Nothing Special   »   [go: up one dir, main page]
Scribd Logo
Upload

Welcome to Scribd!

  • 95 views

    Workshop 03.1: Linear Structural Analysis: Introduction To ANSYS Mechanical

    Uploaded by

    Emrah

    Copyright:

    © All Rights Reserved
    Download as PDF, TXT or read online from Scribd

    Workshop 03.1: Linear Structural Analysis: Introduction To ANSYS Mechanical

    Uploaded by

    Emrah
    95 views24 pages

    Original Title

    Mechanical_Intro_17.0_WS03.1_Linear_Structural_Analysis

    Copyright

    © © All Rights Reserved

    Available Formats

    PDF, TXT or read online from Scribd

    Did you find this document useful?

    Is this content inappropriate?

    Copyright:

    © All Rights Reserved
    Download as PDF, TXT or read online from Scribd
    Download as pdf or txt
    95 views24 pages

    Workshop 03.1: Linear Structural Analysis: Introduction To ANSYS Mechanical

    Uploaded by

    Emrah

    Copyright:

    © All Rights Reserved
    Download as PDF, TXT or read online from Scribd
    Download as pdf or txt
    of 24

    17.

    0 Release

    Workshop 03.1: Linear Structural Analysis


    Introduction to ANSYS Mechanical

    1 © 2016 ANSYS, Inc. March 11, 2016


    Goals
    The geometry for Workshop 03.1 consists of a 5-part assembly representing an
    impeller-type pump. Our primary goals are to analyze the assembly with a 100 N load
    on the belt to confirm that:
    − The impeller will not deflect more than 0.075 mm with the applied load.
    − The plastic pump housing will not exceed the material’s elastic limits around the shaft bore.

    2 © 2016 ANSYS, Inc. March 11, 2016


    Assumptions
    • The pump housing is rigidly mounted to the rest of the pump assembly. To simulate
    this, a frictionless support is applied to the mounting face.
    • Similarly, frictionless surfaces on the mounting hole counter bores will be used to
    simulate the mounting bolt contacts. (Note that if accurate stresses were desired at
    the mounting holes, a “Compression Only” support would be a better choice).
    • A 100-N bearing load is used on the pulley to simulate the load from the drive belt.
    The bearing load will distribute the force over the face of the pulley and provide a
    reasonable approximation of the force distribution caused by belt contact.

    3 © 2016 ANSYS, Inc. March 11, 2016


    Project Schematic
    1. From the Toolbox insert a “Static
    Structural” system into the Project
    Schematic. 1.

    2. From the Geometry cell, RMB and


    “Import Geometry > Browse”.
    Import the file “Pump_assy_3.stp”.
    2.

    3. Double click the “Model” cell to


    3.
    start the Mechanical application.

    4 © 2016 ANSYS, Inc. March 11, 2016


    Preprocessing
    4. From the main menu within the ANSYS Mechanical environment, select Units, and
    change the system’s unit to “Metric (mm, kg, N, s, mV, mA).” (Note: The material
    data is not being checked, but it is still good practice to confirm the units.)
    5. Return to the Workbench window and add “Polyethylene” the Engineering Data:
    a. Double-click the Engineering Data cell.
    b. Activate the Engineering Data Sources toggle, highlight General Materials, and click the “+”
    sign next to “Polyethylene”.
    c. Return to Project Schematic.

    5a.
    5c.

    5b.

    5 © 2016 ANSYS, Inc. March 11, 2016


    Preprocessing
    6. Refresh the Model cell:
    a. Click Model cell and RMB > Refresh. 6a.
    b. Return to the Mechanical window.

    7. Change the material on the pump housing:


    7a.
    a. Highlight “PumpHousing” under geometry.
    b. From details change the material assignment to
    “Polyethylene”. 7b.

    6 © 2016 ANSYS, Inc. March 11, 2016


    Preprocessing
    8. Change the contact behavior for one of the contact
    regions (shown below):
    a. Use the shift key to select all of the contact regions, then
    RMB > Rename Based on Definition.
    b. From the Details window, change the contact Type to “No
    Separation” for contact region “Bonded - PumpHousing to
    Shaft.”
    • The remainder of the contacts will be left as “Bonded”
    (this is the default contact Type).

    7 © 2016 ANSYS, Inc. March 11, 2016


    Environment
    9. Apply the bearing load to the pulley:
    a. Highlight the “Static Structural” branch.
    b. Highlight the pulley’s groove surface.
    c. RMB > Insert > Bearing Load”.
    d. From the detail window change Define By to “Components” and X Component to “100 N.”

    8 © 2016 ANSYS, Inc. March 11, 2016


    Environment
    10. Apply supports to the assembly:
    a. Highlight the mating face on the pump housing (part 1).
    b. “RMB > Insert > Frictionless Support”.

    9 © 2016 ANSYS, Inc. March 11, 2016


    Environment
    • Now we will add the frictionless supports to the 8 countersink portions of the
    mounting holes (shown here).
    • Each of the required surfaces could be selected individually while holding the CTRL
    key. However, this could be accomplished more swiftly by the use of either Named
    Selections (proceed to Slide 11) or a macro (proceed to Slide 12).

    10 © 2016 ANSYS, Inc. March 11, 2016


    Environment—Alternative 1
    11. Select any one of the countersink surfaces, then:
    a. RMB, choose “Create Named Selection.” 11a.
    b. Under “Apply geometry items of same,” check box for “size.”
    c. Click “OK.”
    d. RMB on Static Structural and insert a Frictionless Support.
    e. In the details window switch “Scoping Method” to Named
    Selection.
    f. Under “Named Selection” switch to “Selection.”
    11b.
    11f.

    g. Proceed to Step 13 on Slide 14.

    11 © 2016 ANSYS, Inc. March 11, 2016


    Environment—Alternative 2
    11. Rather than using Named Selections, the selection can be accomplished by
    running a “select by size” macro:
    a. Highlight any one of the countersink surfaces.
    b. Choose “Tools > Run Macro… ” and browse to:
    C:\Program Files\ANSYS Inc\v170\aisol\DesignSpace\DSPages\macros
    c. In the file browser, choose “selectBySize.js.”
    d. Click “Open.”
    e. Proceed to Step 12 on 11a.
    Slide 13.

    11c.

    11d.
    12 © 2016 ANSYS, Inc. March 11, 2016
    Environment
    12. The 8 countersink surfaces are now selected. From the context menu, click on
    “Supports” and choose “Frictionless Support” or “RMB > Insert > Frictionless
    Support.”

    13 © 2016 ANSYS, Inc. March 11, 2016


    Solution
    13. Highlight the “Analysis Settings” branch. In the Details
    view, confirm that Weak Springs is set to “Off.” 13.

    14. Solve.

    14 © 2016 ANSYS, Inc. March 11, 2016


    Postprocessing
    15. Add results:
    a. Highlight the solution branch.
    b. From the context toolbar, choose Stress > Equivalent (von-Mises) or
    RMB > Insert > Stress > Equivalent (von-Mises).
    c. Repeat the step above, choosing Deformation > Total.
    d. Solve again.
    • Note: Adding results objects and clicking Solve will not cause a
    complete solution to take place. Requesting new results requires only
    the reading of data from the results file, and should take just a second
    or two.
    • Alternatively, the newly defined results can be requested by RMB >
    Solution > Evaluate All Results.

    15 © 2016 ANSYS, Inc. March 11, 2016


    Postprocessing
    • While the overall plots can be used as a reality check to verify our loads, the plots
    are less than ideal since much of the model is displayed in few colors. (Your results
    may vary slightly due to meshing differences).

    • To improve the quality of results available we will “scope” results to individual


    parts.
    16 © 2016 ANSYS, Inc. March 11, 2016
    Postprocessing
    16. Scope the results to specified geometry: 16a.
    a. Highlight the “Solution” branch and switch the selection
    filter to “Body” select mode.
    b. Select the impeller. 16b.
    c. “RMB > Insert > Stress > equivalent (von-Mises)”
    • Notice the detail for the new result indicates a scope of
    1 Body.
    • Now the local variation in the results are more visually
    distinct.
    17. Repeat the procedure above to insert “Total
    Deformation” results for the impeller part.
    18. Repeat to add individually scoped stress and
    deformation results for the pump housing.

    17 © 2016 ANSYS, Inc. March 11, 2016


    Postprocessing
    19. To give more meaningful names to the result objects, it is useful to automatically
    rename the new results:
    a. Select all results objects > RMB > Rename Based on Definition. The result objects should now
    contain more informative names
    20. RMB > Evaluate All Results

    19

    18 © 2016 ANSYS, Inc. March 11, 2016


    Postprocessing
    • By checking the impeller deformation we can verify that one of our goals is met. The
    maximum deformation is approximately 0.022 mm (goal < 0.075 mm).

    19 © 2016 ANSYS, Inc. March 11, 2016


    Postprocessing
    • Inspection of the housing stress shows that, overall, the stress levels are below the
    material’s elastic limit (tensile yield = 25 MPa). We could again use scoping to isolate
    the results in the area of interest.

    20 © 2016 ANSYS, Inc. March 11, 2016


    Postprocessing—Examining Stress Results
    • Stress results contours are not as “smooth” as deformation results contours,
    because the displacement field is continuous across element boundaries whereas
    the stress field is not. Therefore, the stress results contours may show small
    discontinuities where they cross element boundaries. By default, ANSYS displays an
    averaged stress result to reduce these discontinuities. You may also choose to view
    the unaveraged stress results:

    Averaged — versus — Unaveraged

    21 © 2016 ANSYS, Inc. March 11, 2016


    Go Further!
    If you find yourself with extra time, consider the following:
    1. The Mesh is very coarse. In order to get more physically meaningful results, the
    mesh must be refined—apply mesh controls to refine the mesh. Try to achieve
    something similar to this:

    22 © 2016 ANSYS, Inc. March 11, 2016


    Go Further!

    2. Solve again and re-examine the results:

    23 © 2016 ANSYS, Inc. March 11, 2016


    END
    Workshop 03.1: Linear Structural Analysis

    24 © 2016 ANSYS, Inc. March 11, 2016

    You might also like