MasterFrame FEA - Semi-Detached House Raft

Posted on January 23rd, 2019 in Analysis

Summary

This video demonstrates the process of using MasterSeries software to design a raft foundation for a semi-detached house with garages. The presenter meticulously outlines how to import a DXF drawing, define the structural elements like slabs and beams, and apply various dead and live loads to the model. A significant portion of the demonstration focuses on Finite Element Analysis (FEA), specifically addressing how to refine the mesh, interpret stress errors, and implement attached beams to improve the model's accuracy and stability before finally reviewing the required reinforcement for the raft.

Key Points

• DXF Import
• Slab Loading
• Mesh Refinement
• Reinforcement Design
• Strip Averaging

Description

This video demonstration outlines the process of designing a raft foundation for a semi-detached house with garages using MasterSeries Software, focusing on finite element analysis (FEA).

The process involves several key steps:

• Model Import and Initial Setup:

    ◦ The drawing of the semi-detached house is first saved as a DXF file.

    ◦ This DXF file is then imported into MasterFrame, creating a new file named "Sammy house".

    ◦ The model initially consists of fifteen members and twelve nodes.

• Creating the FEA Surface (Slab):

    ◦ A brand new slab is added, covering the entire panel.

    ◦ It is defined as being on "soft clay" with 10,000 kilonewtons per meter cubed compression only support.

    ◦ The slab material is set to AC30 isotropic and 200mm thick.

• Applying Loads:

    ◦ Live loads of -2.5 kN/m² are applied as "alternate loads" across the garage and the rest of the structure.

    ◦ Various dead line loads are added:

        ▪ Two loads of -15 kilonewtons each are placed across the structure to carry the first floor and roof.

        ▪ A third dead load of -30 kilonewtons is applied.

        ▪ Smaller dead loads of -10 kilonewtons are added front and back.

    ◦ Live line loads for the roof and first floor are then applied, ranging from -5 kilonewtons to -20 kilonewtons, using existing load points.

    ◦ The loads are assigned to FE surface load patterns (L1/D1 and L2/D2) for patterning.

• Analysis Setup and Initial Instability:

    ◦ Eurocode loading cases (concrete 1.35 and 1.25 factors) are imported.

    ◦ A default 1-meter mesh is set for the FE surface global options.

    ◦ An initial static analysis reveals the frame is unstable because it can rotate.

    ◦ Two pinned restraints (no Y, X, or Z rotation) are added to stabilize the structure.

• Error Checking and Mesh Refinement:

    ◦ Graphical results show significant errors (up to 17%) in certain areas.

    ◦ The global mesh size is reduced to 0.5 meters to reduce overall errors.

    ◦ To further improve accuracy around critical points, local mesh intensities are applied, with a mesh size of 0.1 meters and a radius of influence of 1.5 meters. This results in a much finer mesh around these points.

• Structural Modifications: Adding Drop Beams:

    ◦ To reduce remaining errors and enhance the structure, drop beams are introduced.

    ◦ Selected members are changed to concrete members, 400mm wide by 200mm deep.

    ◦ These are then defined as "attached beams" in the FE surface properties, indicating they are an additional 200mm deep and drop down from the centerline of the slab.

• Re-analysis and Results Interpretation:

    ◦ After adding beams, re-analysis shows "tiny tiny errors" that are considered acceptable.

    ◦ Initial displacement and moment results reveal an unexpected asymmetrical loading.

    ◦ Upon checking the loading, it is discovered that a load was applied on the wrong axis, causing the asymmetry.

    ◦ After correcting the load direction and re-analyzing, the results become symmetrical, showing expected high and low displacements and moments based on the pattern loading.

    ◦ Peak smoothing is considered but deemed ineffective in this case due to the absence of columns.

• Reinforcement Design and Slab/Beam Adjustments:

    ◦ The initial assessment of reinforcement (using EC2, 500 steel, 35N concrete) suggests that the current slab might be too thick or the reinforcement too light, especially for hugging (bottom steel).

    ◦ To optimize, the slab thickness is reduced from 200mm to 150mm.

    ◦ All attached beam depths are globally reduced from 200mm to 150mm and widths from 400mm to 300mm.

    ◦ A re-analysis with the thinner slab and beams shows a need for more reinforcement, particularly for Y top steel (393 mm²/m), with localized high values.

• Detailed Reinforcement Assessment using Force Lines:

    ◦ To accurately assess localized high reinforcement requirements, force lines are drawn through the structure.

    ◦ By applying a 1-meter strip width average, the high peak values for moments are reduced to more sensible figures (e.g., 500-600 mm²/m for YY bottom steel).

    ◦ This indicates that a base mesh (e.g., 393 mm²/m, or tens at 200mm spacing) would be needed, potentially with additional reinforcement over a 1-meter strip in critical areas.