higher stress values on 1 node than neighbors- ignore? 1

[StevePAA]

here's a general question that would apply to any FEA program.

I've recently done some FEAs on round flat plates, fairly easy analyses, relatively low stresses, basic stuff. Lets say a 15-18" dia .5" thick plate using a .12 mesh size. Just making up numbers, I'll get a max stress of 6000 psi occuring on one node, and then on all the nodes surrounding it get 5000 psi or lower- say 15% lower on all surrounding nodes. The max stress is not in a critical area- away from any holes, edges, cuts, etc; just on the flat area of the plate. I usually discount the high value if not in a "threatening" location and use the nearby more commonly occuring values of 5000 psi to calculate the factor of safety. I don't do this if the max stress is on a corner, near a hole, etc.

Would this be viewed as ok by another FEA user who might look at one of my reports in the future, or am I setting myself up to be crucified?

 

[GBor]

It depends on the situation. In general, the answer is, "no", but particularly in something as simple as a flat, round plate, the question is why does such an anomoly occur?

Some "rules of thumb": If the stress gradient across any element is greater than 10% of the stress range in the problem, you need to refine the mesh in that area. Stress "hard points" (like the one you suggest in your post) are generally ignored and the adjacent nodes are averaged for a more realistic stress value.

One question: Are you using "smoothed" results, or "unsmoothed"?

Load application nodes (forces, not pressures) and boundary conditions represent theoretically infinite stress (area is theoretically zero, but analytically has value), so you have to apply some engineering judgement.

Hope this helps...

Garland E. Borowski, PE
Engineering Manager
Star Aviation

 

[StevePAA]

Thanks for the help.

I can't post a pic, which would really help, and this is going to be a pain to explain... but more info stated example: round plate, large hole in ctr, three smaller holes (~2") evenly spaced on a diameter about center- so when viewed in "XZ" plane the three smaller holes are at ~12, 4, 8 o'clock. The plate is fixed tx, ty, tz at the hole at 12:00 and ty at the other two- constraints extend out from hole ~.5" radially all around the hole's diameter. Vertical load applied about the large hole in the ctr ~1" radially outside it, all around.

The max stress occurs near the hole at 12:00 and not surprisingly is one node radially outside the last of the constraint nodes. Looking at the view of this hole, The max stress is at ~7:30. Stress is ~5200 and one node away, at same radius from ctr of hole is ~4300. If I go to the mirror image of the max position, ~4:30 the stress values here are more uniform- vary from ~4400-4900 over 6 nodes radially around the hole. The mesh *is* a little "nicer" on this side.

So, it sounds like I need a smaller mesh around the holes to try and get rid of the spike and smooth it out?

Answer to your question: Smooth results. In the option box, the smoothing function is mean and none of the following boxes are checked

 

[GBor]

I'm picturing the end of a pipe flange with three bolts, but the pressure would be uniformally outward, so I'm guessing that isn't quite right, but functionally, it should be similar. Perhaps a buried pipe flange?

You definitely need more elements around the bolt hole. Sounds like you have automeshed a 2-D profile, so I would encourage you to reduce the arc angle to no more than 30 degrees (instead of the default of 60. Personally, considering the simplicity of the example, I would encourage 15 so that you get 24 elements around the perimeter. If bolt holes are an issue, 12 should be an absolute minimum and 18 is preferred (so you could use 20 degrees for the arc angle).

 

[StevePAA]

Gbor: sounds like you're on the right track with my attempt to describe a picture with less than 1000 words. A large "pipe flange", ~15" inner hole, with three ~1.75" "bolt holes" around the inner hole. The 1.75" holes are large enough where I have ~40? elements around them. So, I have enough elements for that. But, around each 1.75" hole there are four .19" holes equally spaced. These have 6 elements around each and are probably contributing to the "problem". The boundary conditions extend past these smaller holes by two elements radially.

The "curvature of edge curve" setting is at 60 degrees. I changed it and ran one at 30 and it didn't really change anything as the max stress area is far enough away where it reverts back to the .12 mesh by then and the mesh is a little funky. Sounds like I'll try refinement points and see how that looks on a future run.

Basically the flange is constrained around the 1.75 holes and lets say the hole's axis is vertical and for the analysis I'm simulating the presence of a 15" inner pipe that applies a load to the flange pulling down on the center portion.

It's actually a 3D part. I initally ran it as a midplane mesh but then later redid it when they changed the part where I needed to incorporate two close holes with nearly intersecting chamfers that they were concerned about (not an issue). I used the same mesh size for each and have 4 elements thru the brick part so the results for both were very similar. IIRC the midplane gave a higher max stress but not by much.