I have heard from another source that the bearing load is busted - it did not produce the same results in a buckling calc as the force option did. This resulted in a bent very long hydraulic cylinder as it wasn't obvious the bearing load was not behaving - at least to the practitioner who did the analysis - his boss figured it out though. I have not used the bearing load in a while so you may want to file a bug report.
Hi Bill, thanks for the reply.
After a bit more investigation it does look like it could be a bug. I've modelled a simple flat bar with a hole in it and the deformed shape shows a "twist" that I wouldn't expect to see.
Image below shows the problem. I know that the deformed shape is massively exaggerated by the software but this still seems odd.
I'm on the Academic 2011/2012 version. Could some kind person with a full 2011 or 2012 with latest service packs please try to replicate to see if the issue exists in the commercial version?
Since you did a test case (good for you), can you move the bar around wrt the origin and see if it changes the result?
Also can you vary the mesh in the hole, say one side coarse and the other fine and see if that changes the results?
Can you switch from draft to normal elements and see if that changes the results?
And of course last but not least, what were the global reactions when you get this results. They should exactly equal the force applied to the pin hole. If not you have a serious bug.
Here's the results from various tests on my flat bar with a hole:
Draft mesh - Default mesh setting. Same result
Normal mesh - Default mesh setting. Same result
Normal mesh - Coarsest setting - Same result
Normal mesh - Finest setting - Same result
Fine mesh on front face, coarse on back face - Same result, still bends in the same direction.
However, a coarse mesh on front face, fine on back face gives a bend in the opposite direction.
Using a force instead of a bearing load gives a perfectly straight pull, no matter what the mesh settings are, and even with a coarse mesh on one side of the part and fine mesh on the other.
So it looks like the variation in the mesh on each side in combination with a bearing load leads to some kind of torque or moment effect.
What are my alternatives to bearing load? I could split the face and use a straightforward force I suppose, or is it possible to create a bearing load type variable force across a cylindrical face some other way?
I meant Draft mesh and a High Quality mesh. The imposition of the load into nodal loads as a lot to do with whether the elements have midside nodes or not. Changing reactions due to changing mesh is a bit troublesome.
I was suggesting splitting the faces down the long centerline so half the hole in bearing has a fine mesh and half a coarse mesh. But I think you captured the problem enough to send it in.
You can also plot stress across and around the hole.
Silly me, looking at the scaling on the displacement plot shows a very tiny displacement off axis in line with the ever so slightly out of balance global reactions. The displacement magnification is around 17,000 in one direction and around 1,000 in the other. There should have been global reaction moments too and they should have been zero. This is troublesome, but perhaps not a show stopper just yet. .15N/10,000N is pretty good actually. That can be due simply to numerical accuracy.
And like Bill mentioned, you didn't have the load on the edge instead of the face did you?
Forgot to add..
Load applied was 10000N
Reaction forces for the entire model are listed as:
Would this be classed as being within acceptable levels of error?
It shouldnot bend that way no matter the deflection magnitude if it was applied in the vertical direction so something is not right. Do the reactions equal the applied load?
After looking at the picture a bit closer is hte load applied to the hole edge or the face of the bore? It should be on the face.
I can confirm that the bearing load is on the face, and not the edge.
The part is modelled about the origin and is perfectly symmetrical. The bottom face of the bar is fixed, and the co-ordinate system used to define the bearing load is right in the centre of the hole, halfway through the thickness of the plate.
As I mentioned in my last post, using a force instead of a bearing load gives a perfectly vertical deformed shape so it looks like the bearing load command is at fault here.
You can use the force command and then use the non-uniform option. You have to use a 2nd order parametric polynomial to approximate the load. A parabolic distribution should be close enough and reference it to a local coordinate system would be the most convenient thing to do.
A late reply, but in case anyone still looks at this question, without seeing your mesh it's hard to tell, but if it isn't symmetric your bearing load distribution will not be perfectly symmetric. What is the actual value of the lateral displacement? Probe the far corner at the top to see what the actual value is. Having a deformation scale of 17800 is pretty extreme, indicating the model displacement is very small (as your numbers indicate, as well).
You can also show the reaction force at the restraint to identify how much side load is being reacted through the boundary condition/restraint. I do see a .06 lbf out of plane reaction force for my 2,000 lbf bearing load, and a .0089 lbf lateral reaction force, but that is a reasonable error given the few numbers of elements and any assymetric elements surrounding the load and the rest of the structure.
Maybe they fixed it in 2013, that's what I'm running it on now, but I applied a more ridulous load not knowing all your geometry and I get .0099" displacement, but it is perfectly symmetric.
Regardless, you can reduce the effects of this problem a bit by adding a mesh control to the surface of the hole, so it uses a consistent element size at the interface.
I just used default mesh control settings, but it reduces the out of plane reaction force from .06 lbf to .0145 lbf and the lateral reaction force from .0089 lbf to .0040795.
The reaction force can be used in a separate simulation to see how much deflection and stress it causes. I think your model issue is splitting hairs, based on the above, like I say, unless something was fixed by the 2013 version.
By taking that same model and applying only the reaction load I mentioned in the first case I see a .0006" deflection when applying the load at the top edge of the part, and it causes less than 24 psi of stress. If you have ever used a tenths indicator (one ten thousandth of an inch), a deflection of .0006" can be made by taking a breath while holding the indicator or part, across a 7 inch length, which is the bar I modeled.
Regardless, there are some tools in SolidWorks Simulation/Cosmos that can help you diagnose whether it should concern you or not. My thoughts are that I'm not worried about it because I know I wouldn't expect the load to be 'perfectly' aligned with only one axis anyway.