Page History

[Problem Specification|SIMULATION:3D Curved Beam]
[1. Start-up and preliminary set-up|SIMULATION:3D Curved Beam step 1]
[2. Specify element type and constants|SIMULATION:3D Curved Beam step 2]
[3. Specify material properties|SIMULATION:3D Curved Beam step 3]
[4. Specify geometry|SIMULATION:3D Curved Beam step 4]
[5. Mesh geometry|SIMULATION:3D Curved Beam step 5]
{color:#ff0000}{*}6. Specify boundary conditions{*}{color}
[7. Solve\!|SIMULATION:3D Curved Beam step 7]
[8. Postprocess the results|SIMULATION:3D Curved Beam step 8]
[9. Validate the results|SIMULATION:3D Curved Beam step 9]

h2. {color:#000000}Step 6: Specify boundary conditions{color}

Recall that the BCs for face 1 are:
u=0 at node A (keypoint 1)
v=0 at all face 1 nodes
w=0 along AB (line L7)

These BCs are in the cylindrical coordinate system. Switch to this coordinate          system:

*Utility Menu > WorkPlane > Change Active          CS to > Global Cylindrical*

We'll work with areas while specifying the BCs. So plot areas: *Utility          Menu > Plot > Areas*

h4. {color:#cc0000}Rotate Nodal Coordinate System{color}

In ANSYS, the boundary constraints are applied in the          nodal coordinate system which by default is parallel to the global Cartesian          system. Since we want to apply the constraints in the global Cylindrical          coordinate system, we need to rotate the nodal coordinate system into          the active coordinate system (i.e. Cylindrical) using the nrotat command.

Type nrotat,all in the _Input_ window.

To see the help page for _nrotat_, type help,nrotat in the _Input_ window.

h4. {color:#cc0000}Apply u=0 at Node A{color}

*Main Menu > Preprocessor > Loads >          Define Loads > Apply > Structural > Displacement > On Nodes*

Select node at A in the lower-right corner and click *{_}OK{_}* in the pick menu. Select *{_}UX{_}* for *{_}DOFs          to be constrained{_}*. You can leave the *{_}Displacement          value{_}* blank since the default is zero. Click *{_}OK{_}*.          You'll see an arrow symbol in the _Graphics_ window indicating that          the node A is constrained in the radial direction.

h4. {color:#cc0000}Select Nodes on Face 1{color}

ANSYS provides extensive capabilities, referred to as          "select logic", for selecting a subset of the full model using          various criteria. We'll use select logic to select the nodes on face 1.          We'll first select the area corresponding to face 1 and then select the          nodes attached to this area.

Utility Menu > Select > Entities

Select *{_}Areas{_}* from the pull-down menu          at the top. Make sure *{_}By Num/Pick{_}* is selected below that. Click *{_}Apply{_}*.

Hold down the left mouse button until face 1 is picked. Click *{_}OK{_}* in the pick menu.

Only the area corresponding to face 1 is selected currently. Verify this: *Utility Menu > Plot > Areas.*

Next we'll select the nodes attached to the selected area. In the _Select          Entities_ menu, select *{_}Nodes{_}* from          the pull-down menu at the top and *{_}Attached{_}* to below that. Select *{_}Areas, All{_}* below that. Click *{_}Apply{_}*.

Check that only nodes attached to face 1 are currently selected: *Utility          Menu > Plot > Nodes*

h4. {color:#cc0000}Apply v=0 on Face 1{color}

*Main Menu > Preprocessor > Loads >          Define Loads > Apply > Structural > Displacement > On Nodes*

*{_}Pick All{_}* nodes in the pick menu.          Select *{_}UY{_}* for *{_}DOFs          to be constrained{_}* and click *{_}OK{_}*.          You'll see arrow symbols in the _Graphics_ window indicating that          the nodes on face 1 are constrained in the circumferential direction.

We can use _Pick All_ since only the nodes on face          1 are currently selected. ANSYS commands apply only to the currently selected          entities.

h4. {color:#cc0000}Select Nodes Along AB{color}

*Plot lines: Utility Menu > Plot > Lines*

In the _Select Entities_ menu, select *{_}Lines{_}* from the pull-down menu at the top and *{_}By          Num/Pick{_}{*}{*}{_}Apply{_}* below that. Click .

Click on line AB (L7) and *{_}OK{_}* in the          pick menu.

Next we'll select the nodes attached to the selected line. In the _Select          Entities_ menu, select *{_}Nodes{_}* from          the pull-down menu at the top and *{_}Attached          to{_}* below that. Select *{_}Lines, All{_}* below that. Click *{_}Apply._*

Check that only nodes attached to line AB are currently selected: *Utility          Menu > Plot > Nodes*

h4. {color:#cc0000}Apply w=0 Along AB{color}

*Main Menu > Preprocessor > Loads >          Define Loads > Apply > Structural > Displacement > On Nodes*

*{_}Pick All{_}* nodes in the pick menu.          Select *{_}UZ{_}* for *{_}DOFs          to be constrained{_}* and click *{_}OK{_}*.

h4. {color:#cc0000}Define Function{color}

Recall that the BCs for face 2 are:
v=0.0001(r{~}c~\-r) at all face 2 nodes
w=0 along CD (line L5)

Since the BC on v is a function of the spatial coordinates, we need to          define a function to apply this BC. Bring up the function editor:

*Utility Menu > Parameters > Functions          > Define/Edit...*

You can enter the function using the calculator buttons or type it in.          The variables such as *{_}TIME{_}*, *{_}X{_}*, *{_}Y{_}* etc. that are available for defining          functions are in the pull-down list below the *{_}Result{_}* field. For entering the spatial coordinates _X_ and _Y_, use          the pull-down menu. Enter the function:

Result = 1e-4*(72.2e-3 - sqrt(
{X}
\^2\+
{Y}
\^2))
\\

Note that variables are enclosed in squiggly brackets.

Save the function: *Function Editor > File          > Save*

Use vface2.func for the filename.

Close the function editor.

h4. {color:#cc0000}Define Table from Function{color}

ANSYS doesn't allow the user to use functions directly          while applying loads to a model. Instead, one has to go through the additional          step of using a "Function Loader" that retrieves the function          and loads it as a _Table_ array. The _Table_ array can then          be applied to the model. The process is not exactly elegant but then we          are engineers.

*Utility Menu > Parameters > Functions          > Read From File*

Select _vface2.func_ and click *{_}Open{_}*.

Enter vface2 for *{_}Table          parameter name{_}*.

Observe that ANSYS displays the equation that will be used in creating          the _Table_ array. Click *{_}OK{_}*.

h4. {color:#cc0000}Select Nodes on Face 2{color}

Start by selecting the whole model to undo previous selects.

*Utility Menu > Select > Everything*

*Utility Menu > Plot > Areas*

To select the nodes on face 2, we'll follow the same procedure as for          face 1.

*Utility Menu > Select > Entities*

Select *{_}Areas{_}* from the pull-down menu          at the top. Select *{_}By Num/Pick{_}* below          that. Click *{_}Apply{_}*.

Hold down the left mouse button until face 2 is picked. Click *{_}OK{_}* in the pick menu.

Only the area corresponding to face 2 is selected currently. Verify this: *Utility Menu > Plot > Areas.*

Next we'll select the nodes attached to the selected area. In the _Select          Entities_ menu, select *{_}Nodes{_}* from          the pull-down menu at the top and *{_}Attached          to{_}* below that. Select *{_}Areas, All{_}* below that. Click *{_}Apply{_}*.

Check that only nodes attached to face 2 are currently selected: *Utility          Menu > Plot > Nodes*

h4. {color:#cc0000}Apply BC for v on Face 2{color}

We'll use the _vface2_ table that we created to apply this BC.

*Main Menu > Preprocessor > Loads >          Define Loads > Apply > Structural > Displacement > On Nodes*

*{_}Pick All{_}* nodes in the pick menu.          Select *{_}UY{_}* for *{_}DOFs          to be constrained{_}*. Select *{_}Existing table{_}* under *{_}Apply as{_}* and click *{_}OK{_}*.

We have defined only one table (*{_}VFACE2{_}*)          and that is automatically selected. Click *{_}OK{_}*.

You'll see arrow symbols in the _Graphics_ window indicating that          the nodes on face 2 are constrained in the circumferential direction.

h4. {color:#cc0000}{*}Select{*}{color} {color:#cc0000}{*}Nodes Along CD{*}{color}

Plot lines: *Utility Menu > Plot > Lines*

In the _Select Entities_ menu, select *{_}Lines{_}* from the pull-down menu at the top and *{_}By          Num/Pick{_}* below that. Click *{_}Apply{_}*.

Click on line CD (L5) and *{_}OK{_}* in the          pick menu.

Next we'll select the nodes attached to the selected line. In the _Select          Entities_ menu, select *{_}Nodes{_}* from          the pull-down menu at the top and *{_}Attached          to{_}* below that. Select *{_}Lines, All{_}* below that. Click *{_}Apply{_}*.

Check that only nodes attached to line CD are currently selected: *Utility          Menu > Plot > Nodes*

h4. {color:#cc0000}Apply w=0 Along CD{color}

*Main Menu > Preprocessor > Loads >          Define Loads > Apply > Structural > Displacement > On Nodes*

Pick All nodes in the pick menu.          Select *{_}UZ{_}* for *{_}DOFs          to be constrained{_}*. Select *{_}Constant value{_}* under *{_}Apply as{_}* and click *{_}OK{_}*.

*Utility Menu > Select > Everything*

*Utility Menu > Plot > Volumes*

Save your work:*Toolbar > SAVE_DB*

Go to [Step 7: Solve\!|SIMULATION:3D Curved Beam step 7]