How to model a pin inside a link plate?

J_Marc

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.

Victor

It sounds like there's no constraint in the vertical direction. In that case I would expect either a solver failure or a very large (and erroneous) rigid body displacement in the vertical direction if there's any slight imbalance in the opposing forces. There's bound to be some imbalance, especially with a distributed force on an irregular mesh. If that happened, numerical errors in the displacements may have also led to incorrect stresses.

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.

J_Marc

Hi Victor,
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.

J_Marc

Hi,
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.

Victor

Link_plate_coarse seems to be OK. I think you have an extra zero in your hand calculation. I get:

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.

Victor

It just occurred to me that you're probably interested in the stress near the hole, not in the middle of the plate. In that case, yes, you'll need a more refined mesh like you made, and will have to be careful about the distribution of the load. If you didn't have a hand calculation to compare to, you would have to repeatedly refine the mesh until the stress stops changing much. That gives you an estimate of the discretization error.

You can also replace hex8 with hex20 which don't need such a fine mesh to get as accurate results.

[Deleted User]

Hi,

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

J_Marc

Hi,
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.

Victor

You should expect much more than 416.7MPa there because it's a stress concentration. Not that 808.6 MPa is necessarily correct either though because of the coarse mesh.

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.

J_Marc

Very true, I forgot to include the stress concentration factor Kt 2.16
Nominal tension stress σnom 416.67 MPa
Maximum tension stress at the edge of hole σmax 898.28 MPa

[Deleted User]

Here is the link to Netgen; http://sourceforge.net/projects/netgen-mesher/files/netgen-mesher/6.0/

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.

Victor

Yea, you can sometimes get really weird elements buried in there with the automesher. I've found the worst ones seem to be where two faces of a tet are nearly co-planar and both on the same surface of the object. It looks perfectly OK visually but makes extreme stresses at that location and a mesh quality plot would pick this up.

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.

[Deleted User]

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. So that kind of ruined mesh density studies for me. Unless you know what the stress is supposed to be you will have no idea how many elements you need to match reality. I ended up just going with the element quality plot and the modal analysis results instead. I increase the element count until the mode shapes are well defined. But this is just me. I imagine everyone does things differently. You really have to test the part and do the FEA then figure out all the settings that work. But I'm curious what everyone thinks about this. This doesn't just apply to Mecway. The cube test is something I have done in a lot of software and they all seem to act the same way. So I have been a bit puzzled as to how a mesh density study does much good unless you have test data to match it against.

J_Marc

Hi Prop_design,
It's unfortunate but Netgen gives me an error after install. I am still experimenting with Mecway and I like it so far.

[Deleted User]

that error just means you need to install Python 3.4. if you installed the 32bit version of Netgen, install the 32 bit version of Python. vice versa, if you installed the 64bit version of Netgen, install the 64bit version of Python.

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/

J_Marc

Hi prop_design,
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.

[Deleted User]

hmm, yeah that is puzzling. i didn't know there was a python 3.5. however, i'm not familiar with python. i just spent several hours reinstalling it because SU2 also needed it. getting both programs to work correctly was a bear. i wish people didn't require python but it seems to be all the rage. i will check out your mecway files. maybe i can export the model into netgen somehow. it will give me a chance to learn something new.

[Deleted User]

so looking at your model, have you considered doing a 2d analysis. i think it would be more appropriate mesh wise. you could use a shell mesh. i was also wondering if you meant to have sort of hexagonal holes, rather than circles. that is creating stress concentrations. it doesn't seem like you can export a vol file. but your model is pretty simple and lends itself to creation in Mecway. i was thinking you were going from CAD to Mecway, in that case stopping over at Netgen is nice because of the element quality plot.

[Deleted User]

ok, so i'm not very good with creating models in mecway. so i took a few measurements of your model in mecway and re-created it in rhino. i then brought it into netgen and back into mecway. play around with it and see if it does you better. i think i got the dimensions right but please double check. i wasn't too sure on your materials and loads so i figured i'd let you take a look and go from there. hope this helps some. i attached the various files.

[Deleted User]

here is the model in 3d. gives you more options i think. you can get the element quality plot i was talking about when modeling in 3d. as you can see, Mecway brings in the netgen model in a really nice way (by grouping the surfaces for you).

[Deleted User]

i attached a first pass at an analysis of the 3d model. the stress distribution looks a lot more refined than your coarse model. when bringing the model in from netgen it seems like there is a unit conversion. the model was in mm but somehow when you bring it into mecway it is meters. so the previously attached models are probably the wrong size. your model wasn't properly constrained. i changed the frictionless support to a fixed support. you can perform a modal analysis on the part too. it is nice to do, at a minimum, just to see if the mesh density is refined. the modes should have well defined shapes, if the mesh density is high enough. i'll do that next. but this should give you a good start.

[Deleted User]

sorry for all the posts. the mode shapes look very well refined. so this should be a good mesh in my opinion anyway. I don't know that I have your loading right and the model size may or may not be right. so check it all out and let me know if this helps you any.

[Deleted User]

I did the stress and modes as a 2d model as well. they are attached as a zip file to save space. similar results as the 3d model. just showing two ways you can go about this. I prefer the 3d model approach as the modes are better defined and you get element quality. it's also easier to set the boundary conditions with the 3d model, as Mecway groups the surfaces for the 3d model import. you would have to test to see which is closer to reality.

johnkent

Since the upper surface of the pin hole pulls away from the pin, a more appropriate boundary condition is the compression only BC applied completely around inner surface. Below is a png of the stresses for 1280 hex20 elements with max stresses at the hole of around 230 MPa.

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.

VMH

I was doing a quick model and video of this and just saw your comments (johnkent). I agree.

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.

VMH

For this particular example, frictionless support on half of the interior face of the hole away from the load direction should also yield similar results because that half should always in compression and no tension.

johnkent

VMH - I recomputed my version with just the bottom half and a similar color scale so that our results are quite similar despite this model only has 672 hex20 elements.

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.

VMH

johnkent, thanks for your updates.

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

Victor

Hello prop_design. I'd like to address something you said quite a way back in this thread which I think it's quite important. You probably know some of this but it's also for other people who might be reading this because it's a common issue with deciding what you can and can't trust in FEA results. This is a bit tangential to the original discussion.

> 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.
Don't use the unrealistic idealizations - radius the reentrant corners if they're rounded in real life.
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.

[Deleted User]

thanks victor,

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.

[Deleted User]

attached are results and a model for a 0.1mm fixed displacement BC applied at one hole. the other hole was fixed. this represents the idea of two very stiff pins welded into the holes and then one pin being pulled 0.1mm while the other is held in place. but there are a lot of different scenarios that one can think up, so this may not be what you were going for.