Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
How to model a pin inside a link plate?
Hi,
This can either be a 2D or 3D problem. The manual problem would be to work the cross sectional area of the member and calculate the stress. My dilemma is that I don't get the correct answer. I get a very high stress much more than anticipated. I have placed a -F (force) on half the bottom hole & +F (force) on half top hole. I get both hole distorting in x-direction so I restricted the displacement around both holes. Increasing the number of nodes does not fix the problem. It seems that a node or elements are giving erroneous answers. I failed to save the problem so I am unable to load the liml for inspection but I will try to replicate the values again.
This can either be a 2D or 3D problem. The manual problem would be to work the cross sectional area of the member and calculate the stress. My dilemma is that I don't get the correct answer. I get a very high stress much more than anticipated. I have placed a -F (force) on half the bottom hole & +F (force) on half top hole. I get both hole distorting in x-direction so I restricted the displacement around both holes. Increasing the number of nodes does not fix the problem. It seems that a node or elements are giving erroneous answers. I failed to save the problem so I am unable to load the liml for inspection but I will try to replicate the values again.
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
I'd put a force on only one hole, and a constraint on the other. You could use frictionless support on half the hole so that the hole is allowed to deform around the rigid pin. Once it's working, you could go a bit further and use compression only support, though that'll be slower to solve since it's nonlinear.
Alternatively, model only one half and represent the symmetry with a vertical constraint.
Thanks for the prompt response, I have attached two liml file. Coarse & Refine 3D model of the plate in question. I was expecting the stress to be around 416MPa.
I have been experimenting. The closest I got to a consistent result was by converting the 500kN +Y force as a pressure of 265.3MPa normal to the arch surface. Superfine meshed the entire part to 10240 elements and 12663 nodes.
Stress = F/A
= 100kN / 0.0024m^2
= 41.7MPa
Mecway shows Stress YY = 40-42MPa on all the nodes in middle cross section of the plate.
Link_Plate_Refine looks good too with
Stress = 500kN/0.0024m^2 = 208MPa
compared to Mecway's result of 201-216 MPa.
You can also replace hex8 with hex20 which don't need such a fine mesh to get as accurate results.
You may want to mesh the part in Netgen, so that you can view the element quality. Mesh quality is difficult to determine by visual inspection. Often times a mesh that looks good is of poor quality in reality. It is very easy to mesh the part in Netgen, view the element quality, and save the mesh for import into Mecway. Mecway does a great job of importing the mesh so that you can apply loads to it easily.
Anthony
Yes I was more after the stress at the hole. I get 808.6MPa on the coarse; 500e3N/(120mm-60mm)x20mm =416.7MPa
I will try refining the mesh with hex8 & hex20. PS : Where do I get Netgen, Thank for your help.
That's a good point about element quality, Anthony. There are some "kite" shaped hex's here, but it doesn't look too severe to me, especially being away from the maximum stress region.
Nominal tension stress σnom 416.67 MPa
Maximum tension stress at the edge of hole σmax 898.28 MPa
I have a video on how to use it here; http://code.fosshub.com/PROP_DESIGN/downloads
Usually you can only see the surface mesh and not the volume mesh. Moreover, when you look at the mesh, you usually are only seeing one side of a pyramid or cube. So that side might look good but the element be junk. If there are thousands and thousands of elements, visually checking them all is not fun. This is why I recommend using the element quality plot in Netgen. The element quality plot enables you to quickly and easily see the quality of all the elements. This gives you confidence your mesh is good (without even actually looking at the mesh itself). It also eliminates the need for a mesh density study. You get a quality mesh on the first pass.
I wouldn't go so far as to say it eliminates the need for a mesh density study. Even perfect cubes and regular tethrahedra will usually give very wrong results if they're not fine enough. Once you've got a feel for how fine it needs to be, then perhaps you can get away with it though. I think you found that spot with the propellers, so there's not much need to recheck those types of mesh every time.
It's unfortunate but Netgen gives me an error after install. I am still experimenting with Mecway and I like it so far.
yeah I am new to Mecway also. i have found it is fantastic. not only for the price but the features. it makes a lot of things very easy that much more expensive software can't even do. i have compared it a lot to ANSYS 15 and 16 and it compares very well, in my tests.
if you post your CAD model and Mecway models, i can play around with them if you like.
here is the link to Python; https://www.python.org/downloads/
Yes, I installed python 3.5 the latest release but this version of Netgen likes python version 3.4. Thanks for the heads up. I didn't do a CAD model for the link plate. I created it in Mecway. As for the Liml file, they are uploaded on this forum third post. A coarse version and a refine version.
Problem with the frictionless support is that it pinches the sides of the hole with artificial stress concentrations.
All refinement, including recircularizing of the hole, was done within Mecway.
J_Marc, I'm not sure if you have a 3D CAD modeler of preference if decided to use for this example (we don't have to). Click on link below for a quick video.
FreeCAD was used for modeling of the link plate as an example. Taking advantage of symmetry of this type by only modeling half of the link plate.
A very coarse mesh for this example was used and was refined locally around the hole for convergence. Trial and error of meshing for demonstration purposes.
The max stress at the hole was found to be about 214 MPa using 100 kN applied axial tension, thickness of 20mm, hole radius of 30mm, width of plate of 120mm, etc.
But notice how in both of our results, the strap has deformed _away_ from the "pin" leaving only about 20 to 30 degress in compression on the bottom (would be instructive to know which elements actually in contact).
Now I'm thinking my "pinch" effect stress rise above for the 180 degree frictionless BC was an artifact of the abrupt change in BC.
btw, I only constrained two nodes on the bottom of hole as fixed. Mecway flagged these in red, but nevertheless nonlinear solution converged even with default tolerance to give a smooth stress distribution.
Quadratic hex elements (Hex20) require much less elements as compare to quadratic tet elements (Tet10) to get about the same results. If you look my video at my second meshing run (first refinement) at the hole, you will see I had about same as your max vonMises stress. But after refine it further, the max stress when down on the third run. Then on the fourth run after refine even further, there was no change in the max stress and reached convergence so the third run was good and no further refinement was needed.
I'm curious if you were to refine your model again around the hole, would your max stress convergence to about the same max stress you have now. In either case, our numbers are already very close and the stress contour are about the same. Thanks
> I have found decreasing the element size to usually be a bad thing after a while. If you take a cube and analyze it under it's own weight for instance. So just a cube of aluminum say 1in x 1in x 1in. Mesh it with perhaps four elements along each length and then keep increasing it. It seems like the stress just moves into the corners.
A finer mesh really does give more accurate results. If you're getting better results from a coarser mesh then the model or software must be wrong and the seemingly good result is only a coincidence, not a reliable improvement.
It's quite common in linear elastic analysis for the peak stress to keep on increasing without limit as you refine the mesh. This is usually caused by having a stress concentration that leads to a theoretically infinite stress. FEA software reports infinite stress by showing ever-increasing stress as you refine the mesh. Where this happens, there isn't some best mesh density that gives the correct stress - all these values are wrong. You'll know when this is happening because the stress won't approach any constant value, and that's a sign to ignore those stresses - if it doesn't converge, then it's meaningless.
The picture here shows a cube under self weight with a fixed support on its base. You can see the peak stress is at the corners as you described and this keeps increasing as you refine it so we can't trust any results at those locations no matter what the mesh density is. The problem is not that we refined it too much, but that the model is wrong - we're modelling a perfectly sharp reentrant corner with no material yielding, which won't happen in reality.
Some solutions are:
A) Ignore stress at these locations because the model doesn't reflect the real object. It'll still be OK in the rest of the model.
C) Use a nonlinear analysis with a plastic material model so that it'll yield and redistribute the stress as it does in real life - keeping it finite. This isn't available in Mecway but you can export to CalculiX to do that. For brittle materials, you might need some kind of crack modelling.
that is informative. i never knew exactly why this occurred, just observed that it did.
as for the boundary conditions and model for the original post. i am still not clear on what is trying to be achieved. the original model had holes that were not round. i took the liberty of assuming they were supposed to be round. as for the BCs, i have ran the model a lot of different ways trying to think of different scenarios one might test the part. you can get different results depending how you set things up. i would just recommend thinking of how this part is going to be used and model accordingly. i can't say what way is correct because i am not clear on what is trying to be accomplished. in any event, i still recommend everything i stated previously.
this is an interesting thread. funny how the simple models spur the most thought. i did run the model in ansys using the same setups and mecway and ansys match once again. ansys is a lot easier to bring in assemblies and you get more contact options. so if you were to model this part with bolts and nuts attached, it is easier and a little more options in ansys. but right now, even the attachment of bolts and nuts is unclear to me as you can do that a lot of different ways as well. after awhile you can only really model a plate in tension before you get confused on what is going on here.
for a single part, it is faster to get going and get results in mecway. it's also a lot more enjoyable than ansys (in my opinion). also, if you want your holes to stay round under loading you may want to fix one hole and then use a displacement boundary condition.