HELP - Results Yielding Negative Modal Period(s) 1

[Bjorn_Steinhagen]

Hi There,

I was hoping to get some help on an issue that has just popped up on a model I'm currently working on. The issue is best summarized by the mark-up attached. If anyone has some insight into a possible fix please let me know!

Thanks in advance.

 

[Trenno]

Hi Bjorn,

As a starting point for a 92m tall building, you're probably expecting a frequency of around H/46 (2 sec) or # floors/10 = 24/10 = 2.4 sec. Assuming the 5th mode is correct and your proper fundamental mode, then you're in the upper bounds but still in the ballpark.

How are you applying wind or seismic loads? Do you have semi-rigid diaphragms assigned? Are you getting the program to calculate centre of mass and rigidity?

ETABS applies wind/seismic loads to diaphragms by sharing the total load at each floor amongst 5 joints present on that diaphragm. ETABS might be creating these ghost joints during this process.

Also, if you are using user-defined wind/seismic loads, the location that you specify within the Load Pattern dialogue will create a joint at that location. This joint isn't technically a joint on the model, but ETABS creates this joint internally so as to apply the point load.

 

[Agent666]

Check the analysis log, is it saying the structure is ill conditioned or unstable?

 

[Bjorn_Steinhagen]

Trenno

Thanks for the response!

The wind loads were User Defined and the location I specified was refined so as to not occur somewhere 'off' the diapraghm on the roof level - thanks for that suggestion! However, the negative period still exists. The diaphragms are semi-rigid and I am not getting the program to calculate the centre of mass and rigidity (found when going Analyze > Set Load Cases to Run > Calculate Diaphragm Centers of Rigidity - correct?)

The seismic loading is an auto lateral load based on the code I am working with.

In summary, I am still getting the error but I appreciate the feedback, my understanding has grown that much more.

Agent666

No, it isn't saying the structure is ill conditioned or unstable.



Any other recommendations or advice?

 

[Agent666]

The way you apply the loads at a single point by the sounds of it is the wrong way to do it with semi-rigid diaphragm. You just end up deforming your diaphragm locally and not distributing the load correctly (more load goes to elements closer to the point the load was applied to.

Try the standard solver, it gives more info on instabilities, does this say anything regarding loss of accuracy or similar?

Additionally have you reviewed the mode shape for the negative modes, is it some isolated part of the structure flapping about that is unstable or has massive deflections that would indicate some issues.

If you change to a rigid diaphragm, does the same thing occur.

What about the check model function, anything useful there?

 

[Trenno]

I think this ties in with my thread earlier in the year.

Do you need to set up two different diaphragms for the roof level?

Have you somehow set the roof levels to be similar to the typical floors - so it's trying to apply the seismic load at the COM of the floor below?

I'm almost certain this joint is being generated as a part of the auto/user loading routine. You need to figure out why ETABS wants to apply the load at this location.

[URL unfurl="true"]https://www.eng-tips.com/viewthread.cfm?qid=449130[/url]

 

[Trenno]

As a side note - a negative period/frequency indicates the mode shape if the modal mass/loading was in the opposite direction. It's not fundamentally incorrect or invalid.

 

[Bjorn_Steinhagen]

Agent666:

Tried running the standard solver. Looking at the log there is some substantial lost accuracy at specific joint (ID ~73750) but can't find that joint anywhere so must be an ETABS created pointed? Extract from the run log below:

* * * W A R N I N G * * *
NUMERICAL PROBLEMS ENCOUNTERED DURING EQUATION SOLUTION:

TYPE LABEL DOF X-COORD Y-COORD Z-COORD PROBLEM VALUE
----- ------- -- ----------- ----------- ----------- ------------- -----------
Joint ~73750 UY 8180.000 7690.000 43300.000 Lost accuracy 6.8 digits
Joint ~73750 UY 8180.000 7690.000 43300.000 Diagonal < 0 -0.213742
Block 3 by block 2
Block 3 by block 3
Block 4 by block 3
Block 4 by block 4
Block 5 by block 4
Block 5 by block 5
Block 6 by block 5
Block 6 by block 6
Block 7 by block 1
Block 7 by block 2
Block 7 by block 3
Block 7 by block 4
Block 7 by block 5
Block 7 by block 6
Block 7 by block 7

* * * W A R N I N G * * *
NUMERICAL PROBLEMS ENCOUNTERED DURING EQUATION SOLUTION:

TYPE LABEL DOF X-COORD Y-COORD Z-COORD PROBLEM VALUE
----- ------- -- ----------- ----------- ----------- ------------- -----------
Cnstr 17 R3 13791.550 9312.227 43300.000 Lost accuracy 6.7 digits

---------------------------------
BASIC STABILITY CHECK FOR LINEAR LOAD CASES:
NUMBER OF NEGATIVE STIFFNESS EIGENVALUES SHOULD BE ZERO FOR STABILITY.
(NOTE: FURTHER CHECKS SHOULD BE CONSIDERED AS DEEMED NECESSARY,
SUCH AS REVIEWING EIGEN MODES FOR MECHANISMS AND RIGID-BODY MOTION)

NUMBER OF NEGATIVE EIGENVALUES = 1

* * * W A R N I N G * * *
THE STRUCTURE IS UNSTABLE OR ILL-CONDITIONED !!
CHECK THE STRUCTURE CAREFULLY FOR:
- INADEQUATE SUPPORT CONDITIONS, OR
- ONE OR MORE INTERNAL MECHANISMS, OR
- ZERO OR NEGATIVE STIFFNESS PROPERTIES, OR
- EXTREMELY LARGE STIFFNESS PROPERTIES, OR
- BUCKLING DUE TO P-DELTA OR GEOMETRIC NONLINEARITY, OR
- A FREQUENCY SHIFT (IF ANY) ONTO A NATURAL FREQUENCY

 

[Bjorn_Steinhagen]

Trenno

Thanks for linking in that thread from earlier on, very useful reading and good to know going forward! What is strange is that the wind loading hasn't changed for a long time but the negative period issue is very recent so I'm skeptical that it is that.

Roof levels not similar to any other levels, maybe worthwhile investigating assigning two diaphragms like you suggested

Thanks

 

[Trenno]

"~" before a joint label means it was created during the meshing or load generation routines. That's why you can't select it as it's like a pseudo joint.

I also note that the offending joint isn't at the roof level like you initially suspected.

Does this location fall within an opening zone? Is it very close to another joint or object? Do you have edge constraints turned on for walls and floors?

 

[Agent666]

Did you try the other suggestions I had to find the source of the instability?

 

[Bjorn_Steinhagen]

Agent666:

Yes, I did try the other suggestions. Reviewing the animations for the negative shape mode didn't show any 'loose' elements or elements flapping around. Also, changing diaphragms to rigid didn't make a difference. In good news, only down to one negative shape mode now

 

[Agent666]

That's a falsity though given your model is still ill conditioned amd not actually solving. Try excluding the wind case (or apply the load not as a point load (refer to suggestions in the thread trenno linked to)), does it solve then without the ill conditioned error?

Also temporarily removing any pinned end releases, or increasing section sizes, do these have any effect. Sometimes with pinned beams, it results in column spinning if you have a torsional pin at the base. I tend to just start throwing massive changes at the model one at a time until you discover or narrow down the issue.

Anything noted in the check model function?

 

[Bjorn_Steinhagen]

Nothing noted in the model function.

I have nonetheless figured out the issue! Thank you Agent666 and Trenno for pointing me to the run log to locate the error. It was an ill condition associated with edge releases assigned to a slab that was assigned and I wasn't aware of the changes (see picture below)

.

Thanks all for the help! Appreciate all the suggestions and have definitely learnt a lot which is never wasted time.