Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Davit arm calculation
Hello, i am a mechanical engineer primarily focused on designing pressure vessels . In my work i have used mainly PVElite and Nozzle pro ( when it was necessary) so i am not that familiar with finite element analysis in depth .
On our latest project the client demanded that we support a rather large cover by way of davit and we calculated the davit arm using calculations from D. Moss's book . We reached a thickness of 80 mm , using a bar of S355J2 ( EN 10025-2).
The arm is holding very well , however i wanted to check it using a finite element software as well.
I got the free version of Mecway ( which , by the way i think it's a very nice software for new comers to FEA, especially because it lets users apply forces and supports on directly selected faces ) and modeled the davit arm as best i could ( i attached here the files) and i have a few questions because i think i am doing something wrong :
1 ) I wanted to model the brackets that hold the arm but i could only put fixed supports by choosing the faces and not the nodes ( when i put a fixed support on a node i get an error about the node not being on a beam element). How can i chose a node to make it a fixed support ?
2 ) Is the meshing correct ?
3 ) After running the analysis i got a von Misses stress of 13.46 MPa as an element value ( i read in mecway manual that it is better to look at element value than node value if i have a low number of nodes) which is much smaller than the yield strength of S355J2 at 80 mm thick ( 325 MPa ).Is my model correct and hence forth the analysis ?
Because it seems to me that if i modeled correctly and thus the analysis is correct , that i could have chosen a thinner bar for my davit arm.
Any response is more than welcome.
On our latest project the client demanded that we support a rather large cover by way of davit and we calculated the davit arm using calculations from D. Moss's book . We reached a thickness of 80 mm , using a bar of S355J2 ( EN 10025-2).
The arm is holding very well , however i wanted to check it using a finite element software as well.
I got the free version of Mecway ( which , by the way i think it's a very nice software for new comers to FEA, especially because it lets users apply forces and supports on directly selected faces ) and modeled the davit arm as best i could ( i attached here the files) and i have a few questions because i think i am doing something wrong :
1 ) I wanted to model the brackets that hold the arm but i could only put fixed supports by choosing the faces and not the nodes ( when i put a fixed support on a node i get an error about the node not being on a beam element). How can i chose a node to make it a fixed support ?
2 ) Is the meshing correct ?
3 ) After running the analysis i got a von Misses stress of 13.46 MPa as an element value ( i read in mecway manual that it is better to look at element value than node value if i have a low number of nodes) which is much smaller than the yield strength of S355J2 at 80 mm thick ( 325 MPa ).Is my model correct and hence forth the analysis ?
Because it seems to me that if i modeled correctly and thus the analysis is correct , that i could have chosen a thinner bar for my davit arm.
Any response is more than welcome.
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
I see a few possible problems with your model. First, the model doesn't match the provided data. The modeled diameter of the davit arm was 160 mm instead of 80 mm (see attachment). Also, it's best to use quadratic tetrahedral element (TET10) vs. linear tetrahedral element (TET4) for stresses calculation. There are a few papers on this but here is one (http://www.designspace.com/staticassets/ANSYS/staticassets/resourcelibrary/confpaper/2004-Int-ANSYS-Conf-9.PDF).
As for modeling the fix support, there are a few ways. I would also create the surfaces where the davit arm support located and then select those surfaces as your fix supports instead of fixing the whole area as you did but the results wouldn't be much different unless you use contacts to simulate the motions to your davit arm support (the two bracklets). Another way is by manually selecting nodes and restraining them (displacements) where the davit arm support located creating a coupling to resist the motion, but due to the meshing, you may not be able to select them nicely (see attachment).
See YouTube video below. Results are close to hand calculations. Maybe mesh refinement may get the results closer or maybe not all loads are accounted for. Hope this help a little. Note: 1 N/mm^2 = 1 MPa. Files are attached if interested.
If i could make a suggestion : could you possibly record your voice in the youtube videos ( maybe say like : why you use that kind of mesh for a particular shape , give more details about what you are doing...). I've seen in another thread that you asked if anyone knows about another free screen capture , you could use obsproject : https://obsproject.com/.
It is primarily used for streaming games to twich.tv but it also contains a feature where you can capture your screen and record it with sound on your local computer. It's open source , it works on mac and linux.
I also started with the non-commercial version and then upgraded to commercial version later on.
I do however have a few questions :
1 - You put as forces acting on the arm vertical force and horizontal force from Moss calculations. Those forces are the weight multiplied by a constant ( vertical impact factor and horizontal impact factor , values i don't know where Moss got them from ). My question is : if i don't have those constants , can i add only the force derived from weight ? ( meaning 655 kg multiplied by 9.81 to get the value 6523.65 in N )
2 - What is the value of 377.6 MPa ? I thought that von Mises stress gives the value at which the material enters plastic deformation but this value is bigger than the minimum yield strength specified in the standard for that thickness ( 325 MPa ). Also when you began moving the cursor down you reached the value of 166.2 MPa where i thing the failure starts ( from the red value displayed in the arm curve) Am i right or even close ?
Thanks again for taking the time to answer me .
1. If you know the actual loads, I would use those.
2. The peak von Mises stress sometime mislead the user that the stresses could be very high. It depends on mesh density, quality, etc. A mesh convergence study could be done to validate that. Sometime you may find that as you refine the mesh further and further, the stresses continue increasing which indicate that they are not real and can be ignored.
In practice, I focus more on the stress contours instead of just focusing on only the peak value because that value may be very localized or even not real.
I would run a coarser mesh first to obtain initial solutions (also to save some time to have an overview of the solution and identify possible errors). I then review the stress contours by setting the user-defined upper/max limit for von Mises to an allowable or acceptable von Mises stress (say 0.67 x material yield or 1.5 safety factor against yield). Areas in black (default. you can change this to gray or any other color under Tool --> Option --> Contour plot --> Out of Range) exceed the user-defined upper/max limit. I would focus more in that areas. Then, I run finer mesh to obtain the solutions. If the result differences are within say 5%, the previous mesh (coarser) would be adequate.
There are a few books that would be helpful to you starting out. One of them is Practical Stress Analysis with Finite Elements. It doesn't have too much theory. Another one is Building Better Products with Finite Element Analysis 1st Edition.
For the 2nd question, without have seen the model, means that you are above your material yield point, so is meaningless. A lineal analysis can gave results over the yield point and is telling you that you must improve the desing to decrease this value.
A non lineal analisys would gave you stress at this points at the yield value, but the strains would show you that you are reaching plastic deformations (thus the part is not usefull for normal engineering purposses).
- No mesh convergence study = no estimate of error = probably wrong.
- Peak stress is often at a stress singularity so it's also wrong. Most models have these and you have to judge whether to ignore them or improve the model.
With those concepts under you belt, you don't need to worry about choosing the right element shapes or much else since the mesh convergence study will reveal whatever error they cause. This is for solids at least.
Victor, is there any chance in near future for an additional option for displaying in MECWAY results the element stress at Gauss points? I think this will be a very useful information regarding evaluating the magnitude of any local/nodal stresses but also the quality of mesh.
In Nozzle pro i would input diameters of the shell , nozzle and thicknesses , chose the material for the shell and nozzle from the integrated database , input the forces and moments acting on the nozzle , pressure and temperature, and hit run. The software then meshes the model , analyses it and tells me whether or not the nozzle is withstanding those forces and moments ( so the software compares the results with the yield strength of the material taking into considerations the safety factors ).
For pressure vessels , ASME Sect VIII Div. 2 Part 5 in conjunction with ASME NB-3200 is my customer's FEA criteria. Also WRC 429 gives instructions on performing FEA on ASME pressure vessels but for me ,performing FEA on an entire pressure vessel, is like designing a nuclear pressure vessel in kinder-garden.
I think i need to understand first the basics of FEA if i want to move forward, that is why i wanted to start with something simple (or at least it was simple from my point of view ) like a beam with a force at one end.