Irregular shaped manual floor mesh

[radiocontrolhead]

Long time lurker, first time poster.

I am trying to understand the idea behind a floor mesh and how to generate a reasonable one in etabs manually. I am trying to achieve proper connectivity between the slab and walls and find it to be difficult when the slabs are to be modeled with intentions of capturing in plane forces/deformations (semi-rigid). The modeling procedure at my current workplace is to assume the slab as a "null" shell element and to add an additional mass to this shell where only the lateral resisting elements will be considered. I have since realized it is a very barebones approach to yield preliminary results and may not account for all conditions as described below for this project. I find that I have to apply a line load above walls to account for vertical loads, and to divide these shells so that connectivity is achieved between wall and slab, and then further refine the mesh in the horizontal direction. it's essentially a backdoor approach. Wanted to hear what others thought of this? Slabs are designed using a different slab design software, say, Ram Concept.

Project Info:

approximately 10" thick conventional slab with a large opening in the centeral region for a pool and spa. These will be supported on grade but the perimeter walls are essentially retaining walls, designed separately. The northern slab edge is supported by a 13' retaining wall that supports a surcharge of a 3 story wood framed structure above it. The idea is that this slab acts as a pool deck for the wood structure at the slab level.

Few questions:

1) are there any guidelines to producing a mesh to achieve connectivity between the walls and slab? The automesh feature in Etabs just doesn't produce results that I am looking for mainly due to the irregularity.
2) Based on the mesh I have generated (attached), will I need to model each individual plate for the slab or is there an easier way to have etabs break the slab into these segments based on an uploaded DXF file?
3) Is this far more work than is absolutely required and am I overthinking this design?
4) Depending on the connection between the top of the northern retaining wall and slab (say pinned and not allowed to slip), is it reasonable to assume that the core walls surrounding the pool will be the primary resisting elements in providing an "at-rest" retaining wall condition?
4) I understand I can account for the opening by treating it as a deep beam using a simple beam analogy, but if i wanted etabs to calcualtie these in plane stresses i would need to model as "semi-rigid" with a manually generated mesh presented above?
5) Just for giggles, how would you treat a design as such? I am only trying to pick the brains of other engineers and their approach to this problem.

I really appreciate everyones time with this. Although this may or may not be(depending on responses) an overkill approach, I will use it as an exercise to understand the underlying concepts for future projects.

 

[Trenno]

I'll have a crack.

1) Make sure to have 'edge constraints' checked on. Also try modelling the slab to the wall centreline, making sure there is a slab node at the wall ends.

2) You can import the dxf and trace over the breaks with null elements. Then divide the shell with intersecting beams. You can even import it and let ETABS recognise that layer as null elements.

3) ETABS automesh produces fairly poor meshes in my experience. I think it's a great habit to have most of your slabs manually meshed.

4) Only one way to find out... Load will be attracted to stiffness. The central group of walls seem like a good candidate.

5) I would assume so.

6) Is the problem having to manually mesh the slab? Or how to design the walls?

As a side note, I usually use the mesh that RAM Concept produces as the mesh in ETABS. Set the element size in RAM Concept to something manageable, export the dwg. Then import the dwg as a floor. ETABS will then recognise the layer used and assign slab section properties to your triangles/quads. Also having a manual mesh saves a huge amount of run time, when performing the analysis. Just make sure you're not letting ETABS try and automesh your manual mesh...

Hope this helps.

 

[radiocontrolhead]

In response to your input above (much appreciated):

1) I will use edge constraints and will revise the mesh such that more nodes coincide with wall centerline and always have nodes at wall ends.

2) I am not 100% clear on this but I will do some experimenting and report back with any questions I might have.

3) Ok great, I think so too, just wasn't sure if it was absolutely necessary.

4) Perfect

5) Perfect

6) The main problem is having to manually mesh the slab and having a solid approach to it. With that said, it came from the fact that I wanted to capture in plane stresses due to the large openings in the center of the slab and to design the core walls for the the eccentric earth pressure from the the northern at-rest retaining walls. (see attached for etabs model clarification). The only way I think i may be able to do so is to model the slab as a shell element instead of using a null shell approach (mentioned in OP).

 

[Trenno]

Hi RCH,

Just to clarify point 2).

I think it may be easier to change the layer of your red mesh edges to something unique in AutoCAD. Then using the 'import floor plan' dialogue Link, set the red mesh edge layer to beams. I believe you may even be able to assign them the null property at this step. If not, go to 'select' > 'select by type' > 'frames' then assign them the null property. Now select the total floor shell and go to 'edit' > 'divide shells' > 'divide shells with selected frames.' This should split your slab shell into the desired mesh you're after. Then, for completeness, you can select all the beams and delete them.

As a surefire way to check your slabs and walls are connected at wall ends, draw a window over the corner or end of a wall. If down in the left hand corner of the screen it says 1 joint selected, you know your slab and wall are connected properly. If there are more than one joint selected, you'll have to move the offending node back to the wall centreline/end. You'll see this when you plot modal shapes too, things are easily detected when you run the animation in the bottom right hand corner - walls and slabs dance! The 'Align' function also comes in handy when you need to stitch together slabs and walls.

I've found, the less modelling within ETABS you can do, the better. Save your time in AutoCAD by making sure things are aligned and connected properly. Stitching models together can be a nightmare when you have a large model. I'd recommend also letting RAM Concept create your meshes for you. Let me know if you'd like me to run through the steps for that process. You may still need to do a little cleaning, but I think it's worth it for the simplicity of generating a good mesh.

Here some food for thought - how about you try modelling your in-plane loads in your RAM Concept model? Set your walls to 'shear walls' and set up some additional load cases for lateral (Fx and Fy) loads. You can then plot all the stresses you'd ever want, to see how the load is distributed around your floor plate. Might be a good validation of what ETABS is telling you.

Hope this helps.

 

[radiocontrolhead]

Hi Trenno,

Thank you very much for the helpful clarification and advice. I am going to execute the steps for breaking up the slab mesh via null beams shortly. I think I will be able to get through it with success.

It would be great if you could go through the steps on how to import a mesh from Ram into Etabs. What I couldn't understand was lets say once the ram concept mesh has been successfully imported into Etabs, would the walls (in etabs) need to be divided in such a way to ensure that they are connected to the slab? In your terms, to "stitch" them together? I am not aware of any way to divide the walls in Ram concept in finite "widths" along the wall length forcing Ram Concept to include nodes at those divisions.

I have no issue with having to come back and "stitch" the walls to the floor slabs if it means having a more accurate in-plane stress analysis from a more refined mesh. I have attached the mesh generated from Ram concept (screen shot) for sake of discussion. The mesh size is limited to 4' and accounts for the drop panels that are required for design, something I hadn't yet gotten to with my preliminary manual mesh...

Again, I truly appreciate your help with this.

 

[Trenno]

Hi RCH,

There isn't a plugin or anything for a RAM to ETABS import. However, once you generate your mesh, go to the 'mesh plan' layer in RAM Concept > Export that mesh plan with columns and walls turned on, this helps you visualize better. In AutoCAD you may want to change the layer of the mesh to something unique. Then using the .dwg file of your RAM mesh use the floor plan import in ETABS as described in my earlier post. Set the mesh so as to assign it a slab section property. Again, you may need to make sure slab nodes are connected to columns and walls.

Technically speaking, you should only need to model slabs in both RAM and ETABS to the centreline of walls. RAM treats walls as essentially line spring supports. The thickness of the wall determines the spring stiffness etc. I notice in your screenshot, you've modelled the slab edge to the far edge of the central pool walls. You may want to trim this back to the centreline before you try and export the mesh. The slab between the centreline of the wall and the far edge of the wall is essentially cantilevering and RAM attempts to mesh this very finely but for no real benefit.

I don't think you will need to divide the wall to match the slab mesh, along the length of the walls. The edge constraint tool in ETABS should take care of this, but you need to ensure the slab edge is aligned with the wall centreline.

Another beauty of using the RAM mesh in ETABS, is that you are able to easily identify slab thickness changes. As such, you're able to quickly assign the drop panels a thicker/stiffer section in your ETABS model. I've done this for one way slab/beam systems in the past.

I recommend giving my suggestion of modelling lateral loads in RAM a shot. It wouldn't take long, because you already have you model finished and working nicely in RAM. Plus it's only a single story building, as such I don't think lateral deflection will be a huge issue for you.

Good luck!