Results comparison

[40818]

Thought i'd throw a question out there:

If you have a coarse grid model of say 9 Quad4 elements in a 3 rows of 3 columns (Nastran) and apply a load to the model to generate shears and endloads within the quads. And then use hand calcs to size the panels, all well and good.
If a finer grid model of say 81 Quad4 elements in a 9x9 similar group (so 9 elements take the place of the original element) and apply the same loading. How is the best way to compare the results of the new model against the old.
So if the original quad had 10N/mm shear flow, how do you compare (combine?) the new more detailed elements back to the original.
Hope that makes sense.

 

[rb1957]

results from a quad are good at its centroid, then the centroid of the 1st of 3 quads would be at the same location as the centroid of the 2nd of 9 quads. this would be the same as plotting element results against element centroid.

clear as mud, no!?

 

[EdR]

40818:

I would plot the results (whatever you are interested in displ, and or stress components) for each mesh vs. position ( an x-y plot) and see how the plotted data overlays...You know that (assuming both models are correctly put together and solved) the finer mesh will have better results and you should be able to get a reasonable estimate of the correlation between the meshs......I also think this would give a better picture of what is going on than rb's method....

Ed.R.

 

[40818]

Thenaks for the replies.
I ran 2 quick models today, and was going to upload the details, but typically i forgot, will do it tomorrow.
However, basically i had the 3x3 grid and applied a transverse load at teh top of the sqaure, and contrained at the bottom of the sqaure. As would be expected the centre quad conatined only shear (around 23N/mm) and no endloads. The same loading etc applied to a 9x9 square grid and once again the (smaller) centre grid contains only shear, but the magnitude is just over double (around 58N/mm).
Plotting the shear across the centre line of the square grid it can be seen that the more detailed plot (9 elements across) is trying to form a parabola, where as the coarse grid (3 elements across) is only able to form a pointy 2 line shape.
The mangitude of difference however was a bit of a surprise

 

[EdR]

40818:

Sounds like you are seeing a behaviour similar to beam shear across a beam cross section....The 3x3 is trying to show the average shear across the section while the 9x9 is showing a much more realistic set of shear values....If you think of a beam shear situation the average shear values times 1.5 are the max values of the actual parabolic shear values (for rectangular x-sections).....given that your section is probably more like a deep beam I suspect that double is not too bad a value (you could probably check a deep beam solution in a handbook for a better estimate of the values).....

Ed.R.

 

[GBor]

Now run an 81x81 element version and see what happens. You could still be converging. As you said,

Plotting the shear across the centre line of the square grid it can be seen that the more detailed plot (9 elements across) is trying to form a parabola, where as the coarse grid (3 elements across) is only able to form a pointy 2 line shape.

This tells me you haven't converged yet. Depending on the magnitude compared to your overall size of the model, 2x may not be unexpected.

You should also be able to do a hand calculation of this situation.

 

[40818]

I was on my way into work today when i realised something about the runs. I had applied the load onto the surface edge for the original coarse mesh. I simply deleted the mesh and created a finer one for the second run. I didn't however change the loading, so it was 2.5 times the original (and as it wasn't work stuff and i was busy i didn't recheck the second f.06 (what a muppet!)). The penny dropped this morning and i re-ran with identical loading and the pure shear in the centre element matched to within 2.5% so i would think that firstly RB1957 method works for this instance, but comparison between other centre elements around the periphery shows a slightly greater discrepancy, more so with the endloads rather than the pure shear.
I have uploaded a wordpad file which contains BOTH input decks, so if your interested then you would have to just copy out the separate parts before using.

 

[hondaknight1]

I have to agree with GBor, the problem could still be converging. This is a feature of plate elements, and is normally used as a method to teach students about accuracy. If you did this as a single element it would not be accurate, and you should not expect it to be. The important thing to be aware of is that most plate element formulations converge on mesh size from below, ie they show an error which gives less displacement than would be expected from hand calcs, typically -10% for a 1x1 mesh of a simply supported plate with a concentrated vertical load. Conversely some converge from above, they show more displacement than would be expected. These can give typically +15% displacement for a 1x1 grid, which is a greater error but at least its conservative. Just remember to always do a mesh convergence study to validate your results. You should be able to find out more about your element formulation from the software literature. Its also a good example about how you need to be careful when comparing results from different software producers. They use differing element formulations which converge in different ways, and its instructive to note which codes use elements that converge from a conservative postion and which converge from below. Then its question of which is more likely to give you a warm feeling....