left.

      Is the displacement I should apply to the structure in the test is the same as the stroke value?
    • peteroznewman
      Subscriber
      Yes, stroke equals displacement.
    • ISSAMAZERTY
      Subscriber
      Thank you.

      I did everything we mentioned, but I'm still getting large results compared to the experience.
      I think the problem is elsewhere.
    • ISSAMAZERTY
      Subscriber
      Hello Mr. Peter
      Thank you for your useful answers.

      I got good results. I had a problem with the mesh.
      I have a question about comparing the experiment with simulations, when extracting the graph the stress increases with increasing the strain, it doesn't go down like the experiment.
      Is there a property in the material that I must add to show the results, such as an experiment, or any other solution?

      Thank you again.
    • peteroznewman
      Subscriber
      Engineering Stress is Force/Area.
      An experiment records force and divides by the area. What area did they use?
      You should plot the reaction force from your simulation and compare it with the force measured in the experiment. Then you don't care about area.
    • ISSAMAZERTY
      Subscriber
      In the experiment when a large displacement is applied the force values begin to decrease until they are absent at refraction, the simulation reverses the larger the displacement, the higher the force value

      Is there a way to show reaction force like an experiment?
    • ISSAMAZERTY
      Subscriber
      I would like to say how do I do tensile test to see necking ? (Tensile strength simulation model)
    • peteroznewman
      Subscriber
      If you have plasticity in the material model, you can see necking occur in the simulation.
      https://forum.ansys.com/discussion/23145/why-doesnt-the-load-passes-through-max-shear-stress-direction-for-ductile-materials
    • ISSAMAZERTY
      Subscriber
      I am using bilinear isotropic hardening, but no necking occurs in the simulation.

    • ISSAMAZERTY
      Subscriber
      Sorry, can you explain to me more how to define plasticity in the material model?
    • ISSAMAZERTY
      Subscriber
      For this curve.

      Thanks.

    • peteroznewman
      Subscriber
      You have plasticity in the model. Bilinear Isotropic Hardening is one type of plasticity.
      Try using 0 for the Tangent Modulus.
      Another issue with your model is the number of elements through the thickness of the wall. Please show a close-up image of the mesh that shows how many elements are across the thickness.
    • ISSAMAZERTY
      Subscriber
      Is there a problem with the mesh?

    • peteroznewman
      Subscriber
      To accurately simulate plasticity, you want at least 4 elements (and preferably more) through the thickness. This mesh has 1 element through the thickness.
      Using tet elements will create a very large model because you will have an element size of t/4 to get four elements through the thickness.
      Take some time to slice the geometry up into sweepable solids so that you can use a Mesh Method of Sweep that allows you to specify 4 elements in the sweep direction while using a larger element size in the other directions.
    • ISSAMAZERTY
      Subscriber
      I minified element size 10 times, but the force curve hasn't changed.
      But curve stress has changed.
      This is the force curve.

    • ISSAMAZERTY
      Subscriber
      I have used 0 for the Tangent Modulus.
    • peteroznewman
      Subscriber
      Please overlay the experimental force displacement curve with the simulation force displacement curve.
    • ISSAMAZERTY
      Subscriber
      force displacement curve when using 0 for the Tangent Modulus.


    • peteroznewman
      Subscriber
      The simulation model is too stiff initially. You can either make the geometry slightly thinner, or reduce the Young's modulus. I would do the second.
      Divide the initial slope of the experimental Force Displacement by the initial slope of the simulation Force Displacement curve to get a reduction factor. Multiply that factor by the Young's modulus to get a new Young's Modulus to rerun the simulation.
    • ISSAMAZERTY
      Subscriber
      It looks good now, it has improved.
      The only problem left is the necking region.
      Thank you so much again for your helpful answers.

    • ISSAMAZERTY
      Subscriber
      I tried a large displacement application, and got these results.

      The necking region has appeared, but it is far away.
    • ISSAMAZERTY
      Subscriber
      Can I reduce Young's modulus?
      Isn't that a change in the material with which I'm doing the experiment?
    • peteroznewman
      Subscriber
      I expect your structure is 3D printed. Where did the Young's modulus value come from?
      Print solid tensile test coupons in different directions to obtain force-displacement data from multiple samples, and convert them into Stress-Strain data. You need to use an Instron type tensile testing machine with a proper extensometer to measure displacement in a 40 mm gauge length at the center. Show the data, labeled by print direction. You have to print with these coupons flat on the bed, with a 4 mm build height as well as vertical with a 170 mm build height and some off at other angles.
    • ISSAMAZERTY
      Subscriber
      Yes, what you said is correct, the experiment was carried out with the same machine with the following measurements :
      I only have the stroke value of the gauge.
      I think the problem is that I do not have the complete displacement for the structure (i.e. 70 mm).
    • ISSAMAZERTY
      Subscriber
      Do you have any idea how to solve this problem, or a way to find out the complete displacement of the structure?
      Thanks
    • ISSAMAZERTY
      Subscriber
      I hope I explained the problem well, sir.
    • peteroznewman
      Subscriber
      Are you saying that solid, flat, tensile test coupons were printed and tested in the same machine that is pulling the complex 3D shape with curves and holes?
      What do you mean you only have the stroke value of the gauge? Is that for the tensile test coupon? Was an extensometer used to measure the gauge length elongation? What was the gauge length that the extensometer was place along?
      Please reply with a full description. Add some images or figures to make it clear what was measured.
    • ISSAMAZERTY
      Subscriber

      Instron type tensile testing machine was used.
      The extensometer is placed in the place you specified to measure the stroke value of the gauge.
      I am now available on Excel with:
      the stroke value of the gauge.
      applied force.
    • ISSAMAZERTY
      Subscriber
      The extensometer is placed to select 15 mm in the middle.
      Thanks.
    • ISSAMAZERTY
      Subscriber
      Sorry, the stroke value is only set in 15mm (in place of the extensometer)
    • peteroznewman
      Subscriber
      So a tensile coupon was printed on the same 3D printer that printed the 3D structure. Good. Was it printed in at least two build directions? Flat on the platen with a build thickness of 4 mm and built vertically with a build thickness of 70 mm. The properties of the material may change with build direction.
      If you have the force and extension values on the 15 mm gauge length, you can convert that to stress and strain values. If you want to attach an Excel spreadsheet, you have to put it in a zip archive first. I use the 7z format.
    • ISSAMAZERTY
      Subscriber
      Yes, I have force and extension values on the 15 mm gauge length.
      I also have stress and strain value.
      like this :

      The question is how can I use it correctly in ANSYS simulations, to get good results??
    • peteroznewman
      Subscriber
      Create a Multilinear Plasticity material model.
    • ISSAMAZERTY
      Subscriber
      Hello Mr. Peter.
      I used the method you mentioned, but I'm still facing the same problem.
      (I used the material's stress-strain curve).
      Thanks.
    • peteroznewman
      Subscriber
      Did you implement the conversion from Engineering Stress and Strain to True Stress and Strain correctly? You can attach the spreadsheet by putting it in a 7zip archive.
      Conversion of Engineering Stress and Strain to True Stress and Strain can only be done up to the point when necking begins. You can't use the experimental data from the tensile test after necking begins because the equations used in the conversion have an assumption that the plasticity is uniform over the entire gauge length, width and thickness (constant volume assumption). That is violated as soon as necking begins. So mark in the spreadsheet the rows where the necking was present in the data.
      The simulation is not going to exactly match the experimental data. How close are the curves with the latest revision to the model with the new material model?
    • ISSAMAZERTY
      Subscriber
      I did not understand what is required is the excel file for the material or for the experiment.
      I'm importing the material's curve stress-strain file into ANSYS (the material's values are trues).

      I need more clarification.

      Thanks.
    • peteroznewman
      Subscriber
      In one of your posts, you inserted this image. Is this material data from a flat tensile test coupon or from the 3D structure?
      You use the stress-strain data from the material test of the flat tensile test coupon. Data from that test is in terms of Engineering Stress and Engineering Strain. It must be converted into True Stress and True Strain to use in a Multilinear Kinematic Hardening Plasticity material model. I want to see a plot of the Engineering Stress and Engineering Strain.
    • ISSAMAZERTY
      Subscriber
      As for the picture (Excel) I sent earlier, it is for the 3D structure.
      This is the Engineering Stress and Engineering Strain curve (from the material test of the flat tensile test coupon):

      Sorry I didn't explain things well.

      Thanks.
    • peteroznewman
      Subscriber
      You should convert the data in the material spreadsheet to True Stress True Strain, then create a Multilinear Kinematic Hardening plasticity material model.
    • ISSAMAZERTY
      Subscriber
      I converted it and created a Multilinear Kinematic Hardening plasticity material model., but I didn't get as good results as I mentioned earlier.
      These are the new results I got :

    • peteroznewman
      Subscriber
      You have good agreement between the experimental force-displacement and the simulation force-displacement.
      Conversion to Stress is problematic with a complex 3D structure full of holes. What area do you use?
      Let's stick to force-displacement.
    • ISSAMAZERTY
      Subscriber
      This is a force-displacement curve.

    • peteroznewman
      Subscriber
      In the last post you show an experimental force of 800 N.
      Previously, you showed an experimental force around 1500 N.
      Was that a different experiment? I don't think I can help you anymore.
    • JaniraBei
      Subscriber
      Good evening,
      I readanswer about Tension Force and since I'm facing the same problem with a lattice structure I'd like to know how I can request the Tension Force to the solver.
      Thanks for helping!

    • peteroznewman
      Subscriber
      Insert into the Solution branch in Workbench a Probe of the Reaction Force of the Displacement that is causing the sample to be compressed or stretched.
    • JaniraBei
      Subscriber
      Thank you so much!
Viewing 57 reply threads
  • You must be logged in to reply to this topic.