-
Re: How to Simulate a Bump Test?
built into modal time history is the ability to use a sine wave directly, if you can make the bumps a sine, then you can leverage that directly. otherwise build the curve in excel and input it.
and you're right, this is going to take a long time. what do you wnat to learn/gain from this analysis? what do you think will happen over multiple bumps? most people are concerned about things breaking free or loosening from multiple bumps which isn't really going to be shown in a simulation.
if you still want to go down this path and you're interested in the maximum response,and you're ok with a sine wave, you could look at a harmonic analysis
-
Re: How to Simulate a Bump Test?
Unfortunately cannot do anything to convert the half sine into a full sine wave. Its part of the product requirements. So cannot use a full sine wave. If I did it wont really be a bump but more of a vibration. So harmonic analysis is pretty much ruled out.
My objective is to assess the stresses and displacements around the critical areas like that near the contacts of the surfaces so that it does not exceed the tensile strength of the fasteners and the material of the enclosure.
My concern is from previous experience that increasing the time step will increase the computing space and time by a lot. In this case if I were to consider 4000 bumps with a repetition rate of a bump per second that would be a total of 4000 seconds. Considering the pulse duration that I have been given is in milliseconds I pretty much shudder to think what's going to happen if I were to put a time increment of a smaller order. I might actually have to go on vacation for a few days whilst attaching 10 Terabytes of hard drive to my computer. But that might be nice too.
Any suggestions on what can be done???
-
Re: How to Simulate a Bump Test?
let's look at it from a more physical perspective, what do you think the bumps are going to do to displacement and stress? do you think you're going to get super position of the input waves such that there won't be enough damping and the structural displacements and stresses will increase? if so run a sample curve for a shorter period of time and see if that happens. if it does, you're stuck with what you describe, if it doesn't maybe this test isn't necessary. remember, we're talking about linear static analysis. there won't be any material wear if that is part of your concern. you'd need nonlinear dynamic for that.
but then, think about this, if you do this as a physical test, how long will it take? how many prototypes do you need to test? even if you go with a larger time step, draft quality elements and a coarse mesh, you can still narrow down what you need to do a lot quicker than you could physically.
i think you've identified the limitations you have, but you need to go back and figure out if simulation is "worth" it in this case and if it is, what assumptions are you willing to get away with to get a solution in a reasonable amount of time. this is the balance you always have to work with.
-
Re: How to Simulate a Bump Test?
Thank you very much for all the help Jared! You are right I think that stress will increase with the increasing bumps and that is what I want to try and identify. I will try what you suggest. I might try this for for a duration of 5 seconds and see what I get.
Fortunately I am only validating one of our designs so I have some time but not a lot of it. Just a question about the time step. Will a larger timestep be enough to cover this problem? The pulse duration I have been given is of the range of 6 milliseconds but If I were to take the time increment to be around 0.1 or 0.01 seconds would that affect the accuracy of the result seeing that the duration of the actual pulse is much smaller than the time step?
I think the balance here is between time, computer space and accuracy. In the end I might just run a few simulations at 1 seconds then 2 seconds upto 5 seconds and see If I can extrapolate the data on excel. May not be the most ideal way but I guess I have to come up with some kind of workable solution for now.
-
Re: How to Simulate a Bump Test?
your time step definitely cannot be smaller than your input curve if you want results that will capture the behavior properly. if you're interested in some additional training, feel free to contact me at jared@hawkridgesys.com. This is a service that we offer here at Hawk Ridge Systems.
-
-
-
-
-
-
Re: How to Simulate a Bump Test?
Atif,
I would try simulating one bump. The reason that people choose to do 1 to 3 bumps per second is that they want it done in a reasonably short period of time and they don't believe that the system is going to move in such a way that the bumps interact with one another. If you run your simulation for a total time of a few times the bump period and everything is damping out quickly, then you are pretty sure that the assumptions were correct. Of course, this all assumes that you have a good handle on the damping in your system, which is often not true.
Jerry S.
-
Re: How to Simulate a Bump Test?
Thank you Jerry. I think what you and Jared have suggested earlier are right. I carried out the simulation for 3 bumps in one second taking a time step of 1 millisecond. I examined the stress plot and as expected found that the stress is highest at the part where the input curve peaks (thrice). I also found that the stress at each peak is pretty much the same and the stress on the last step is significantly lower so that pretty much shows that the stress does not increase with the no of bumps.
But since there is a constant loading and unloading wont there be fatigue which needs to be accounted for. I looked at the manual and found that you can do fatigue analysis on Solidworks. According to the manual linear studies do no predict failure due to fatigue. Will the fatigue analysis work for a linear dynamic analysis or is it only for static analysis? Can I take the results for just one second from the linear dynamic analysis and then apply it for say 1400 or 4000 cycles?
-
Re: How to Simulate a Bump Test?
what you're seeing from a dynamic perspective makes sense but remember that it is also affected by damping.
regarding fatigue, remember that solidworks simulation is high cycle fatigue.
as per the help, you can bring in a time step from a time history analysis: http://help.solidworks.com/2013/English/SolidWorks/cworks/c_Fatigue_Events.htm?id=3a2d2fc53ad34cb29cb4f2dd413dbf19#Pg0
-
Re: How to Simulate a Bump Test?
Atif,
Four thousand cycles is not very many for fatigue. I would not try to do a fatigue analysis in SolidWorks, I would just go through the numbers in a text book type of analysis. You will most likely find that it isn't an issue, unless your stresses are quite high.
Jerry S.
-
Re: How to Simulate a Bump Test?
Why would it not be a good idea to do a fatigue analysis on solidworks? Is there any particular reason?
The stress levels I have reached at the curve peaks are approximately 12% of the tensile strength (around 290MPa) of the material that we are using. Would that be considered as high enough stress for factoring fatigue?
-
Re: How to Simulate a Bump Test?
Atif, check an an curve with your data to determine if fatigue could be an issue.
Regarding solidworks fatigue, it is meant for high cycle fatigue, similar to the standard sn curve check. What jerry is saying is what you're doing may not be considered high cycle. Read up a bit more before making a decision.
-
Re: How to Simulate a Bump Test?
Thank you for the inputs. I did some research and found a good paper on fatigue data on the material that we are using. Turns out I was worrying too much and what Jerry had suggested earlier was right when he said that 4000 cycles will not be a problem. Fatigue only seems to be an issue when you reach an order 10^5 cycles. The stress is also well under the limit. Manager seems to be happy with the explanation too so all turned out well.
Again thank you very much Jared and Jerry for helping me out. This discussion was really helpful.
-
-
-
-
-