OS-HM-T:3020 接触する固体ブロックのNLSTAT解析

チュートリアルレベル：初級本チュートリアルの目的は、弾塑性材料、接触、前の非線形荷重ケースに引き続く非線形解を含む、OptiStructの非線形陰的微小変位解析の実行を示すことにあります。

開始する前に、このチュートリアルで使用するファイルを作業ディレクトリにコピーします。

図 1は、本チュートリアルに使用される構造モデルを示します。２つの四角い固体ブロックは、弾塑性スチール材料から成っています。ブロックの寸法と材料パラメータは下記の表を参照してください。

最初の非線形サブケースで、圧力が上の固体ブロックに作用します。その上部の角は、X方向とY方向が拘束されています。上の固体は下の固体と接触し、その底部の角はX、Y、Z方向が拘束されています。２番目の非線形サブケースは、除荷のシミューレートで、前の載荷のサブケースの非線形解の続きになります。
図 1. モデルと荷重の詳細


表 1. パラメータ
単位系 長さ： mm

時間： s

質量：Mgg

力：N

応力：MPa
上のブロック 72 mm x 72 mm
下のブロック 100 mm x 100 mm
ブロックの厚み 20 mm
材料 スチール、弾塑性:

初期密度（⍴）：7.90e-9 kg/mm3

ヤング率（E）：210000 MPa

ポワソン比（v）：0.3

降伏応力(σ0)：850.0 MPa
作用圧力 1000.0 MPa、上のブロックの中心に作用
以下の演習が含まれます：
  • 弾塑性材料の生成
  • 2つのブロック間の接触の定義
  • 非線形陰解法のパラメータの定義
  • 最初のサブケース（載荷）のNLSTAT解析のセットアップ
  • 2つ目のサブケース（徐荷）のNLSTAT解析のセットアップ
  • ジョブのサブミットと結果の確認

Launch HyperWorks

  1. Launch Altair HyperWorks.
  2. In the New Session window, select HyperMesh from the list of tools.
  3. For Profile, select OptiStruct.
  4. Click Create Session.
    図 2. Create New Session


    This loads the user profile, including the appropriate template, menus, and functionalities of HyperMesh relevant for generating models for OptiStruct.

Import the Model

  1. On the menu bar, select File > Import > HyperMesh Model.
  2. Navigate to and select nlstat.hm.
  3. Click Import.

モデルのセットアップ

Create the Elasto-plastic Material

First, the stress versus plastic strain curve for the material needs to be defined.

  1. In the Model Browser, right-click and select Create > Curve.
    A new window of the Curve Editor opens.
  2. For Name, enter stress-strain.
  3. Enter the following values for (x, y) in the pop-up window.

    (x1, y1) = (0.00, 850.00)

    (x2, y2) = (0.20, 5940.60)

    図 3. Create Stress-strain Curve


  4. In the Model Browser, under Curves, select the stress-strain curve.
  5. Click Color and select a color from the palette.
  6. To update the elasto-plastic material, in the Model Browser select the material steel.
    The Entity Editor opens.
  7. Selet the MATS1 check box to define elastic-plastic material.
  8. For TID, select Unspecified > Curves.
  9. In the Select Curves dialog, select the stress_strain curve and click OK.
  10. Input the following values in the editor.
    • E = 210000.0
    • NU = 0.3
    • RHO = 7.9e-09
    • TYPE = PLASTIC
    • YF = 1
    • HR = 1
    • LIMIT = 850.0
    • TYPSTRN = 1
    TYPSTRN of 1 specifies stress (Y) versus strain (X).
    図 4. Define Elastic-Plastic Material


    See 表 1 for details.

Define Contact Between the Two Blocks

The contact surfaces for the two blocks need to be defined.

  1. In the Model Browser, right-click and select Create > Set.
  2. For Name, enter top.
  3. For Card Image, select SET_ELEM from the drop-down menu.
  4. For Set Type, verify non-ordered is selected.
  5. For Entity IDs, select Unspecified > Property.
  6. In the Select Properties dialog, select the top solid block Solid1 and click Close.
    図 5. Create Set


  7. Similarly, create another set named bottom.
  8. Repeat steps 3 through 6 and for Entity IDs, select Solid2,
  9. To define the interface, in the Model Browser, right-click and select Create > Contact.
  10. For Name, enter SOLID_CONTACT.
  11. Click Color and select a color from the palette.
  12. For Card Image, select CONTACT from the drop-down menu.
  13. For Main Entity IDs, select Set from the extended selection menu.
  14. In the Advanced selection dialog, choose bottom and click OK.
  15. For Secondary Entity IDs, select the top set.
  16. For TYPE, select SLIDE from the drop-down menu.
  17. For MORIENT, select NORM from the drop-down menu.
  18. Click Close.
    図 6. Define Contact Surfaces


Define Nonlinear Implicit Parameters

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
  2. For Name, enter nlparm.
  3. For Config type, select Nonlinear Parameters.
    The default type is NLPARM.
  4. Enter the following values in the dialog:
    • NINC = 10
    • DT = 0.0
    • MAXITER = 25
    • CONV = UPW
    • EPSU = 0.001
    • EPSP = 0.001
    • EPSW = 1e-07
    図 7. Define Nonlinear Parameters


    See 表 1 for details.

Create the First Nonlinear (Loading) Subcase

  1. In the Model Browser, right-click and select Create > Load Step.
  2. For Name, enter loading.
  3. For Analysis type, select Non-linear static from the drop-down menu.
  4. For SPC, click Unspecified > Loadcol.
  5. From the dialog, select SPC from the list of load collectors and click OK.
  6. For LOAD, click Unspecified > Loadcol.
  7. From the dialog, select pressure from the list of load collectors and click OK.
  8. For NLPARM, click Unspecified > Load step inputs.
  9. From the dialog, select nlparm from the list of load step inputs and click OK.
  10. Click Close.
    図 8. Create Loading Subcase


Create the Second Nonlinear (Unloading) Subcase

  1. In the Model Browser, right-click and select Create > Load Step.
  2. For Name, enter unload.
  3. For Analysis type, select Non-linear static from the drop-down menu.
  4. For SPC, click Unspecified > Loadcol.
  5. From the dialog, select SPC from the list of load collectors and click OK.
  6. For NLPARM, click Unspecified > Load step inputs.
  7. From the dialog, select nlparm from the list of load step inputs and click OK.
  8. Select the CNTNLSUB check box and set the option to Yes.
  9. Click Close.
    図 9. Create Unloading Subcase


Define Output Control Parameters

  1. In the Model Browser, right-click and select Create > Cards > Output.
  2. Under CONTF, DISPLACEMENT, and STRESS, set Option to Yes.
  3. Under STRAIN, set EXTRA to PLASTIC.
  4. Click Close.

Submit the Job

Run OptiStruct.

  1. From the Analyze ribbon, click Run OptiStruct Solver.
    図 10. Select Run OptiStruct Solver


    A browser window opens.
  2. Select the directory where you want to write the OptiStruct model file.
  3. For File name, enter nlstat_complete.
    The .fem filename extension is the recommended extension for Bulk Data Format input decks.
  4. Click Save.
  5. Click Export.
  6. For run options, toggle .
  7. Click Run.
    If the job is successful, you should see new results files in the directory in which nlstat_complete.fem was run. The nlstat_complete.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

View Results

  1. Launch HyperView.
  2. Plot the Displacement, the von Mises stress, plastic strains and contact pressure contours at the end of the first (loading) step.
    図 11. Contour of Displacements in Blocks Subject to Loading


    図 12. Contour of von Mises Stress in Blocks Subject to Loading


    図 13. Contour of Plastic Strains in Blocks Subject to Loading


    図 14. Contour of Contact Pressure in Block Interface after the First (Loading) Subcase


  3. Change the subcase to the second (unloading) subcase and plot the displacement contour to see the change in displacements in the blocks subject to unloading.
    図 15. Contour of Displacements in Blocks Subject to Unloading in Second Subcase