ABAQUS 货物吊车

example: cargo crane

A light-service, cargo crane is shown in

Figure 6

–

10

. You have been asked to

determine the static deflections of the crane when it carries a load of 10 kN.

You should also identify the critical members and joints in the structure: i.e.,

those with the highest stresses and loads. Because this is a static analysis you

will analyze the cargo crane using Abaqus/Standard.

Figure 6

–

10

Sketch of a light-service cargo crane.

The crane consists of two truss structures joined together by cross bracing.

The two main members in each truss structure are steel box beams (box

cross-sections). Each truss structure is stiffened by internal bracing, which is

welded to the main members. The cross bracing connecting the two truss

structures is bolted to the truss structures. These connections can transmit

little, if any, moment and, therefore, are treated as pinned joints. Both the

internal bracing and cross bracing use steel box beams with smaller

cross- sections than the main members of the truss structures. The two truss

structures are connected at their ends (at point E) in such a way that allows

independent movement in the 3-direction and all of the rotations, while

constraining the displacements in the 1- and 2-directions to be the same. The

crane is welded firmly to a massive structure at points A, B, C, and D. The

dimensions of the crane are shown in

Figure 6

–

11

. In the following figures,

truss A is the structure consisting of members AE, BE, and their internal

bracing; and truss B consists of members CE, DE, and their internal bracing.

Figure 6

–

11

Dimensions (in m) of the cargo crane.

The ratio of the typical cross-section dimension to global axial length in the

main members of the crane is much less than 1/15. The ratio is approximately

1/15 in the shortest member used for internal bracing. Therefore, it is valid to

use beam elements to model the crane.

6.4.1 Preprocessing

—

creating the model with Abaqus/CAE

In this section we discuss how to use Abaqus/CAE to create the entire model

for this simulation. Abaqus provides scripts that replicate the complete analysis

model for this problem. Run one of these scripts if you encounter difficulties

following the instructions given below or if you wish to check your work. Scripts

are available in the following locations:

A Python script for this example is provided in

“

Cargo crane,

”

Section

A.4

. Instructions of how to fetch the script and run it within Abaqus/CAE

are given in

Appendix A,

“

Example Files

.”

?

A plug-in script for this example is available in the Abaqus/CAE Plug-in

toolset. To run the script from Abaqus/CAE, select

Plug- ins

Abaqus

Getting Started

, highlight

Cargo crane

, and click

Run

. For more

information about the Getting Started plug-ins, see

“

Running the

Getting Started with Abaqus examples,

”

Section 79.1 of the

Abaqus/CAE User's Manual

.

?

If you do not have access to Abaqus/CAE or another preprocessor, the input

file required for this problem can be created manually, as discussed

in

“

Example: cargo crane,

”

Section 6.4 of Getting Started with Abaqus:

Keywords Edition

.

Creating the parts

The welded joints between the internal bracing and main members in the

crane provide complete continuity of the translations and rotations from one

region of the model to the next. Therefore, you need only a single geometric

entity (i.e., vertex) at each welded joint in the model. A single part is used to

represent the internal bracing and main members. For convenience, both truss

structures will be treated as a single part.

The bolted joints, which connect the cross bracing to the truss structures, and

the connection at the tip of the truss structures are different from the welded

joint connections. Since these joints do not provide complete continuity for all

degrees of freedom, separate vertices are needed for connection. Thus, the

cross bracing must be treated as a separate part since distinct geometric

entities are required to model the bolted joints. Appropriate constraints

between the separate vertices must be specified.

We begin by discussing a technique to define the truss geometry. Since the

two truss structures are identical, it is sufficient to define the base feature of

the part using only the geometry of a single truss structure. The sketch of the

truss geometry can be saved and then used to add the second truss structure

to the part definition.

The dimensions shown in

Figure 6

–

11

are relative to a global Cartesian

coordinate system. The base feature, however, must be sketched in a local

plane. To make the sketching easier, datum features will be used. A datum

plane, parallel to one of the trusses (truss B in

Figure 6

–

10

, for example), will

serve as the sketch plane. The orientation of the sketch plane will be defined

using a datum axis.

To define the geometry of a single truss:

1.

To create a datum plane, a part must first be created. A part consisting

of a single reference point will serve this purpose. Begin by creating a

three-dimensional deformable part using the point base feature. Set the

approximate part size to

20.0

, and name the part

Truss

. Place the point

at the origin. This point represents point D in

Figure 6

–

10

.

2.

Using the

Create Datum Point: Offset From Point

tool

, create two

datum points at distances of

(0, 1, 0)

and

(8, 1.5, 0.9)

from the

reference point. These points represent points C and E, respectively,

in

Figure 6

–

10

. Reset the view using the

Auto-Fit View

tool

the

View Manipulation

toolbar to see the full model.

3.

Using the

Create Datum Plane: 3 Points

tool

in

, create a datum

plane to serve as the sketch plane. Select the reference point first, and

then select the other two datum points in a counterclockwise fashion.

Click mouse button 2 to exit the procedure.

Note:

While selecting the points in this way is not required, it will

make certain operations that follow easier. For example, by

selecting the points in a counterclockwise order, the normal to

the plane points out of the viewport and the sketch plane will be

oriented automatically in the 1

–

2 view in the Sketcher. If you

select the points in a clockwise order, the plane's normal will

point into the viewport and the sketch plane will have to be

adjusted in the Sketcher.

4.

Using the

Create Datum Axis: Principal Axis

tool

, create a datum

axis parallel to the

Y-Axis

. As noted earlier, this axis will be used to

position the sketch plane.

5.

You are now ready to sketch the geometry. Use the

Create Wire:

Planar

tool

to enter the Sketcher. Select the datum plane as the

plane on which to sketch the wire geometry; select the datum axis as

the axis that will appear vertical and to the left of the sketch. You may

need to resize the view to select these entities.

6.

Once in the Sketcher, use the

Sketcher Options

tool to modify the

display. In the

General

tab, change the

Sheet size

to

20

and reduce

the

Grid spacing

to

8

. Zoom in to see the datum points more clearly.

Note:

If the sketch plane is not oriented in the 1

–

2 plane, use

the

Views

toolbar to change to the X

–

Y view.

Using the

Create Lines: Connected

tool

, sketch the lines

representing the main truss, as shown in

Figure 6

–

12

. The datum points

that were projected are treated as fixed points in the sketch. Any line

connected to one of these points effectively inherits a fixed constraint at

that point.

Figure 6

–

12

Main members of the truss.

7.

Next, create a series of connected lines as shown in

Figure 6

–

13

to

approximate the interior bracing of the truss.

Figure 6

–

13

Rough layout of interior members.

At this stage, the layout of the interior bracing is arbitrary and is

intended only as a rough approximation of the true shape. The

endpoints of the lines, however, must snap to the edges of the main

truss members. This is indicated in the figure by the presence of small

circles next to the intersections of the interior bracing with the main

members. Avoid creating 90

?

angles because that will introduce

unwanted additional constraints.

8.

Split the edges of the main members at the points where they intersect

the interior bracing.

9.

Dimension the vertical distance between the left endpoints of the sketch

and the horizontal distance between the reference point and the right

endpoint of the sketch, as shown in

Figure 6

–

14

. These dimensions will

act as additional constraints on the sketch. Accept the values shown in

the prompt area when creating the dimensions. These values represent

the dimensions of the part, projected from the global Cartesian

coordinate system (depicted in

Figure 6

–

11

) to the local sketch plane.

Figure 6

–

14

Dimensioned sketch.

10.

Apply parallel constraints to the segments of the top edge of the main

member, then repeat this operation for the bottom edge of the main

member. These constraints ensure that these line segments remain

colinear.

11.

To complete the sketch, recognize from

Figure 6

–

11

that the interior

bracing breaks the main members into equal length segments on both

its top and bottom edges. Thus, impose equal length constraints on the

segments of the top edge of the main member; repeat this operation for

the bottom edge of the main member. The final sketch appears as

shown in

Figure 6

–

15

.

Figure 6

–

15

Final sketch of single truss structure.

12.

Using the

Save Sketch As

tool

, save the sketch as

Truss

.

13.

Click

Done

to exit the Sketcher and to save the base feature of the part.

The other truss will also be added as a planar wire feature by projecting the

truss created here onto a new datum plane.

To define the geometry of the second truss structure:

1.

Define three datum points using offsets from the end points of the truss,

as shown in Figure 6

–

16. The offsets from the parent vertices are

indicated in the figure. You may need to rotate your sketch to see the

datum points.

Figure 6

–

16

Datum points, plane, and axis.

2.

Create a datum plane using these

three points

. As before, the points

defining the plane should be chosen in a counterclockwise order.

3.

Use the

Create Wire: Planar

tool to add a feature to the part. Select the

new d

atum plane

as the sketch plane and the datum axis created earlier

as the edge that will appear vertical and on the left of the sketch.

Note:

If the sketch plane is not oriented in the 1

–

2 plane, use

the

Views

toolbar to change to the X

–

Y view.

4.

Use the

Add Sketch

tool

to retrieve the truss sketch. Translate the

sketch by selecting the vertex at the top left end of the new truss as the

starting point of the translation vector and the datum point

labeled

P

in

Figure 6

–

16

as the endpoint of the vector. Zoom in and

rotate the view as necessary to facilitate your selections.

Note:

If the points defining either the original or new datum

plane were not selected in a counterclockwise order, you will

have to mirror the sketch before translating it. If necessary,

cancel the sketch retrieval operation, create the necessary

construction line for mirroring, and retrieve the sketch again.

5.

Click

Done

in the prompt area to exit the Sketcher.

The final truss part is shown in

Figure 6

–

17

. The visibility of all datum and

reference geometry has been suppressed.

Figure 6

–

17

Final geometry of the truss structures; highlighted vertices

indicate the locations of the pin joints.

Recall that the cross bracing must be treated as a separate part to properly

represent the pin joints between it and the trusses. The easiest way to sketch

the cross bracing, however, is to create wire features directly between the

locations of the joints in the trusses. Thus, we will adopt the following method

to create the cross bracing part: first, a copy of the truss part will be created

and the wires representing the cross brace will be added to it (we cannot use

this new part as is because the vertices at the joints are shared and, thus,

cannot represent a pin joint); then, we will use the cut feature available in

the Assembly module to perform a Boolean cut between the truss with the

cross brace and the truss without the cross brace, leaving the cross brace

geometry as a distinct part. The procedure is described in detail below.

To create the cross brace geometry:

1.

In the Model Tree, click mouse button 3 on the

Truss

item underneath

the

Parts

container and select

Copy

from the menu that appears. In

the

Part Copy

dialog box, name the new part

Truss-all

, and click

OK

.

2.

The pin locations are highlighted in

Figure 6

–

17

. Use the

Create Wire:

Point to Point

tool

. In the

Create Wire Feature

dialog box, accept

the default setting of

Chained wires

and click

Add

to add the cross

bracing geometry to the new part, as shown in

Figure 6

–

18

(the vertices

in this figure correspond to those labeled in

Figure 6

–

17

; the visibility of

the truss in

Figure 6

–

18

has been suppressed). Use the following

coordinates to specify a similar view:

Viewpoint

(1.19, 5.18, 7.89),

Up

vector

(

–

0.40, 0.76,

–

0.51).

Figure 6

–

18

Cross bracing geometry.

Tip:

If you make a mistake while connecting the cross bracing

geometry, you can delete a line using the

Delete

Feature

tool

; you cannot recover deleted features.

3.

Create an instance of each part (

Truss

and

Truss- all

).

4.

From the main menu bar of the Assembly module, select

Merge/Cut

. In the

Merge/Cut Instances

dialog box, name the new

part

Cross brace

, select

Cut geometry

in the

Operations

field, and

click

Continue

.

5.

From the

Instance List

, select

Truss-all-1

as the instance to be cut

and

Truss-1

as the instance that will make the cut.

After the cut is made, a new part named

Cross brace

is created that

contains only the cross brace geometry. The current model assembly

contains only an instance of this part; the original part instances are

suppressed by default. Since we will need to use the original truss in the

model assembly, click mouse button 3 on

Truss-1

underneath

the

Instances

container and select

Resume

from the menu that

appears to resume this part instance.

We now define the beam section properties.

Defining beam section properties

Since the material behavior in this simulation is assumed to be linear elastic, it

is more efficient from a computational point of view to precompute the beam

section properties. Assume the trusses and bracing are made of a mild

strength steel with

= 200.0

?

10

9

Pa,

= 0.25, and

= 80.0

?

10

9

Pa. All

the beams in this structure have a box-shaped cross-section.

A box- section is shown in

Figure 6

–

19

. The dimensions shown in

Figure

6

–

19

are for the main members of the two trusses in the crane. The

dimensions of the beam sections for the bracing members are shown in

Figure

6

–

20

.

Figure 6

–

19

Cross- section geometry and dimensions (in m) of the main

members.

Figure 6

–

20

Cross- section geometry and dimensions (in m) of the internal and

cross bracing members.

To define the beam section properties:

1.

In the Model Tree, double-click the

Profiles

container to create a box

profile for the main members of the truss structures; then, create a

second profile for the internal and cross bracing. Name the

profiles

MainBoxProfile

and

BraceBoxProfile

, respectively. Use the

dimensions shown in

Figure 6

–

19

and

Figure 6

–

20

to complete the

profile definitions.

2.

Create one

Beam

section for the main members of the truss structures

and one for the internal and cross bracing. Name the

sections

MainMemberSection

and

BracingSection

, respectively.

a.

For both section definitions, specify that section integration will

be performed before the analysis. When this type of section

integration is chosen, material properties are defined as part of

the section definition rather than in a separate material definition.

b.

Choose

MainBoxProfile

for the main members' section definition,

and

BraceBoxProfile

for the bracing section definition.

c.

Click the

Basic

tab, and enter the Young's and shear moduli

noted earlier in the appropriate fields of the data table.

d.

Enter the

Section Poisson's ratio

in the appropriate text field of

the

Edit Beam Section

dialog box.

3.

Assign

MainMemberSection

to the geometry regions representing the

main members of the trusses and

BracingSection

to the regions

representing the internal and cross bracing members. Use the

Part

list

located in the context bar to retrieve each part. You can ignore

the

Truss- all

part since it is no longer needed.

Defining beam section orientations

The beam section axes for the main members should be oriented such that the

beam 1-axis is orthogonal to the plane of the truss structures shown in the

elevation view (

Figure 6

–

11

) and the beam 2-axis is orthogonal to the

elements in that plane. The approximate

-vector for the internal truss

bracing is the same as for the main members of the respective truss

structures.

In its local coordinate system, the

Truss

part is oriented as shown in

Figure

6

–

21

.

Figure 6

–

21

Orientation of the truss in its local coordinate system.

From the main menu bar of the Property module, select

Assign

Beam

Section Orientation

to specify an approximate

-vector for each truss

structure. As noted earlier, the direction of this vector should be orthogonal to

the plane of the truss. Thus, for truss B, the approximate

= (

–

0.1118, 0.0,

0.9936); while for the other truss structure (truss A), the approximate

=

(

–

0.1118, 0.0,

–

0.9936).

You may want to check that your beam sections and orientations are correct.

From the main menu bar, select

View

Part Display Options

and toggle

on

Render beam profiles

to see a graphical representation of the beam

profile. Toggle off

Render beam profiles

before continuing with the rest of the

example. This functionality is also available in the Visualization module

through the

ODB Display Options

dialog box.

From the main menu bar, select

Assign

Element Tangent

to specify the

beam tangent directions. Flip the tangent directions as necessary so that they

appear as shown in

Figure 6

–

22

.

Figure 6

–

22

Beam tangent directions.