The equilibrium doesn’t check between panels!!!

[brhm]

We discovered on the table “Reduced results for panels” that two panels have different values on a common edge!

We made a test with a very simple model (described below) and we got the same problem.

We hope AutuDesk can help us.
The subject is very important for our current project and we don’t have so much time…

Thank you.

Our test (see the attached picture):
The structure is a beam with a section of 25x70cm and 5m length. There are two pinned supports at each end and the last is 5kN/m. The table of results shows the total forces in 6 vertical sections along the beam. The sections are denoted by the node numbers.
In the table the first and last row shows the common line between the panels and should be (at least) similar.

Look at the shear force TRy: 9,54kN one side and -13,79kN the other side. The correct value should be 3,125kN !!!! HELP

PD. IF THE FORUM IS ABOUT RSA WHY WE CAN NOT ATTACH RSA FILES?????

[rbruins]

We discovered on the table “Reduced results for panels” that two panels have different values on a common edge!

We made a test with a very simple model (described below) and we got the same problem.

We hope AutuDesk can help us.
The subject is very important for our current project and we don’t have so much time…

Thank you.

Our test (see the attached picture):
The structure is a beam with a section of 25x70cm and 5m length. There are two pinned supports at each end and the last is 5kN/m. The table of results shows the total forces in 6 vertical sections along the beam. The sections are denoted by the node numbers.
In the table the first and last row shows the common line between the panels and should be (at least) similar.

Look at the shear force TRy: 9,54kN one side and -13,79kN the other side. The correct value should be 3,125kN !!!! HELP

PD. IF THE FORUM IS ABOUT RSA WHY WE CAN NOT ATTACH RSA FILES?????

I've made the same test,
a 3d shell type with two different loadlocations, and 3 meshdensities (,35m ,175m and 0,05m) The supports have been modified to even-out the Nxy force at the supports. I've also made panelcuts at mid-span and at quarterspan. Panel 17 and 23 have the same properties as the test you've made.

First of all, the mesh density of .35m is too large and gives an integral value of 2,68kN at Mid-span independent of application height. And reaches 3.06kN at the finest meshdensity. Which is normal as UDL is applied nodally and will also be applied to the neighboring element.

the total nodal force should be mesh * 5 / 2. And is transfered over two element thus giving"

Meshdensity: 0.35 = > F = (0.35 * 5 / 2) /2 = 0.4375 => 3.125-.4375 = 2.6875 kN
Meshdensity: 0.175 = > F = (0.175 * 5 / 2) /2 = 0.21875 => 3.125-.4375 = 2.90625 kN
Meshdensity: 0.05 = > F = (0.05 * 5 / 2) /2 = 0.0625 => 3.125-.4375 = 3.0625 kN

Furthermore the reduced results are not averaged! (as the panelcuts are (globally)). For 17 and 23 this gives (-2.23+-3.13)/2 = 2.68kN, which gives the same result.

Compared to your test, the same thing happens. As (+9.54 + - 13.79)/2 = -2.13kN which is the same value as the integral value found in your model!

The big difference between the test is that I use as 3d shell that you use a 2d Compression panel. Thus the only thing you can to is try the same thing and use a 3d-shell.

Good Luck!

[brhm]

I see...very interesting...

I would like a formal "doucumentation" about all this from AutoDesk...

rubins, thank you very much!

About your sugestion: We have a big project and we are using already 2D-plates.
It is too late for switching into a 3D elements...

[rbruins]

I see...very interesting...

I would like a formal "doucumentation" about all this from AutoDesk...

rubins, thank you very much!

About your sugestion: We have a big project and we are using already 2D-plates.
It is too late for switching into a 3D elements...

There is no need for Formal documentation on this subject.
I've had a look in my FEM - book and what happens is called spurious shear strain!
This is also known as shearlocking!
The 4 node planestress element doesn't have the posibilty of discribing constant shear when being forced in bending! And this happens in your test.

See also :
http://ocw.mit.edu/NR/rdonlyres/Mechanical-Engineering/2-094Spring-2008/B90A4FF0-6958-47E6-957A-FA8204FB331E/0/lec19.pdf

And made visible with the attachements (One is a shell element, the other the planestress version!)

This is why you should always take care in chosing the correct element type when using FEM!

[O75steve]

Hi,

A question on the first reply of RBruins : how do you make a panel cut to apply only to a certain panel, and not to all the panels it would normally cut through ?

Also, what does the option "Reduction of forces above columns and walls" under Panel Cuts / Parameters exactly do ?

And lastly, in RSA 2011, when selecting Diagram Analysis under Panel Cuts / Cuts , nothing happens in my model. Is this an error of the new version ?

Thanks for any answers in advance,

Steven