4 Replies Latest reply on Jul 26, 2018 2:57 PM by Ryan Dark

    Weird looking simulation - Did i messes up with fixtures?

    Fernando Rossi

      Hello guys!

       

      I have a very very simple beam and have to check it for buckling.

      Results "by hand" went ok, but when i simulate it, i'm having some weird results.

      Did I mess up with fixtures?

       

      Its a simple beam (H150 x 1/4" thick) with 2 steel pins of 40mm on the ends. Beam will handle a 148KN compression force.

      I did a hinge fixture in the beam holes.

      Force (148KN) is aplied in both holes (should i have done half force on each hole?)

      It has a 500mm steel place on both sides for reiforce (I did the extrude with merge option, should be any different to use SolidWorks weld on it?)

        • Re: Weird looking simulation - Did i messes up with fixtures?
          Taylor Duran

          I don't have the Simulation package that includes buckling analysis anymore but I would start by modeling the beam using a weldment feature and then boss extrudes for the stiffening plates up to the surface of the flanges. If the profile you need isn't available there are plenty tutorials on how to create custom weldment profiles.

           

          Try a global bonded compatible mesh treating both the beam and plates as solid bodies and then again with the beam as a beam element and the plates as solid bodies with the touching faces of the plates and beams as bonded.  Double check your math that you've accounted for the correct end conditions (pinned-pinned => Leff = L) and the variable area moment of inertia throughout the cross section.

          • Re: Weird looking simulation - Did i messes up with fixtures?
            Ryan Dark

            Hi Fernando,

            I looked through your setup and some odd things stand out.  Why do you have both a load and a fixture applied to the same face.  This is surely messing up the results just by having the axial load ground out on that fixture.  I removed that face from the fixture and re-ran the study.  The buckling load factor went from -311 (an oddly high value and direction) to 0.021553 (pretty darn buckle-y) which is probably a more realistic result (but still not akin to what you describe)

             

            If you are trying to pin the end that has the load then you will need to explore a different fixture to act as a sliding pin.  Such a fixture could be created by making an Intersection Split Line onto the model (GoEngineer - SOLIDWORKS: Split Lines) using the right plane and the cylindrical hole faces.  Then, you would apply a "Use Reference Geometry" fixture electing only two coaxial split line edges and locking down the global X direction for those edges.  This would in effect make a pin that is capable of sliding in the Z-direction like many analytical buckling equations assume.

             

            Additionally, the "Fixed" type fixture applied to the opposite side does not make a pin-like constraint.  You would want to change this to a "On Cylindrical Face" fixture applied to the hole shank faces with axial and radial directions restrained while still allowing for circumferential movement to make this into a pin.

             

            That's a lot of changes now that I'm done typing it but the result is a buckling load factor ~0.18.  This image mostly illustrates how the setup now exists for reference.

             

              • Re: Weird looking simulation - Did i messes up with fixtures?
                Fernando Rossi

                Hello Ryan!

                 

                Why do you have both a load and a fixture applied to the same face.

                 

                Well, i thought that the pin would act as a constrain, leaving the beam to rotate freely, but the same pin also inputs the force to the beam.

                 

                If you are trying to pin the end that has the load then you will need to explore a different fixture to act as a sliding pin.  Such a fixture could be created by making an Intersection Split Line onto the model (GoEngineer - SOLIDWORKS: Split Lines) using the right plane and the cylindrical hole faces.  Then, you would apply a "Use Reference Geometry" fixture electing only two coaxial split line edges and locking down the global X direction for those edges.  This would in effect make a pin that is capable of sliding in the Z-direction like many analytical buckling equations assume.

                I'm having a hard time here to understand this. Do you mean that i have to split the cylindrical face on 2, like the image below:

                viga.jpg

                Then, on the "blue" marked faces above, I apply the 148KN force.

                On the other half face, I constrain on X and Y, using Reference Geometry, constraning just RADIAL movement. I used a AXIS 2 as the axis of constrain (the pink selection tab)

                tab)viga2.jpg

                This i did not understand. Half of the cylinder will be applied force (OK, makes sense),but the other half would act as a constrain?

                 

                On the other end of the beam, I used the cylindrical face, radial and axial fixture.

                 

                But, in the end, I end with this:

                The Iterative Solver stopped.

                The solver has numerical difficulties.

                Model may not have adequate fixtures.

                No results saved.

                  • Re: Weird looking simulation - Did i messes up with fixtures?
                    Ryan Dark

                    Fernando,

                    The study you sent over has a "Fixed" restraint applied.  This would not act like a Pin when applied to any face.  It would immobilize the face entirely, even from rotating.

                     

                    I see that you have made a new Plane but it is in the incorrect direction.  The Split Line must be applied along the plane of symmetry of the part which would be parallel to the Right Plane and positioned bisecting the model.  Change your plane to that orientation and you will have the edges you need for the "Use Reference Geometry" fixture.  Do not select a face though; select one of the split line edges.  Also, make sure you restrain the correct direction (global X) to make a pin behavior.  So, you are selecting edges that are aligned in the global X direction.

                     

                    If you remake the Use Reference Geometry fixture in this way you will find that the model becomes stable and does not give you the solver warning you have now.