19 Replies Latest reply on Jul 17, 2013 9:43 PM by Ray Cardenas

    Thermal Question

    Ray Cardenas

      As an example: If I have a Solid Round Part and I add a Thermal Load of 75 Deg C, do the displacement results (Numbers on Color Bar) show the change in Diameter, or Radius?

       

      Also if I add a Thermal Load of -60 deg C, shouldn't the results show negative values?

        • Re: Thermal Question
          Mike Pogue

          Ray,

           

          Good questions. The colors in the displacement plot show the absolute value of the distance from a node's final position to the same node's starting position. It's just a subtraction of two vectors. The calculation does not realize this is a cylinder. You can interpret it as the radius, I'm pretty sure. You can also export ther deformed part.

          • Re: Thermal Question
            Shaun Densberger

            As Mike correctly pointed out, the displacement results show the displacement from the initial position to the final position for the nodes.

             

            I would be careful with assuming the displacement results you currently have as the radial displacements. Depending on how you constrained your system, the results on the outside edge of the rod could include displacement components from radial expansions and axial expansions. If you want to look at pure radial movement, then you need to define a cylindrical coordinate system and change you displacement plot results to the radial axis.

             

            Regarding the -60 deg C load, it depends on what results you are showing. If you have it list the magnitude (i.e. a scalar), then the displacements will always be positive. If can change the plot to show the displacements for a given axis (x,y, or z), then you will see negative values (if they exist).

             

            EDIT: Jared made a very good point in his post; make sure you set the proper zero-strain temperature!

              • Re: Thermal Question
                Ray Cardenas

                Hi Shaun/Jared,

                Just catching up to you guys. Thank you for the feedback. The constraints I have are Under the Advanced Fixtures - On Cylindrical Faces - with the center translation picked with 0 rad, and on the bottom of the part I picked the Roller Slider Constraint. Does this sound like it would work for radial displacement, or should I go with the displacement plot and radial axis method? I'm not sure if they are one in the same.

                 

                On the -60 C Question I believe I understand what your saying, so I'll see if I can set that up different.

                 

                How do I know if I'm in cartesian or cylindrical system? The zero strain I'm at is 77 deg F

                 

                Thanks guys,

                Ray

                  • Re: Thermal Question
                    Jared Conway

                    from the description of yoru restraint, you've told the software to allow the part to expand outwards (radially) and also axially. this should work BUT if you have any imbalance you might have some singular matrix problems..etc. consider some symmetry to solve this.

                     

                    for outputs, if you haven't chosen an axis or don't see cylindrical restraints in the bottom of your graphics window, you're probably working in cartesian. if you switch to cylindrical your outputs are radial, circumferential and axial dispalcements instead of xyz

                    • Re: Thermal Question
                      Shaun Densberger

                      Ray, it sounds like you have a constraint issue here. If you're trying to model the thermal expansion of a rod resting on a frictionless surface, then the easiest way to model it is using symmetry. We want the rod to expand radially relative to the center of the rod. One way to do this would be to prevent all radial movement of all of the nodes that are on axis with the rod; however, I don't know how one would do this in SW. Another way would be to make a quarter-symmetry model and apply roller constraints on one of the ends of the rod, and the two surfaces exposed by "cutting" out 3/4 of the rod (see link below).

                       

                      http://prntscr.com/1fu0g0

                       

                      The displacements you will get by default will not be purely radial; they will be a resultant of the radial and axial displacements. They might be mostly radial IF your radial dimension is much larger than your axial dimension; if it is the other way around (axial is much larger than radial) then the default displacement results will be mostly axial. You're best off making a plot of radial expansion via a cylindrical coordinate system.

                  • Re: Thermal Question
                    Jared Conway

                    hi ray,so we're talking about a static analysis where you've set the zero strain and then applied a body load of 75deg C? what was the zero strain temp?

                     

                    when you're displaying the results are you showing them in the cartesian or cylindrical coordinate system?

                     

                    what mike says is 100% correct but there might be more than meets the eye for this one if you're seeing results you don't expect

                      • Re: Thermal Question
                        Ray Cardenas

                        Hi Jared,

                        From your last comments it sounds like your refering to Hoop and Radial Stress - is this correct? If so is this the more accurate way of getting the Radial Displacements for a cylinrical part when applying thermal loads?

                          • Re: Thermal Question
                            Jared Conway

                            displacements and stress are separate

                            FEA solves displacements then calculates strain then calculates stress

                             

                            when we review these parameters the default funcitonality in simulation is to plot them in X,Y,Z components

                             

                            if we choose an axis, we are provided the results in radial, circumferential and axial displacements relative to the axis

                             

                            if you choose stress, the answer is similar and you get hoop and radial stress components

                             

                            i don't really know what you mean by "accurate way" the output is the output. accuracy is based on your problem setup. if your displacements are accurate, your stress is "accurate". accurate is relative because of other conditions like singularities, concentrations..etc.

                              • Re: Thermal Question
                                Ray Cardenas

                                Hi Jared,

                                My mistake I meant Hoop and Radial Displacements, not stress. Also "accurate" was a poor chioce of words, what I've been asking for is the correct way of setting this up. Bottom line, it seems as if I need to constrain this rod by the center axis so that it expands uniformormaly from the center, which I may have already done. I will use a different approach based on what I'm hearing from everyone here and compare to what I done already, and finally verify with a hand calc.

                                 

                                Thanks for the help Everyone

                                  • Re: Thermal Question
                                    Jared Conway

                                    just to add here, shauns' saying if you choose resultant vs a component, you'll get deformations that are made up of all the components of displacement root sum squared.

                                     

                                    also from an analysis perspective, 2d axisymmetric would be the easiest way to deal with the restraints, other symmetry like half and quarter or a slice would be fine too. restrainint along the axis will be difficult but could be done. you'll need to split the body to do that and then you might as well do 2d or other symmetry

                                      • Re: Thermal Question
                                        Ray Cardenas

                                        I saw a video on line not too long ago showing how to do Hoop and Radial Analysis. It showed using a quarter of the part, using Rolling Sliding constraints on the cut surfaces and the ends, and picking a center axis. Aside from the Von Mises you needed to define new plots for stress and displacements. It sounds like this is what I really need to do, along with adding the Temp Load, and in a round about way is what I'm hearing from the responses.

                                         

                                        My 2 cents

                              • Re: Thermal Question
                                Mike Pogue

                                I'd add two things to all the correct advice here:

                                 

                                1. If you are doing symmetry, you probably ought ot go all the way and do a 2d simplification.

                                 

                                2. The actual easiest way to simulate thermal expansion if there are no non-linearities (interferences or bonds with dissimilar materials) is to insert a scale feature with the scale factor = 1+CTE*(T1-T2).

                                  • Re: Thermal Question
                                    Ray Cardenas

                                    Hi Mike,

                                    I've never heard of this technique using a scale feature. If it isn't too much trouble, would there be any way you could explain this a bit more, or maybe send me a link on how to do this?

                                      • Re: Thermal Question
                                        Mike Pogue

                                        If I understand what you are trying to do, based on the fact that you have not physically restrained the part, you are trying to see how the size of a part changes with temperature. I am also assuming there is only one material in your part.

                                         

                                        If this is true, then the answer is that every dimension scales linearly with the CTE*(Tend - Tstart). This is under the assumption that CTE is constant with respect to temperature. While this assumption is false, it is a standard engineering assumption and it is the same assumption the FEA makes.

                                         

                                        So, under all of these assumptions, you can compute the scale factor with a pencil: S = 1 + CTE*(Tend - Tstart). You can then, either with a pencil or by inserting a scale feature in solidworks, calculate any dimension in the part at Tend directly. I think this is an easier way to get the information. You'll notice that S will be less than 1 if Tend is less than Tstart.

                                         

                                        If this is not what you are trying to do, sorry.