Discussion: View Thread

Hello

The last few weeks, I deal with the slab of a METRO station. It is a rectangular reinforced concrete slab of dimensions 110mx26m.
The thickness of the slab varies from 0.6m to 1.0m. The slab will be simply connected to the perimetric diaphragm walls via dowels.
No interior vertical elements will exist. In the interior, rc beams of 2.00x1.60m (bxd) along the smallest dimension have been placed (span 26m).
Initially the point of interest is the beams.  
Two calculations have been made.

In the first calculation, the structure was modeled with surface finite elements of appropriate thickness. Even the beams were modeled with fin. elem. having the corresponding thickness.The software that was used was Sofistik.  

The purpose of the second calculation was to check the computer results.  This was a traditional hand calculation. The beams together with various holes and openings in the slab 'panelised' the slab. Each panel was treated then as a separate slab with the appropriate support conditions. Using Czerny tables, the reactions from each panel were calculated and assigned to the corresponding supporting beam. The beam was then calculated as a simply supported beam acted upon by the said reactions. This calculation is typical for conventional buildings and has been used for many years.

The difference in the beam span moment between the two calculations was more than 50%.  The fem analysis showed that in fact the slab is not panelised and behaves like a one way slab thus carrying a large portion of the load and therefore relieving the beams. The hand calculation was more unfavorable for the beams.

Which calculation is correct? Should the fem results be trusted?



------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------

Dikaios,

While I couldn't be sure without seeing your model, it sounds as though the beams in your finite element model are not behaving as rigidly as they should be. How have you physically modeled the beam webs in your model? What is the center-to-center spacing of the beams? Also, have you modeled the connection between the slab and the perimeter walls as pinned connections distributed around the entire perimeter of the slab, or have you modeled the supports between the slab and the walls discretely at the point where the the beams intersect the wall?

------------------------------
Jason Draper P.E., M.ASCE
Burns & McDonnell
Kansas City MO
------------------------------

Original Message:
Sent: 06-11-2017 13:32
From: Dikaios Psarogiannis
Subject: finite element analysis of slab vs traditional hand calculation

Hello

The last few weeks, I deal with the slab of a METRO station. It is a rectangular reinforced concrete slab of dimensions 110mx26m.
The thickness of the slab varies from 0.6m to 1.0m. The slab will be simply connected to the perimetric diaphragm walls via dowels.
No interior vertical elements will exist. In the interior, rc beams of 2.00x1.60m (bxd) along the smallest dimension have been placed (span 26m).
Initially the point of interest is the beams.  
Two calculations have been made.

In the first calculation, the structure was modeled with surface finite elements of appropriate thickness. Even the beams were modeled with fin. elem. having the corresponding thickness.The software that was used was Sofistik.  

The purpose of the second calculation was to check the computer results.  This was a traditional hand calculation. The beams together with various holes and openings in the slab 'panelised' the slab. Each panel was treated then as a separate slab with the appropriate support conditions. Using Czerny tables, the reactions from each panel were calculated and assigned to the corresponding supporting beam. The beam was then calculated as a simply supported beam acted upon by the said reactions. This calculation is typical for conventional buildings and has been used for many years.

The difference in the beam span moment between the two calculations was more than 50%.  The fem analysis showed that in fact the slab is not panelised and behaves like a one way slab thus carrying a large portion of the load and therefore relieving the beams. The hand calculation was more unfavorable for the beams.

Which calculation is correct? Should the fem results be trusted?



------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------

Thanks to all for your reply

After your replies and a closer look to my calculations, I believe that is a matter of relative stiffness.
The hand calculation is based on Czerny tables. These tables assume rigid supports. For this assumption to be valid, the beams should be much stiffer than the slab. Apparently this does not happen in my case. 


To Mr Jason Draper: The model is supported by pin supports uniformly distributed around the perimeter. At the area of the webs, the elements  thickness equals the web height. All the elements are surface elements and their mid surface of all lies on the same plane (e.g. there are no eccentricities).




------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------

Original Message:
Sent: 06-13-2017 00:50
From: Jason Draper
Subject: finite element analysis of slab vs traditional hand calculation

Dikaios,

While I couldn't be sure without seeing your model, it sounds as though the beams in your finite element model are not behaving as rigidly as they should be. How have you physically modeled the beam webs in your model? What is the center-to-center spacing of the beams? Also, have you modeled the connection between the slab and the perimeter walls as pinned connections distributed around the entire perimeter of the slab, or have you modeled the supports between the slab and the walls discretely at the point where the the beams intersect the wall?

------------------------------
Jason Draper P.E., M.ASCE
Burns & McDonnell
Kansas City MO
------------------------------

Original Message:
Sent: 06-11-2017 13:32
From: Dikaios Psarogiannis
Subject: finite element analysis of slab vs traditional hand calculation

Hello

The last few weeks, I deal with the slab of a METRO station. It is a rectangular reinforced concrete slab of dimensions 110mx26m.
The thickness of the slab varies from 0.6m to 1.0m. The slab will be simply connected to the perimetric diaphragm walls via dowels.
No interior vertical elements will exist. In the interior, rc beams of 2.00x1.60m (bxd) along the smallest dimension have been placed (span 26m).
Initially the point of interest is the beams.  
Two calculations have been made.

In the first calculation, the structure was modeled with surface finite elements of appropriate thickness. Even the beams were modeled with fin. elem. having the corresponding thickness.The software that was used was Sofistik.  

The purpose of the second calculation was to check the computer results.  This was a traditional hand calculation. The beams together with various holes and openings in the slab 'panelised' the slab. Each panel was treated then as a separate slab with the appropriate support conditions. Using Czerny tables, the reactions from each panel were calculated and assigned to the corresponding supporting beam. The beam was then calculated as a simply supported beam acted upon by the said reactions. This calculation is typical for conventional buildings and has been used for many years.

The difference in the beam span moment between the two calculations was more than 50%.  The fem analysis showed that in fact the slab is not panelised and behaves like a one way slab thus carrying a large portion of the load and therefore relieving the beams. The hand calculation was more unfavorable for the beams.

Which calculation is correct? Should the fem results be trusted?



------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------

What is the spacing of the beams? If the beams are regularly spaced I would normally analyze a structure of this type as continuous multi-span one-way slabs supported by simply-supported T-beams.

Do the slabs vary in thickness because the slab spans vary? If you can, make the slab spans equal and maintain a constant slab thickness.

The depth of the beams is shallow for the span, just barely above the threshold of L/16 in the ACI code where you need to start investigating deflection. Since the FEM analysis is based on stiffness of both the slabs and beams, the low stiffness of the beams causes them to carry less load than the hand calculation suggests. This is why your hand calculations proved more unfavorable for the beams.     

Both the hand-calculations and the FEM analysis are likely valid. The FEM analysis is likely more accurate given the low stiffness of the beams. If you proceed by using the FEM analysis, make sure you reinforce the slab as a two-way slab and not provide just temperature and shrinkage steel in the 26m direction.

------------------------------
Kelly Covert, P.E., M.ASCE
Principal - Klepper Hahn & Hyatt
East Syracuse, NY USA
------------------------------

Original Message:
Sent: 06-11-2017 13:32
From: Dikaios Psarogiannis
Subject: finite element analysis of slab vs traditional hand calculation

Hello

The last few weeks, I deal with the slab of a METRO station. It is a rectangular reinforced concrete slab of dimensions 110mx26m.
The thickness of the slab varies from 0.6m to 1.0m. The slab will be simply connected to the perimetric diaphragm walls via dowels.
No interior vertical elements will exist. In the interior, rc beams of 2.00x1.60m (bxd) along the smallest dimension have been placed (span 26m).
Initially the point of interest is the beams.  
Two calculations have been made.

In the first calculation, the structure was modeled with surface finite elements of appropriate thickness. Even the beams were modeled with fin. elem. having the corresponding thickness.The software that was used was Sofistik.  

The purpose of the second calculation was to check the computer results.  This was a traditional hand calculation. The beams together with various holes and openings in the slab 'panelised' the slab. Each panel was treated then as a separate slab with the appropriate support conditions. Using Czerny tables, the reactions from each panel were calculated and assigned to the corresponding supporting beam. The beam was then calculated as a simply supported beam acted upon by the said reactions. This calculation is typical for conventional buildings and has been used for many years.

The difference in the beam span moment between the two calculations was more than 50%.  The fem analysis showed that in fact the slab is not panelised and behaves like a one way slab thus carrying a large portion of the load and therefore relieving the beams. The hand calculation was more unfavorable for the beams.

Which calculation is correct? Should the fem results be trusted?



------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------

The difference between traditional hand calculations and FEM for concrete comes down to behavior.  The older calculations used methods of moment redistribution due to slab cracking behavior.  These crack will form due to initial temperature and shrinkage, thermal loading strain, subgrade and structure settlement, and applied loading.  Most FEM will follow elastic behavior of the material and thin panels will produce large amount of in-plane rigidity that does not match the placed material due to installation defects, thickness variations, and reinforcement placement.  The prudent plan at this juncture could be to follow the hand calculations for the beams since they have accounted for the reductions in stiffness for the slab, and to design the slab thickness and reinforcement from the FEM since load moves toward stiffness in a model and if modeled correctly the idealized slab would carry a larger load than would be redistributed under cracking.

If you wish to perfect the FEM, methods would be needed to locally reduce the thickness of the slab at nodes to create a section with the cracked area (Acr) and the cracked section moment of inertial (Icr).  This is a labor intensive iterative method that requires a large amount of book keeping and may not yield results that are much different for using both approaches and selecting the most conservative for each element.  It starts to follow the adage written by George Box, "all models are wrong, but some are useful."

------------------------------
Christopher Lamar P.E., M.ASCE
EN Engineering
Chicago IL
------------------------------

Original Message:
Sent: 06-11-2017 13:32
From: Dikaios Psarogiannis
Subject: finite element analysis of slab vs traditional hand calculation

Hello

The last few weeks, I deal with the slab of a METRO station. It is a rectangular reinforced concrete slab of dimensions 110mx26m.
The thickness of the slab varies from 0.6m to 1.0m. The slab will be simply connected to the perimetric diaphragm walls via dowels.
No interior vertical elements will exist. In the interior, rc beams of 2.00x1.60m (bxd) along the smallest dimension have been placed (span 26m).
Initially the point of interest is the beams.  
Two calculations have been made.

In the first calculation, the structure was modeled with surface finite elements of appropriate thickness. Even the beams were modeled with fin. elem. having the corresponding thickness.The software that was used was Sofistik.  

The purpose of the second calculation was to check the computer results.  This was a traditional hand calculation. The beams together with various holes and openings in the slab 'panelised' the slab. Each panel was treated then as a separate slab with the appropriate support conditions. Using Czerny tables, the reactions from each panel were calculated and assigned to the corresponding supporting beam. The beam was then calculated as a simply supported beam acted upon by the said reactions. This calculation is typical for conventional buildings and has been used for many years.

The difference in the beam span moment between the two calculations was more than 50%.  The fem analysis showed that in fact the slab is not panelised and behaves like a one way slab thus carrying a large portion of the load and therefore relieving the beams. The hand calculation was more unfavorable for the beams.

Which calculation is correct? Should the fem results be trusted?



------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------

Hello
Based on some analytical research I have done a while ago comparing traditional manual methods and finite element results for slab analysis, I found that in order for the slab to behave similar to the manual assumptions and hence the beams to carry loads close to hand calculations, the beam depth shall be 4 times the thickness of slab. If the beam depth is less than that, beams act proportionally as ribs in the slab which makes the slab to act as an orthotropic deck. If the beam and slab depths are equal, i.e., embedded beams, then the beams carry no load, almost.

Thanks.

------------------------------
Sayed Attaalla Ph.D., P.E., S.E., M.ASCE
Vice President
Peter T. Erdelyi & Associates, Inc.
Los Angeles CA
------------------------------

Original Message:
Sent: 06-11-2017 13:32
From: Dikaios Psarogiannis
Subject: finite element analysis of slab vs traditional hand calculation

Hello

The last few weeks, I deal with the slab of a METRO station. It is a rectangular reinforced concrete slab of dimensions 110mx26m.
The thickness of the slab varies from 0.6m to 1.0m. The slab will be simply connected to the perimetric diaphragm walls via dowels.
No interior vertical elements will exist. In the interior, rc beams of 2.00x1.60m (bxd) along the smallest dimension have been placed (span 26m).
Initially the point of interest is the beams.  
Two calculations have been made.

In the first calculation, the structure was modeled with surface finite elements of appropriate thickness. Even the beams were modeled with fin. elem. having the corresponding thickness.The software that was used was Sofistik.  

The purpose of the second calculation was to check the computer results.  This was a traditional hand calculation. The beams together with various holes and openings in the slab 'panelised' the slab. Each panel was treated then as a separate slab with the appropriate support conditions. Using Czerny tables, the reactions from each panel were calculated and assigned to the corresponding supporting beam. The beam was then calculated as a simply supported beam acted upon by the said reactions. This calculation is typical for conventional buildings and has been used for many years.

The difference in the beam span moment between the two calculations was more than 50%.  The fem analysis showed that in fact the slab is not panelised and behaves like a one way slab thus carrying a large portion of the load and therefore relieving the beams. The hand calculation was more unfavorable for the beams.

Which calculation is correct? Should the fem results be trusted?



------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------

You may wish to look at the relative stiffnesses using the cracked sections.  Research in the 1980s ( I know it is a long time ago) indicated that in a restrained condition that the modulus of rupture could reduced by up to half by creep and shrinkage,  You can estimate a ratio of effective stiffness to the gross stiffness and apply it to your model.  It will likely show the slab elements to be softer compared to the beam elements.


------------------------------
David Thompson P.E., M.ASCE
Principal
KTA Structural Engineers Ltd.
Calgary AB
------------------------------

Original Message:
Sent: 06-11-2017 13:32
From: Dikaios Psarogiannis
Subject: finite element analysis of slab vs traditional hand calculation

Hello

The last few weeks, I deal with the slab of a METRO station. It is a rectangular reinforced concrete slab of dimensions 110mx26m.
The thickness of the slab varies from 0.6m to 1.0m. The slab will be simply connected to the perimetric diaphragm walls via dowels.
No interior vertical elements will exist. In the interior, rc beams of 2.00x1.60m (bxd) along the smallest dimension have been placed (span 26m).
Initially the point of interest is the beams.  
Two calculations have been made.

In the first calculation, the structure was modeled with surface finite elements of appropriate thickness. Even the beams were modeled with fin. elem. having the corresponding thickness.The software that was used was Sofistik.  

The purpose of the second calculation was to check the computer results.  This was a traditional hand calculation. The beams together with various holes and openings in the slab 'panelised' the slab. Each panel was treated then as a separate slab with the appropriate support conditions. Using Czerny tables, the reactions from each panel were calculated and assigned to the corresponding supporting beam. The beam was then calculated as a simply supported beam acted upon by the said reactions. This calculation is typical for conventional buildings and has been used for many years.

The difference in the beam span moment between the two calculations was more than 50%.  The fem analysis showed that in fact the slab is not panelised and behaves like a one way slab thus carrying a large portion of the load and therefore relieving the beams. The hand calculation was more unfavorable for the beams.

Which calculation is correct? Should the fem results be trusted?



------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------

I'm not surprised that your FEM is showing quite a bit of the load being carried in one way slab action.  The reason for this is that the depth of the slab is close (in structural terms) to the depth of the beams.  From the information given, the slab is approximately 2/3 the depth of the beams, so I would expect to see that the slab would carry about 1/3 of the load or so (very rough estimate) and the beams about 2/3, depending on the spacing of the beams and the reinforcing of both the slab and beam.  As others have said, look at the assumptions made in the hand calculations and the relative stiffness of the slab and beams.  That is the key to understanding the results you are getting.

------------------------------
Andrew Holmes P.E., L.S., M.ASCE
Consulting Engineer
Melbourne FL
------------------------------

Original Message:
Sent: 06-14-2017 22:11
From: David Thompson
Subject: finite element analysis of slab vs traditional hand calculation

You may wish to look at the relative stiffnesses using the cracked sections.  Research in the 1980s ( I know it is a long time ago) indicated that in a restrained condition that the modulus of rupture could reduced by up to half by creep and shrinkage,  You can estimate a ratio of effective stiffness to the gross stiffness and apply it to your model.  It will likely show the slab elements to be softer compared to the beam elements.


------------------------------
David Thompson P.E., M.ASCE
Principal
KTA Structural Engineers Ltd.
Calgary AB
------------------------------

Original Message:
Sent: 06-11-2017 13:32
From: Dikaios Psarogiannis
Subject: finite element analysis of slab vs traditional hand calculation

Hello

The last few weeks, I deal with the slab of a METRO station. It is a rectangular reinforced concrete slab of dimensions 110mx26m.
The thickness of the slab varies from 0.6m to 1.0m. The slab will be simply connected to the perimetric diaphragm walls via dowels.
No interior vertical elements will exist. In the interior, rc beams of 2.00x1.60m (bxd) along the smallest dimension have been placed (span 26m).
Initially the point of interest is the beams.  
Two calculations have been made.

In the first calculation, the structure was modeled with surface finite elements of appropriate thickness. Even the beams were modeled with fin. elem. having the corresponding thickness.The software that was used was Sofistik.  

The purpose of the second calculation was to check the computer results.  This was a traditional hand calculation. The beams together with various holes and openings in the slab 'panelised' the slab. Each panel was treated then as a separate slab with the appropriate support conditions. Using Czerny tables, the reactions from each panel were calculated and assigned to the corresponding supporting beam. The beam was then calculated as a simply supported beam acted upon by the said reactions. This calculation is typical for conventional buildings and has been used for many years.

The difference in the beam span moment between the two calculations was more than 50%.  The fem analysis showed that in fact the slab is not panelised and behaves like a one way slab thus carrying a large portion of the load and therefore relieving the beams. The hand calculation was more unfavorable for the beams.

Which calculation is correct? Should the fem results be trusted?



------------------------------
Dikaios Psarogiannis A.M.ASCE
Consulting Engineer
OMETE SA
Holargos
------------------------------