How to make stepped beam in ANSYS 13

[mischelle]

I have one problem with Ansys. How to make beam with two different cross section areas when "Sections" in Menu accept just one?

Regards

 

[nvn]

mischelle: Put a node where you want the cross section to change. For the beam element from nodes 1 to 2, choose the desired cross section. For the beam element from nodes 2 to 3, choose the other cross section you want.

 

[mischelle]

Yes, I already did that but the problem is how to do that, how to define for this nodes from 1 to 2 is section b,h and from 2 to 3 is another b1, h1? How to do that?

 

[mischelle]

How to choose from 1 to 2 one cross section? Because in "Sections" I can define 2, 3 cross sections, but how to now on which part is associate it?

 

[mischelle]

Which functions to use for defining?

 

[nvn]

mischelle: Create the first cross section you want. (You would do this in a Beam Sections menu, although I do not know the exact name of the menu.) Next, create the second cross section you want.

Last, when you create the beam element from nodes 1 to 2, select the first cross section, by selecting a beam cross section button or menu, on the create beam element menu. And when you create the beam element from nodes 2 to 3, select the second cross section. Does this help?

 

[mischelle]

I followed this procedure. Use beam element 188, then define 1. cross section, then in modeling make nodes 1 and 2, straight line and mesh it. Then come back select second cross section, apply 2. Then make node 3, straight line, then mesh then PlotCtrls-style-size and shape-display of element-on and the beam is wit one cross section, doesn't work

 

[nvn]

mischelle: Perhaps try this. (1) In Main menu > Preprocessor > Real Constants, create Real Constant Set 1, and Real Constant Set 2, for your two cross sections.

(2) Create three collinear nodes (nodes 1, 2, and 3). Also create a noncollinear node (node 4), for orientation.

(3) In Main Menu > Preprocessor > Modeling > Create > Elements > Elem Attributes, specify real constant set 1.

(4) In Main Menu > Preprocessor > Modeling > Create > Elements > Auto Numbered > Thru Nodes, verify Pick is enabled.

(5) In the graphics window, define the first beam element by picking node 1, then node 2, then orientation node 4.

(6) In Main menu > Preprocessor > Modeling > Create > Elements > Elem Attributes, specify real constant set 2.

(7) In the graphics window, define the second beam element by picking node 2, then node 3, then orientation node 4.

Please let us know whether or not it works.

 

[mischelle]

nvn: no it is not possible to define real constants if you choose element 188 for the beam. After choosing the element and try to define real constants I got the message "The beam188 element type does not require real constants "

 

[mischelle]

nvn: But I am trying to do this, but when I open Auto Numbered it is not working because it is necessary to no nodes be selected (how). In Element Attributes, I can just choose sections 1 or 2 but I can not select the nodes?

 

[mischelle]

nvn: I am near to solve, first to use nodes, not key points, and instead real constants I defined two cross sections, now I have a problem to mesh, after I finish procedure I can see line between nodes 1 and 2 and the line between 2 and 3, but after that when I want to mesh I choose mesh all lines but the message appears there is no lines? Test it.

 

[nvn]

mischelle: Perhaps try this, continuing from post 8 ...

(8) In Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Nodes > Apply U, Rot on Nodes, verify that Pick and Single are enabled.
(9) In graphics window, select the node(s) you want to constrain.
(10) Select degrees of freedom you want to constrain.
(11) Under Constant value, enter 0.

(12) In Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Force/Moment > On Nodes > Apply F/M on Nodes, verify that Pick and Single are enabled.
(13) In graphics window, pick the node(s) you want to apply loads on.

(14) Select Utility Menu > File > Save as > jobname.db.
(15) Select Utility Menu > File > Resume from... > jobname.db.

(16) Select Main Menu > Solution > Solve > Current LS > (review listed summary) > OK.
(17) When solution is complete, plot results in, e.g., General Postproc > Plot Results > Contour Plot > Predefined > Stress.

Please let us know whether or not it works. Or please let us know if this is not what you want.

 

[mischelle]

nvn: my goal is to obtain natural frequencies, not to define forces, moments and others. So in that case I will put for displacement 0 DOF, so I need modal analysis and I know how to do that for single beam where I made a line like a beam through the keypoints, but here I used nodes and mesh is not working. How to manage mesh? Now I have a beam with two different cross sections and everything is ok, but modal analysis is not working because of mesh. Only options are for mesh: keypoints, areas, volumes, and I have nodes and Ansys does not accept. How to solve and obtain the natural frequencies, please, test it on your computer and if it is work help me with this simple problem, because I do not know what to do, I will be crazy of empty clicking!

 

[nvn]

mischelle: Perhaps try this. I cannot test it at this time. Please test it. And please let us know whether or not it works.

(1) Create keypoints 1, 2, and 3. Create line 1 from keypoint 1 to 2. Create line 2 from keypoint 2 to 3.

(2) In Ansys Main menu > Preprocessor > Real Constants, create Real Constant Set 1, and create Real Constant Set 2, for your two cross sections.

(3) Ansys Main menu > Preprocessor > Meshing > MeshTool > Element Attributes > Lines > Set > select first line > OK > for Real constant set number, enter 1 > OK.

(4) Ansys Main menu > Preprocessor > Meshing > MeshTool > Element Attributes > Lines > Set > select second line > for Real constant set number, enter 2 > OK.

(5) Ansys Main menu > Preprocessor > Meshing > MeshTool > Size Controls: Global > Set > Element edge length > 10 mm > OK > Lines > Mesh > Pick All.

 

[mischelle]

Yes it is working. Thank you very much. How do you make a free free boundary conditions in Ansys?

 

[nvn]

mischelle: Normally, you do nothing. A free-free boundary condition is no boundary conditions, and no constraints. You just select modal analysis, sometimes called normal modes analysis.