11 Replies Latest reply on Jan 15, 2014 12:17 PM by Jared Conway

    Stess / Strain curves; engineering vs true values

    Keith Frankie
    Keith Frankie Jan 13, 2014 11:49 AM

      This study is interesting.  I've been working through some exercises to gain a better understanding of simulation and materials.  Please point out any mistakes I make!

       

      Imagine you perform a standard uniaxial tension test on a sample of 'alloy steel' in a materials lab.  Your machine grabs both ends of the sample and pulls at a constant elongation rate.  Your material is magical though - it follows the SW linear material model and hence has a fixed modulus of elasticity and never breaks.  You would expect the stress/strain curve to be a straight line, right?

       

      So lets do it in SW.  My bar is 1m square x 10m long.  I use a nonlinear static study.  I set the material as 'alloy steel' and mesh it as a beam.  To keep computation time down a mesh control gives us 5 elements.  One end is fixed. A prescribed displacement fixture pulls the other end 10m over the length of the study.  (Tip: create a second solid body so that you can add this fixture type to the beam.  Then exclude this second body from the analysis - you can't add this type of fixture if SW thinks you only have beams).

       

      When your results come up add a time history plot showing the axial beam stress.  Here it is:

       

      Stress Strain.png

      That's not linear!  Note that by running the study from 0 to 100 seconds the x scale can be read as 'Engineering Strain [%]'

       

      What's going on here?  Here's my explination: Young's Modulus (or, as it turns out bilinear or multi linear) material data is interpreted by SW as using true strain.

       

      I saved this data ('file' -> 'save as' in the response graph) and converted the 'percentage engineering strain' to 'engineering strain' and then to true strain.  Re-graphing gives this:

       

      True Conversion.png

       

      Very linear!

       

      The SW help file ( http://help.solidworks.com/2014/English/SolidWorks/cworks/r_input_stress_strain_curve.htm ) says that for most studies engineering strain is used.  It's only for large strain studies that true strain needs to be input.  It seems to me that this chart is incorrect - really SW just always uses true strain.  Because true and engineering strain are so close for small strain values it doesn't really matter.  I also originally interpreted this chart as indicating true strain was needed only when using the 'large strain option' in the study properties, but again I think that is wrong.  (The SW help file is very sparten about the large strain option, but further reading indicates that when the volume of the deformed body changes significantly, as with large strain, this option needs to be used for accurate results.  This is the next step beyond large deformations, where although the shape of the body changes significantly, the volume doesn't necessarily change much.)

      • 2749 Views
      • Tags:
        • Re: Stess / Strain curves; engineering vs true values
          Shaun Densberger
          Shaun Densberger Jan 13, 2014 2:36 PM (in response to Keith Frankie)

          Keith Frankie wrote:

           

          Your material is magical though - it follows the SW linear material model and hence has a fixed modulus of elasticity and never breaks.  You would expect the stress/strain curve to be a straight line, right?

           

          I believe this would depend on how much strain you induce in the specimen; if the strain is larger than 5%, I would expect a non-linear curve. Even though your Young's Modulus is constant (linear material), large strains and the Poisson's Effect should result in a change of the cross-sectional area of the specimen (sometimes called necking). For a uniaxial load, the stress is F/A, and since A is decreasing as your strain increase, so to does your stress. If your Young's Modulus is constant, you should get a curve that has an increasing slope. If I understood you correctly, you ended up inducing 100% strain in your model, placing you well above the 5% rule-of-thumb.

           

           

          Keith Frankie wrote:

           

          I use a nonlinear static study.  I set the material as 'alloy steel' and mesh it as a beam.  To keep computation time down a mesh control gives us 5 elements. 

           

          Hmmm, I'm not sure what SW is doing for non-linear beam elements, so maybe this is part of the problem. Have you tried with a 3D model?

           

           

          Keith Frankie wrote:

           

          What's going on here?  Here's my explination: Young's Modulus (or, as it turns out bilinear or multi linear) material data is interpreted by SW as using true strain.

           

          Wait, did you provide SW with a non-linear material model? If the Young's Modulus is allowed to change, then you could get the stress-strain curve that you go if your Young's Modulus decreases with increasing strain.

           

           

          Keith Frankie wrote:

           

          The SW help file ( http://help.solidworks.com/2014/English/SolidWorks/cworks/r_input_stress_strain_curve.htm ) says that for most studies engineering strain is used.  It's only for large strain studies that true strain needs to be input.  It seems to me that this chart is incorrect - really SW just always uses true strain.  Because true and engineering strain are so close for small strain values it doesn't really matter.  I also originally interpreted this chart as indicating true strain was needed only when using the 'large strain option' in the study properties, but again I think that is wrong.  (The SW help file is very sparten about the large strain option, but further reading indicates that when the volume of the deformed body changes significantly, as with large strain, this option needs to be used for accurate results.  This is the next step beyond large deformations, where although the shape of the body changes significantly, the volume doesn't necessarily change much.)

           

          I think the chart is telling you what type of strain data you need to supply (as opposed to what type of strain formula is being used). It is correct that true strain is only needed if you have the large strain option, because at large strains you will have a significant change in the cross-sectional area.

          • Re: Stess / Strain curves; engineering vs true values
            Roland Schwarz
            Roland Schwarz Jan 13, 2014 2:44 PM (in response to Keith Frankie)

            Keith Frankie wrote:

             

            To keep computation time down a mesh control gives us 5 elements.

            If getting things done fast is more important than getting things right, then, by all means, do this.  Otherwise, refine until convergence.

            • Re: Stess / Strain curves; engineering vs true values
              Keith Frankie
              Keith Frankie Jan 14, 2014 5:52 PM (in response to Keith Frankie)

              Thanks for taking the time to look at this discussion.

               

              I've done several experiments to get to the bottom of this.  Unfortunatly I'm now more confused.  For a summary see the end of this post.


              would be interesting to know what the problem statement is here from the OP.I

               

               

              The purpose of these files and experiemnts was to solidfy my understanding of how Simulation handles material data.  I have another simulation I'm working on where I need this information.  Everythign here is an attempt to simplify my experiments so I don't get confused by extraneous information or options.

               

              If I understood you correctly, you ended up inducing 100% strain in your model

               

              Right - my original experiment takes a 10m stample and strestches it 10m, resulting in 100% strain.

               

              Lets address some other written and unwritten concerns.  See the attached 'Extension Test - Beam.sldprt'  Studies are named consecutively by letter.  It doesn't take long to run all studies.

               

              'Alpha' is the base example.  A beam when stretched 10% has a response graph (stress vs time or engineering strain) that looks linear to the eye, as I would expect.  Done with a nonlinear dynamic study.

               

              'Beta' is 'Alpha' same except with the 'Plasticity - von Mises' material model (direct fron SW).  Looks good.

               

              'Charlie' is 'Alpha' with 100% strain.  This is the baseline! (Almost the same as the original file in this forum thread - see 'India')

               

              'Delta' is done in nonlinear dynamics with a much longer time scale (1000s) so motion doesn't play a role.  Results are no different than 'Charlie' indicating my choice of time (100s total run) isn't the issue.

               

              'Echo' is 'Charlie' except with a custom material with a Poisson's ratio of 0.  Results are identical.  Rerunning with 0.45 also has the same results. I don't think SW considers transverse material movement for beams (even though the data is required).

               

              'Foxtrot' is 'Bravo' with the typical large strain (100%).  Using linear interpolation on the SW Alloy Steel SS material the stress at strain =1 would be 966MPa, but it is reported as 930 at strain = 1 (time=100s).  As with the linear material I believe this is because all materials are input and output using true strain.

               

              'Golf' is 'Charlie' with the large strain option checked.  The reults are again identical.  Perhaps the large strain option doesn't affect beams.  Dunno.  Again according to the help file it's this option that causes SW to switch treat any Stress/Strain curve as using logrithmic strain. http://help.solidworks.com/2014/English/SolidWorks/cworks/r_input_stress_strain_curve.htm

               

              'Hotel' is 'Charlie' with a bi-linear material model (tangent modulus or ETAN applied).  Like 'Charlie' the stress response vs engineering strain is not linear.  1000 steps were used to run this study.

               

              'India' is 'Charlie' except done as a nonlinear static study.  This is the same as the original file in this forum thread.  No difference in results between study types noted.

               

              'Juliet' is 'Charlie' with 1000 elements instead of 5. Results are no different.  Note that in both cases the axial beam forces are identical across all elements anyway.  I did a study with 10,000 elements and there was no difference.

               

              'Kilo' is 'Charlie' without the large displacement flag.  Now the results are linear!

               

              'Lima' is 'Charlie' as a static study without large displacement.  The result is linear!

               

              'Mike' is 'Charlie' as a static study with large displacement.  The result is linear!

               

               

               

              So what about solids?  See Extension Test - Solid.SLDPRT

               

              'Alpha' is an attempt to recreate the same 'Alpha' from the above test with a solid mesh.  The material actually necks in the middle!

               

              'Beta' is 'Alpha' with the DirectSparse solver instead of the iterative solver.  Results are the same.

               

              'Gamma' is 'Alpha' simplfied (quartered).  Results are the same.

               

              'Delta' is 'Gamma' but I activated the large strain option and it necked at the restraint.  The mesh is also finer.

               

              'Epsilon' is 'Delta' without the large strain option (so a finer meshed version of 'gamma').  The study didn't complete but it was necking at the restraint.

               

              AD.png

               

              What causes this necking behaviour?  My guess is the FEA model isn't perfect, so just like a real test specimen a small stress irregularity quickly gets worse and snowballs into a neck.

               

               

              Conclusions:

               

              1) I have no idea what the nonlinear study property "use large displacement formulation" means.  It can't be the same as the "large displacemnt" option for static studies.  The SW help file doesn't explain this option.  Google searches all come up with results for the option related to static studies.  Anyone?

               

              2) The chart in the SW help file http://help.solidworks.com/2014/English/SolidWorks/cworks/r_input_stress_strain_curve.htm doesn't seem correct.  I'd say "Usually when SW computes the stiffness matrix it interprets material properties as if they are provided as true stress and engineering strain.  When using the large displacement formulation in a nonlinear study SW assumes properties are provided in terms of true stress and true (logrithmic) strain"  Note this statement doesn't refer to either large strain situations or the large strain option (which should be used in large strain situations).

                • Re: Stess / Strain curves; engineering vs true values
                  Shaun Densberger
                  Shaun Densberger Jan 14, 2014 6:44 PM (in response to Keith Frankie)

                  First and foremost: you can toss out the results with the beam element models. At the end of the day, beam elements are base off of beam theory, where a long and slender object is represented with 1 dimension. Beam elements can give good results if used correctly, but a draw back of a 1D element is that you lose some information by having only 1 dimension. The beam elements will not handle highly non-linear effects like necking, so you can leave them out (and stick with 3D solid elements) for your testing. Regarding the requirement for the Poisson's Ratio, KB doesn't specifically state how beams are formulated, but I'd be surprised if it wasn't Timoshenko Beam Theory. Without going too far into the theory, Timoshenko Beam Theory requires the Poisson's Ratio to calculate shear deformation. In fact, if you define a material with a Poisson's Ratio of -0.9999 (don't use -1), you'll get your beam elements to behave like Eularian Beam Theory (what you learned in mechanics of materials or some similar class). A Poisson's Ratio of -0.9999 results in a very large shear modulus, driving out the effect of shear deformation.

                   

                  Keith Frankie wrote:

                   

                  What causes this necking behaviour?  My guess is the FEA model isn't perfect, so just like a real test specimen a small stress irregularity quickly gets worse and snowballs into a neck.

                   

                   

                  While it is true that the FEA model isn't perfect an that there are irregularities in the stress distribution (at least on the nodal level), this is not the reason for necking. Necking is due to the Poisson's Effect, where strains in one direction result in strains in the two orthogonal directions. You ran a beam model case with a Poisson's Ratio of 0 (model "Echo") and didn't see a change; I suggest you re-run your 3D solid model "Delta" with a Poisson's Ratio of 0 and see what happens .

                   

                   

                  Keith Frankie wrote:

                   

                  1) I have no idea what the nonlinear study property "use large displacement formulation" means.  It can't be the same as the "large displacemnt" option for static studies.  The SW help file doesn't explain this option.  Google searches all come up with results for the option related to static studies.  Anyone?

                   

                   

                  By nonlinear, do you mean static or dynamic? I can't get on a premium seat of SW at the moment to check on where each check box resides and play around a bit. However, if "use large displacement formulation" is only available for nonlinear dynamic, then that might refer to the technique the software is using (just guessing). Typically, FEA (solid-mechanics) uses Green-Lagranian formulation, but I think for explicit codes (which I THINK SW uses for their nonlinear dynamics) it's more advantageous to use Arbitrary Lagrangian-Eulerian (ALE) formulation. Out of curiosity, why are you using nonlinear dynamics to do this?