Structure with huge displacement

[chen_zhihan_01]

hi can someone help me check whats wrong with this robot model?the displacement values looks really weird

[Krzysztof_Wasik]

Hi @chen_zhihan_01 

Panels  949to961  show excessive displacements. Verify and correct model geometry. Connect those panels with walls

[chen_zhihan_01]

Thank you so much for your help!

I deleted the panels you mentioned (949to961) and re-ran the analysis. The displacement is much better now. But 72 cm still seems too large for a concrete slab.

The remaining warnings are:

• Finite elements with no relation to any panel
• Separate structure
• Instability (type 3) at node 9231

The largest displacement seems to be on the Level 2 slab. Could you advise what to check next?

[Krzysztof_Wasik]

Hi  @chen_zhihan_01 

Columns  471 472 483 543to547  are not connected with slabs (separate structure message) - connect them with slabs to remove this warning.

Refer to video presenting how to identify those columns (https://somup.com/cOjFonVn991)

There are finite elements not assigned to anly panels. They should be deleted to remove - Finite elements with no relation to any panel warning

Such finite elements can be selected as Undefined

Refer to video presenting how to delete them (https://somup.com/cOjFo9VnRc6)

After deleting of thos "orphan" finite elements I would suggest deleting all separate nodes in the model (it is also presented in video)

After model correction (removing all errors) model still shows large deflections from selfweight. In my opinion you should verify geometry and increase number of columns.

Not supported slab segments (working as cantilevers) are too long

[Stephane.kapetanovic]

HI @chen_zhihan_01 

In addition to what  Krzysztof advised, here is a match-check report (on a scale from 0 to 10).

Some panels are still overlapping. I recommend resolving these issues, even if the analysis reports only “Instability Type 3” errors.

Best Regards

pdf report deleted

[chen_zhihan_01]

Hi!

Thank you both for the advice. I tried the following based on your suggestions:

- Deleted the mesh (Local mesh delete), which removed the orphan finite elements and separate nodes
- Disabled "Kinematic constraints in incoherent points" in Job Preferences > Meshing
- Deleted supports, set a user-defined tolerance of 15 mm, regenerated the computational model, then redefined supports

After this, the maximum vertical displacement under self-weight was around -68 cm, concentrated at the curved cantilever slab on the lower levels. The rest of the structure was within a few cm.

I then tried adding columns under the cantilever as suggested. The displacement got worse, it went to around -198 cm. The new columns have supports at their base and the number of $SUB$ groups did not increase, so they appear to be connected.

The "Separate structure" warning is also still present and I have not managed to resolve it.

What would cause added columns to increase deflection instead of reducing it? Is there anything else you would suggest checking for this model?

Thanks again.

[Krzysztof_Wasik]

Hi @chen_zhihan_01 

Open Loads >Load table and delete all selfweight records except of one. You have multiplied selfweight load

[chen_zhihan_01]

Hi, thank you so much for your help!