Design Strip For Irregular Flat Slab? 4

[J189]

I have a flat slab with irregular supports. I want the reinforcement to follow the global x & y direction instead of principal moment direction.
So I am thinking having design strips passing each support but I find it very hard to arrange the design strips. Can anyone share your thoughts or if you can, provide your design strips say latitude for this one?

As these short walls have two ends, do I run two design strips through both ends? Can anyone please share some example of this kind of structure?

Thank you.

 

[J189]

Thanks rapt. I used the same method as you mentioned - same bars throughout with extra bars if required.

I am using FEM as I said - SAFE. I am just not sure how it actually works. I know the design strips are used to pick up peak moments and average out them. So doesn't that mean we need to make sure the strips to be arranged in the way that they pass supports so they can capture the peak moments? Can I simply define say 2metres wide strips from start to end regardless the layout of supports? Won't this be unsafe as the strips may not pick up the peak moments?

 

[Retrograde]

I have very little experience with SLABS, but I thought you could run the design without defining any design strips and instead define an "averaging width" that gets used in the reinforcement calcs.

 

[Celt83]

you'll need to get into SAFE's manual but generally with these FEM plate programs if you have design strips covering the slab you will pick up the peak moments.

In general the program will create series of square/triangular plate elements and will solve for the nodal moment values and use things like shape functions for the moment variation across the element. The purpose of the design strip is to say hey program I want you to sum up all of the moments on the elements enclosed by the design strip and then I want you to perform code checks using an effective section width that matches the strip width. Where the averaging comes in is when say you have a design strip that contains elements with both positive and negative moments some programs will take an enveloping approach by taking absolute values and adding them together and then doing the straight combination and giving you section designs for both.

So even though your strip centerline does not run to a wall/column, as long as the width of the strip reaches these elements the potential peak moments in the shell pieces will be included in the total design moment of the strip.

An import thing to remember with these FEM programs like SAFE is that you aren't performing a design using direct design or equivalent frame methods you are infact doing the strip method which may in some instances line up with one of those other methods.

My Personal Open Source Structural Applications:

https://github.com/buddyd16/Structural-Engineering

Open Source Structural GitHub Group:

https://github.com/open-struct-engineer

 

[rapt]

You have to watch out for programs that automatically combine across a design width to make sure they are not doing something stupid.

There was a case I saw several years ago with one well known FEM design program where the moment across the width of the strip at one location varied from significant +ve to significant -ve and the program dutifully summed the moments across the width and the result was 0 (it even showed a similar case in its manual). So the program designed for 0 at that point. I understand that error has since been fixed in that program after the logic error was pointed out so I will not mention its name.

I would not just assume 2m wide strips. It would depend on the spans in both directions and if you have large concentrated loads like a transfer slab. Probably something like .1 to .15 of the smaller span for the strip width, but make sure signs do no change across the strip width.

 

[J189]

Yes, these are meshes for analysis stage only.
This is what I get confused. Take Ram Concept as an example, when you place the 'span segment', does the program read the moments along the span segment only and then divide by the width to get the mean value or does the program adding the moments of the cross sections and then average out them to a mean value for that cross section?
I have done a quick comparison in SAFE as below. Both of the strip are 3 meters wide. The only difference between them the RHS strip is central placed with 1.5meters width on both right and left sides with span while the the 'span segment' of the RHS strip is shifted 0.5meters lower and change the geometry to be 2 meters on right and 1 meters on left. By doing this, the RHS strip span segment will pass supports while the LHS one will not. But their widths are the same and the strips are cover the same area, meaning the analysis will be exactly the same.

So I can check how the design strip average out the peak moments and get the mean values of the design strip. And below is the strip force and the design results that I get. Apparently the design strips are not doing the same job - meaning they don't average out the values of the cross sections, otherwise the results will be the same. Rather, it works like I said, pick up the values along the segments only and divide by the width?. Am I correct or do I miss anything here.

 

[J189]

Rapt, if the design strip is too wide, like you said, if I adopt 2m wide for where transfer loads are, what will happen? The mean values will be lower but does that mean the slab will crack more to find other load path or will be slab fail in strength? where do you get this 0.1 or 0.15 from? Is there any guide that I can have a look for the strip width definition when complex geometry or transfer loads are involved? Or is it purely just engineer judgement?

 

[Celt83]

does the program read the moments along the span segment only and then divide by the width

no the backend solution is a stiffness matrix for all of the nodes of the mesh, the solution to the fundamental equation F=k*d will yield deformation and force results at all of the nodes. The strip then defines the zone over which the results will be summed, area under the curve.

I would have expected your shifted strip to actually yield a higher design moment at the center column as the design would no longer be truncated to the face of the column.

Another thing worth looking into in their manual is how it lays out design sections along a design strip. It could be in your shifted strip the first design section cuts are further away from the column. Unlike a beam/frame program locations of absolute max/min moments and shear aren’t found automatically, instead the program usually relies on cutting design sections on a regular interval.

My Personal Open Source Structural Applications:

https://github.com/buddyd16/Structural-Engineering

Open Source Structural GitHub Group:

https://github.com/open-struct-engineer

 

[Retrograde]

I understand that in SLABS you can do either a strip based or FEM based analysis.

Refer this CSi YouTube video at around the 15:30 mark.

https://www.youtube.com/watch?v=Q86nocpfTIg&list=PLvfsqlqjBW58i-IZCMASzoAVRT05sKqqo&index=7&t=0s

 

[BAretired]

Doing hand calculations, I might consider bands like those shown below. There would be considerable engineering judgment involved. I don't know if this would be suitable for computer analysis.

BA

 

[J189]

Thanks Celt83. Yes. I understand that is how it works at analysis stage. But does this have to do with the strips? I would expect the FEA is run, get the results, and the only thing strips do is to read these results and average out them. ie. Strip will not affect the analysis, they just get the results from the analysis.

If so, why would the design results differ from central stirp to shifted one? I have uploaded the pic as below to further illustrate my confusion.

 

[J189]

SAFE offer this option too but I don't think FEM based can be used for design directly. The peak moments over support have to be average out.

 

[J189]

This is something what I would do too. The question is how to place the span segments, say for the middle one highlighted below? As I mentioned, supports here dont form a ortho direction. If I place the span segment centrally will it capture the peak moments over the supports where are not centrally located? Please refer the example I had above for this.

 

[Celt83]

So in your section A-A it should be reading the negative and positive moment across all of the plates and doing an envelope of summation, note there should be no averaging per se it should be more direct summation, the program I'm familiar with does the summation (really integration) using only the nodal results because the stress results across the element can have localized concentrations. Also it can't be dividing by the width as that wouldn't produce compatible units, moment is units of force*distance if you then divide by distance you'd be left with units of force. The FEM results for a singular line would also be fairly small by comparison.

I'm not overly familiar with SAFE so you will need to review their manual on how it does the enveloping where there are changes of sign across the design segment.

There are really two components there is the design strip and then also a design segment. The design strip defines the effective width, theta angle for your moment and bar orientation. A design segment is your A-A section which will usually occur at each end of a design strip and at some regular interval along the strip.

Here is the output using the program I am familiar with:
Design Strips with the Design segments shown:

Design Moment Envelopes:

Design Moment Envelopes, after assigning the same support width definition to the offset strip:

My Personal Open Source Structural Applications:

https://github.com/buddyd16/Structural-Engineering

Open Source Structural GitHub Group:

https://github.com/open-struct-engineer

 

[BAretired]

For ease in discussion, I have labelled the strips below. The hatched area B-E, 1-3 is going to behave more or less like a two way slab. That area is going to control slab thickness.

This is something what I would do too. The question is how to place the span segments, say for the middle one highlighted below? As I mentioned, supports here dont form a ortho direction. If I place the span segment centrally will it capture the peak moments over the supports where are not centrally located? Please refer the example I had above for this.

I can't say what your program will capture as I have never used it. If you don't know, you should not be using it either. You have highlighted strip D. I would not be at all concerned about how to place the span segments. If your program is indicating a negative moment for strip D where it crosses strip 2, then I would say that your program is wrong. Both of those strips should be carrying positive moment at the crossing point.

I would visualize bottom reinforcement being virtually constant in both directions in the hatched area. If in doubt, beef it up a bit and extend the same reinforcement throughout the entire slab. I would not expect to see top mats on strip 2 at either C or D.

Using a computer to solve this problem is, in my opinion, the wrong approach. Engineering judgment is a much better tool.

BA

 

[Retrograde]

SAFE offer this option too but I don't think FEM based can be used for design directly. The peak moments over support have to be average out.

FEM can be used directly for the design. If you want to average the peak moments over the support just select that option and select an averaging width.

 

[rapt]

J189

Engineering judgement and logic.

It has to be related to span lengths. With 10m spans you would have different strip widths compared to 5m spans. If you do not understand why, look at some moment distributions. Concentrated loads affect it more are there is a sharper drop off in the moment over the width.

Point load effects on one way slabs are normally allowed by some codes at the load point to be spread over .4L if the load is at mid span. I normally halve this to take an average over the span length. Then transverse span length also affects it if it is not a true one way slab, so .1 to .15 L seems logical.

But it all depends on the moment distribution which you can get from your FEM these days.

2m is not logical in a lot of situations.

 

[KootK]

For a highly irregular layout like this, I feel that this excellent suggestion has gone under the radar here for much too long:

As a first step, do some reading on the "method of zero shear" Example Info

The zero shear method is a truly excellent tool for this kind of thing. With FEM, I can't think of any reason why one wouldn't make use of that.

For me, I'm stepping through things like this:

1) Plot the shear contours and locate the lines of zero shear.

2) Ballpark my expectations for top mats using #1, the thing mounted above my shoulders, and assuming some walking lanes for construction personnel.

3) Move into strips and reinforcing having been well informed by #1 & #2.

If somebody steps up with the zero shear diagram, I'll do the same with some strip recommendations.

 

[KootK]

Also useful to have your orthogonal plot zero shear diagrams as well.

 

[r13]

IMO, your primary reinforcement is running N-S, the strips are represented by the red lines. The blue lines represent secondary reinforcement that will be affected by the rigidity of the primary reinforcement. The remaining area can be reinforced by engineering judgement and detailing.

 

[r13]

Add a few torsional element/edge beam (yellow).