18 Replies Latest reply on Mar 3, 2015 8:17 PM by Jared Conway

    Gravity(Acceleration) in simulation

    Pk M

      Hi I would like to know if we have to apply gravity (acceleration) load for a lifing load simulation. The study I want do is for a overhead crane lifting bracket (stainless steel) for an equipment for "5g" load case. The weight of the equipment is 40lb. I applied 5g load (200 lb) as a remote load  at center of gravity(I am more used to Ansys where when I apply gravity, it used to show corresponding force acting upwards).


      In solidworks simulation,as per help file, it looks like we dont have to give gravity. I just ran above 3 different studies to see affect of gravity - with Gravity UP, Gravity DOWN & No gravity. Interestingly all studies gave almost identical results. I couldn't make sense out of it. I would greatly appreciate if somebody could help me understand it.




        • Re: Gravity(Acceleration) in simulation
          Jared Conway

          results for your up case didn't get included in your pdf


          where is your remote load attached to?


          a case you might want for comparison is the gravity load only.


          seems like a reasonable setup to me. what results are you expecting that you aren't seeing? also what assumptions are you ok with for this anaylsis? could you elaborate on what you do in ansys? and just to be sure, no error messages or anything when running the problem?

          • Re: Gravity(Acceleration) in simulation
            Anthony Botting

            Hi Pk: Jared is right. Try these tests, just to satisfy yourself:


            1. run one more study with gravity only, pointing down (supress remote load). Then, check force reactions at all the supports. The sum should be equal to the weight of your structure and the resultant sum vector (which you can show on-screen) should point upward. Take note of max displacement.

            2. Unsupress remote load and run again. The reactions should now sum to 6g (6 x weight of the structure). Check the max displacement should be about 6x bigger than step 1 (assumes linearity, no stress concentrations or point fixtures).

            3. ANSYS uses opposite directed arrow only because of their sign convention. They use weight body force, F = -mg. SolidWorks' uses weight body force, F = mg, which points their vector in the opposite direction. However, both softwares give the same effect if you stay with their respective convention.

            Hope that helps.

              • Re: Gravity(Acceleration) in simulation
                Pk M

                Thank you Jared & Anthony.


                Let me expalin about this case. This bracket is overhead crane adapter for an equipment (weighing 40 pounds) we use in shop. we use this bracket to move it all around the shop. I want to run study for load case of 5g. I applied 5 * 40 = 200 lb load as remoteload at center of gravity of the eqipment (which is 10 inches below along Y and 1 inch along Z). The weight of the bracket itself is 12.8 pounds (which I didn't included while applying 5g remote load of 200 lb).


                I ran another study as you suggested - with only gravity. The reaction force in Y direction at all 4 supports as follows 9.6 lbf, 6.4 lbf ,9.6 lbf & 5.4 lbf. Resultant reactions at same supports are 14 lbf, 6.72 lbf, 14 lbf & 6.75 lbf. None of these sums equals to weight of the bracket which is 12.8 lb. Max displacement in this case is .00033 in.


                Above values with 5g load and gravity down are as follows. Y reactions are 85.7 lbf, 30.4 lbf, 85.3 lbf, 30.7 lbf.  Resultant reactions are 187 lbf, 30.9 lbf, 186 lbf & 31.3 lbf.  Max displacement in this case is .00604 in.


                I am not sure where I m doing wrong.....I appreciate if you can help me understand it......thank you so much.

                  • Re: Gravity(Acceleration) in simulation
                    Jared Conway

                    hi pk, let's take a step back and work on a simpler model that you can share with us so that we can take a look at what you've done.


                    make a cantilever beam and run these studies:

                    1. gravity only (point gravity in the direction that gravity acts)

                    2. gravity + a known load at the end

                    3. gravity (1x) + a known load at the end x 5


                    Before you setup and run these analyses, take a guess at what you think the reaction forces should be and see if they match up to your simulation.


                    Also, this might be a stupid question, but what are you trying to account for with the 5G load? and is it only the load or do you want the bracket to also see 5x its gravity load?

                      • Re: Gravity(Acceleration) in simulation
                        Pk M

                        Hi Jared,


                        this load case is - scenario, where object is moving down with 5g speed and see how bracket works. So I gave gravity force of 1931.10 in/s^2 ( 386.18 *5 = 1931.10 in/s^2) acting downwards along with 5 * load. Do you think is that wrong practice??


                        Thank you very much for your suggestion. I ran series of studies on simple cantilever bar. It helped me to understand better and I think answered my questions.


                        My obeservations:

                        1. 1. ONLY gravity - As Anthony mentioned, when only gravity is acting, reaction force equals to weight of the bar, which is 1.73 lbf

                            This is obvious

                        1. 2. When only 100 lbf is acting (without gravity), the reaction force is 100 lbf.
                        2. 3. When 1 x gravity DOWN + 100 lbf acting, reaction force is 102 lbf.

                            I assume this because both forces are down 100 + 1.7 ~ 102 lbf.

                        1. 4. When 1 x gravity UP + 100 lbf acting, reaction force is 98.3 lbf. (this I did to make sure reaction force is less than 100 lbf)

                            I assume this because 100 - 1.7 = 98.3 lbf.

                        1. 5. When 1 x gravity DOWN + 5 X 100 lbf acting, reaction force is 502 lbf. Also as Anthony pointed out, max. displacement in this case is 5 times than that of case 3. 

                           I assume this becasue 500 + 1.7 ~ 502 lbf

                        1. 6. When 5 x gravity DOWN + 5 X 100 lbf acting, reaction force is 509 lbf

                           I assume this becuase 500 + 5 * 1.7 = 509 lbf


                        My interpretation:


                        1. 1.From Study 2, As reaction is 100 lbf, this tells me that solidworks doesn't apply gravity by default. We have to apply gravity for all problems involving forces on structures, for results to be more accurate.

                        2. From Study 3 & Study 4, in solidworks we have to select gravity down if we consider subject moving down in that load case. This answers my very question.


                        What do you think? I can share those 6 studies if you are interested to take a look at.

                  • Re: Gravity(Acceleration) in simulation
                    James Riddell



                    We do this here all the time.  To get the 'load' of your parts you must place them in a gravitational field.  If you want to show acceleration/deceleration or inertial loading it is easy just to multiply 'gravity' by 1 +/- your factor and do the same to all your remote loads (since gravity won't act on a force.)  I have not tried it on remote masse in SW.  If you are doing a static linear analysis, or close enough, this will give you a realistic answer.




                    Addendum: If you are looking at a dynamic situation you need to define what is going on, i.e. how much energy you need to absorb.  That you can calculate from first year physics class equations fairly easily.  You'll need to know velocity, distance to stop, etc.

                    • Re: Gravity(Acceleration) in simulation
                      James Riddell



                      Point of clarification here for the discussion's sake:


                      Are you trying to simulate a dynamic load (impact) or are you simulating a proof loading (factor of safety-max load) condition.  If the former, you should probably approach using a dynamic analysis; if the latter then you could use static linear analysis.