FEA Applications I, Homework 11B

MET 415 - FEA Applications I

Prof. Dave Johnson, psuprofdj@psu.edu
Penn State - Erie, The Behrend College

Homework Assignment 11B

Concepts:

Line elements (beams and truss/link) - element types having different DOF's
Pin joints between beams (coincident nodes with Coupled DOF)
Postprocessing:
- ELEMENT Table Usage
- Reaction Force

A simplified model of a backhoe is shown in the figure. Some members can be treated as beam elements. Some can be treated as links. A 2D analysis model is appropriate to determine pin reactions and member forces.

Objective: determine forces at selected pins and forces carried in each member.

Assume all BEAM members have an I-shaped cross section with a section height of 10" (for a standard shape, web thickness: 0.311", flange width: 4.661", flange thickness: 0.491". This produces a cross-section with area = 7.38 in² and MOI = 122.6 in⁴). Use Preprocessor > Sections > Beam > Common Sects

Assume all three hydraulic cylinders are link members with a cross-sectional area of 5.066 in² (for simple tubing with outside radius: 3" and inside radius: 2.718"). Preprocessor > Real Constants > Add/Edit/…

Ignore the weight of the members and consider only the applied horizontal load of 2000 lbf.

Treat the bucket as three links in a right triangle, 3 ft. on each short side.

Since the analysis objective is to determine forces (not deflections and stresses), the material data and member cross-section data is arbitrary. Use steel properties for all parts.

Use (solid modeling) keypoints and lines to create the beam member geometry. [Note: for line element modeling, points B and C in the figure are the same point, B]. The elevation of point D is not critical, just place it lower than point A (about 2 ft. lower elevation than point A).

A sketch of the line geometry (in feet units) is available as an IGES file, backhoe_lines.igs Use a Right-click on this link, then "Save Target As...", then "Save as type: All Files", and use a file name like: backhoe_lines.igs

File > Import > IGES… but turn OFF: merging of coincident keypoints, create solid, and delete small areas. (This way, each line is not connected to any others - they have coincident, but not shared keypoints, where they meet.)

Scale the model to inch measure (use a factor of 12 to convert feet to inches in X and Y, Z=0)

There is one pin joint between two beams that must be specially treated. (If two beams meet at a common node, then they are fully bonded together at that joint). To model a pin, the mesh must have two co-incident nodes at only the spot where the beam/pin junction is needed. In ANSYS, we use Coupled-DOF to force the points to translate together (UX and UY), but leave the rotation/moment un-constrained (ROTZ)

Merge all coincident keypoints EXCEPT the joint (Point E) between the horizontal beam line and lines from the bucket up to point F.

Turn ON, line numbering and keypoint numbering (Toolbar buttons - OR - PlotCtrls > Numbering > …)
Determine which keypoint is on the horizontal beam line at point E
- List > Picked Entities, Lines … notice the KP numbers on ends of horiz. link
Unselect that keypoint (Select > Entities > Keypoints, By Num/Pick, Unselect …)
Merge all coincident keypoints (Preprocessor > Numbering Ctrls > Merge Items … keypoints)
Then Select > Everything
The only remaining coincident keypoints should be at point E.

Since LINK elements have no rotational DOF’s, where a LINK meets a BEAM there is automatically a pin joint. The special case we are handling is where two BEAM’s meet with a pin joint (point E).

Element Type > Add/Edit/Delete > Add ...BEAM188 and LINK180
Element Type > Add/Edit/Delete > Options … always check element behavior options
Real Constants > Add/Edit/Delete > Add ... one real constants needed for LINK180
Material Properties > Material Model > Linear > Elastic > Isotropic ... enter modulus and Poisson's ratio
Preprocessor > Sections > Beam > Common Sects … define the I-beam cross-section

MESH TOOL:
Assign "Attributes" to the lines (material, element type, and real constant set –OR – Section ID) to define which lines will be beams and which will be links.
Note: when specifying Section ID for BEAM, activate the “Pick Orientation KP’s” check box. You will be prompted to pick the KP for orientation. Suggestion: use the KP at point D to orient all beams.
Set Size Controls > On Lines … use 1 division for lines which will be link elements
Set Size Controls > Global … to control mesh on all other lines
Mesh all lines

Create two sets of Coupled DOF sets (for UX and for UY) at the beam-to-beam pin joint. Coupled-DOF’s act on NODES, not keypoints. Define them after you have meshed the model. Preprocessing > Coupling/Ceqn > Couple DOFs … create set 1 (two nodes, UX direction) and set 2 (same two nodes, UY direction)

Constrain KEYPOINTs at locations A and D in UX and UY and UZ
Constrain ALL KEYPOINTs in UZ
Apply Fx force to the left on the KEYPOINT at the bottom edge of the “bucket” links
(To prevent a rigid-body motion failure) Apply a rotational constraint (ROTY) on the KEYPOINT at location F

The ELEMENT TABLE is necessary to evaluate force/stress/etc. for line elements.
Info on the Element Table is also available at this link.

Use the HELP system to determine the data available for the Element Table:

Help,BEAM188

Table 188.1 BEAM188 Element Output Definitions

SF: y,z	Section shear forces
Fx	Axial force
MY, MZ	Bending Moments

Table 188.2 BEAM188 Item and Sequence Numbers

Output Quantity Name	ETABLE and ESOL Command Input
Output Quantity Name	Item	I	J
Fx	SMISC	1	14
My	SMISC	2	15
Mz	SMISC	3	16
SFz	SMISC	5	18
SFy	SMISC	6	19

Postproc > Element Table > Define Table > Add
- SFy-i, By Sequence Number, SMISC,6
- SFy-j, By Sequence Number, SMISC,19
- Mz-i, By Sequence Number, SMISC,3
- Mz-j, By Sequence Number, SMISC,16
Using Plot Results > Contour Plot > Line Elem Res (PLLS command) to show results along beams which vary - end-I to end-J. There are two values for each element to show the variation.

Help,LINK180

Table 180.1 LINK180 Element Output Definitions

Force Member force in the element coordinate system

Sxx Axial Stress

Force	Member force in the element coordinate system
Sxx	Axial Stress

Table 180.2 LINK180 Item and Sequence Numbers

Output Quantity Name	ETABLE and ESOL Command Input
Output Quantity Name	Item	E	I	J
Force	SMISC	1	-	-
Sxx	LS	-	1	2

Postproc > Element Table > Define Table > Add
Using Element Table > Plot Elem Table (PLETAB command) to show results along link elements. There is one values for each element (no variation).

Turn in:

A plot showing the mesh with element shape/size active, and ALL loads and constraints, including the coupled-DOF's

Select all BEAM elements (Select > Entities > Elements, By Attributes, Elem Type Num, …)
(Note: PLLS is done using Plot Results > Contour Plot > Line Elem Res)

Create a (PLLS) plot showing the SHEAR Force (SFz) in each BEAM element
Create a (PLLS) plot showing the Bending Moment (My) in each BEAM element

Select all LINK elements (Select > Entities > Elements, By Attributes, Elem Type Num, …)
(Note: PLETAB is done using Plot Results > Contour Plot > Elem Table)

Create a (PLETAB) plot showing the Axial Force in each LINK element
- PlotControls > Numbering ... activate Numeric Contour Labels + Color & Numbering
- PlotControls > WindowCtrls > Window Options ... de-activate Min-MAX Symbols

Select nodes at pin locations A, D, E (Select > Entities > Nodes, By Num/Pick) - there will be four nodes

Use force listing (PRNLD and/or PRRF) to find pin joint forces (X, Y) and then compute the total reaction (resultant vector) at these pins: A, D, E
Postproc > List Results > Reaction Solu
Postproc > List Results > Nodal Loads
Sketch a free-body diagram and use a hand calc to compare the force components at points A and D (hand calc of force is NOT required at point E)

Research question:

If we wished to run a transient or nonlinear analysis where the hydraulic cylinders changed length and caused the backhoe arm to move, what element in the ANSYS library would we choose to replace the 3D link/truss elements with ?

ANSYS (12.0) Workbench method:

Import the IGES geometry to DesignModeler (use feet units) and in Details: Process Line Bodies, Yes

Use Body Operation, Scale, if the model size needs to be adjusted - check size of the model wrt. the ruler
You should have 10 parts and 10 bodies. If not, Add Frozen for the Import - or - Freeze before the Scaling, Body Operation.
Under Concept, Cross Section > Circular Tube: define inner and outer radii: 0.2265 and 0.25 feet.
Under Concept, Cross Section > I Section: W1 = W2 = 0.3884, W3 = 0.8333, t1 = t2 = 0.0409, t3 = 0.0259 feet.
Under the 10 parts, 10 bodies, assign the proper cross-section to each body
Under the 10 parts, 10 bodies, give each body a meaningful name (in the Details area): like
- BEAM_A-B
- BEAM_F-E
- CYL_B-F
- BEAM_E-Bucket
- CYL_D-B
- Bucket1
- Bucket2
- Bucket3
- CYL_F-Bucket
Notice the 4 bodies which are I-sections still have a yellow checkmark. Alignment is required to define the orientation of the cross-section. (Round sections do not require alignment). To align the I-sections:
- Right mouse on the body and "Select Unaligned Edges."
- In the Details area, click on the yellow cross-seciton Alignment field,
- select a vertical line on the sketch,
- select the UP arrow, and
- Apply
- Do this for all 4 bodies with the I Section shape.
Before you move the model to Simulation, on the Project Schematic page under Properties, activate Basic Geometry Option, Line Bodies

Open Simulation (must be a 3D simulation since WB only has 3D Beam elements)

All line bodies are disconnected Joints must be manually added under "Connections," Body-Body
This process is easier if you suppress some bodies when trying to pick vertices for joints.
BEAM_A-B and BEAM_B-E need a "Fixed" Joint at point B
- Watch the Details Area to make sure you are getting the vertex of the proper body for each joint reference
BEAM_F-E and BEAM_E-Bucket need a "Fixed" Joint at point E
All other joints are "Revolute" joints
- CYL_D-B to either BEAM_A-B or BEAM_B-E at point B
- CYL_B-F to either BEAM_A-B or BEAM_B-E at point B
- CYL_B-F to BEAM_F-E at point F
- CYL_F-Bucket to BEAM_F-E at point F
- BEAM_B-E to either BEAM_F-E or BEAM_E-Bucket at point E
- load vertex on vertical bucket link to vertex on sloped bucket link
- BEAM_E-Bucket to vertical bucket link vertex
- BEAM_E-Bucket to horizontal bucket link vertex
- CYL_F-Bucket to horizontal bucket link vertex
- horizontal bucket link vertex to vertex on sloped bucket link
Apply Simply Supported constraints on points A and D
Apply 2000 lbf load on vertex at lowest corner of the bucket
Solve without "Weak Springs" for one load step with default Auto Time Stepping

Even though WB uses only BEAM188 elements, the bodies with the CYL cross-section should have NO bending stress since they have the revolute joint on each end to behave as a pin joint. Check the Max. and Min. Bending Stress using the Beam Tool for the 6 bodies which have the CYL cross-section to make sure they act as two-force members.

Unfortunately, the only way to extract the axial and shear forces and the bending moments is using the ETABLE in a Solution > Command Object. Select the groups of BEAM188's that represent the I shaped members, define the ETABLE commands, and generate the plots. Then, follow the same process for the CYL cross-section members. Such a Command Object might look like this: