18 Replies Latest reply on Jun 19, 2014 6:42 PM by Jared Conway

    Displacements Too Large

    Nathan Cassou

      I have a temperture probe that I am trying to set up for a fatigue study.

       

      Assumptions:

       

      -The probe gets up to 1200*F and then cools off when the engine shuts down

      -A force is put on the tip of the probe (value unknown) as cyclic loading from a hot air stream. I have seen a sample of the probe and tips are always a bit bent after x amount of hours of use.

       

      I have tried everything I know to stabilize the assembly to get reasonable results. I even tried to back off the force on the tip to around .001 lbs to eliminate the chance that it could be too much force. However I still get the "Displacement too large" error box. I have used bonded contact sets on all the parts and tried various static fixturing methods but none seemed to work. I set the solver to automatic and "Large Displacement" box checked but the simulation still fails.

       

      Any thoughts?

       

      SEE ATTACHED PICS

       

      Nate

        • Re: Displacements Too Large
          Shaun Densberger

          There is most likely a meshing issue at the interface between components. That being said, it looks like (at least based off of the information I have) this model can be simplified. Do you really need the other components? Also, it looks like you have geometry interfering.

           

          Unnecessary Geometry.png

           

          Geometry Interference.png

            • Re: Displacements Too Large
              Nathan Cassou

              I have tried simulations with exlcuded parts that wouldn't really have a bearing including that sheath as well as that upper body. The middle body has the probes brazed into it. I still get the same result.

                • Re: Displacements Too Large
                  Shaun Densberger

                  How are the probe (orange) and the middle body (light blue) in contact with one another in the model? Are they touching on flat surfaces of each component, or are the two cylindrical surface at the non-loaded end the contact location? Can you show me some pictures of just the two from several different angles?

                   

                  EDIT: Post a copy of the model (if you're allowed to).

                    • Re: Displacements Too Large
                      Nathan Cassou

                      Yes, they are two cylindrially mated surfaces. I used a bonded contact between the two.

                        • Re: Displacements Too Large
                          Shaun Densberger

                          Yes, they are two cylindrially mated surfaces. I used a bonded contact between the two.

                           

                          Just to make sure we're on the same page, this connection is just like two cylinders touching (see below), correct? Is this the only connection that the middle body has to any other body in the assembly?

                           

                          http://upload.wikimedia.org/wikipedia/commons/thumb/e/ef/Kontakt_paralleler_Zylinder.jpg/220px-Kontakt_paralleler_Zylinder.jpg

                           

                          If so, then this connection is what might be causing your large displacement issue. I say might because there are different factors in how the software can handle this.

                           

                          In the above images, the contact between the two cylinders is a line (two circles touching creates a point of contact; that point extruded along the length of the cylinder forms a line). In FEA, bonded connections for line contacts can be handled in different ways, and vary from package to package; this is where the 'might' comes into play.

                           

                          Typically a bonded interface between two elements in a FEM is done using node sharing. For a line contact with solid elements, node sharing should result in a hinge. This is because solid elements nodes only have three Degrees of Freedom (DOF): dx, dy, dz (the three translation DOF). Solid elements don't have rotational DOF (rx, ry, rz), where as shell and beam elements have all six DOF (dx, dy, dz, rx, ry, rz). If the z-axis is collinear with your cylinder axis, then your system will allow rotations about z along the line of contact.

                           

                          Whether or not the above will be true depends on several different things within the software package. I'm not 100% sure (can't get on SW at the moment), but SW might be using a multi-point constraint scheme to handle a bonded connection (instead of node sharing) for a line contact. If that is the case, then the model should be stable. If SW is using node sharing, then it won't be.

                           

                          All of that being said, it's generally bad practice to have line contacts. Brazing these two components together will involve a filler material, which will change the line contact into a surface contact. What you could do is go back to your model with just the two components (middle body and probe) and apply two fixed geometry constraints to a single surface on each part (one constraint per part) and see if that runs (it should). After that, remove the constraint from the middle body and try to run it again. If it doesn't run then we know the issue is most likely the connection between the two components. You can then modify your geometry to account for the filler material (thereby creating a surface contact over a line contact). I also suggest you delete the global bonded contact definition and set one up manually.

                           

                          Let me know what you get after trying all of this.

                  • Re: Displacements Too Large
                    Jared Conway

                    can you post the exact error message?

                     

                    also how are you going to use a fatigue analysis for this

                    " I have seen a sample of the probe and tips are always a bit bent after x amount of hours of use."

                      • Re: Displacements Too Large
                        Shaun Densberger

                        Good catch, Jared. Typically fatigue results in a fracturing of the material, not permanent deformation. Given the elevated temperature, I'm thinking this might be a creep phenomenon.

                        • Re: Displacements Too Large
                          Nathan Cassou

                          Jared, this would be my first fatigue simulation. It looked like you set up other studies and then use them in a fatigue study. Correct me if I'm wrong. Shaun it could very well be. I don't know a whole lot about the application of these probes. I have to assume however that the high to low temps that these experience could be used in a fatigue study.

                            • Re: Displacements Too Large
                              Shaun Densberger

                              What type of materials are we dealing with here?

                                • Re: Displacements Too Large
                                  Nathan Cassou

                                  On the effected parts:

                                   

                                  Lower body that holds the probes - Inconel 600

                                   

                                  Sheath - Hastelloy X

                                   

                                  Probes -  Hastelloy X

                                   

                                  Pics of the body that holds the probes. Shaun they are mated to this. Not mated together.

                                  Probe FEA 5.PNGProbe FEA 4.PNG

                                    • Re: Displacements Too Large
                                      Shaun Densberger

                                      Hmm, not familiar with either of these alloys, but after a quick Wikipedia read I'm leaning away from creep. How many hours are they at elevated temperatures for?

                                       

                                      I'd start with a basic static analysis to see what the stresses and displacements are like. You said that there is a cyclical force applied to the probe; do you know the oscillatory frequency of this load?

                                        • Re: Displacements Too Large
                                          Nathan Cassou

                                          So this is the error message I get when I run a static analysis on one probe in the lower body as shown. Only 5 lbs at the tip.

                                           

                                          Probe FEA 7.PNGProbe FEA 6.PNG

                                            • Re: Displacements Too Large
                                              Shaun Densberger

                                              Where are you applying your constraints (I don't see it in the picture you posted)? Did you replace the global bonded contact with a manual contact between the outer surface of the probe and the inner surface of the part that holds the probe? Can you post a screen shot or table of the material properties you're using?

                                               

                                              This model looks very basic, so we should be able to get this to run (without a warning) in no time (famous last words...).

                                              • Re: Displacements Too Large
                                                Jared Conway

                                                the error message indicates that you either have too high of a load and are getting large displacements that don't work with the linear static (small displacement) assumption

                                                 

                                                or you're missing how things are connected together.

                                                 

                                                i would recommend you start small, just analyze the gold rod with the load. see if you can get that to work. if youcan, add the next part and so on.

                                                 

                                                but i'd also take a step back and answer this question

                                                " don't know a whole lot about the application of these probes."

                                                 

                                                fatigue isn't going to show it bending after being cycled. you need nonlinear with a von misses plasticity model. or like shaun said, it might be creep. which would also be nonlinear.

                                                 

                                                all that fatigue is going to tell you is the life of the part

                                    • Re: Displacements Too Large
                                      Nathan Cassou

                                      Okay so I finally tried just changing the material of the probe from Hastelloy X to 321 SS rod to see if a stronger material would make an difference. It now runs with any load and good results.