Mechanisms and
Motion
In Pro/ENGINEER
a Mechanism is an assembly with two or more components. The components of this
assembly are connected in such a way as to have some degree of freedom to
permit motion. These connections define the degrees of freedom of one
body with respect to the body(ies) it is being assembled to. Mechanism
Design may then be used to study the motion of the mechanism
kinematically. Mechanism Design can also check for interferences, which
may occur between components in the range of motion of the mechanism.
Mechanism
Connection types and their required References:
|
Connection Type |
References Required at Part Level |
References Required at Assembly Level |
|
Pin |
- Axis |
- Axis |
|
Slider |
- Axis |
- Axis |
|
Cylindrical |
- Axis |
- Axis |
|
Ball |
- Point |
- Point |
|
Planar |
- Planar Surface |
- Planar Surface |
|
Bearing |
- Point |
- Point |
|
Connection Type |
DOF |
Description |
|
|
|
Rotation |
Translation |
|
|
Pin |
1 |
0 |
Rotates about an axis. |
|
Slider |
0 |
1 |
Translates along an axis |
|
Cylinder |
1 |
1 |
Translation along and rotation about a specific axis. |
|
Ball |
3 |
0 |
A "ball-in-spherical-cup" joint allows rotation in any direction. |
|
Planar |
1 |
2 |
Bodies connected by a planar joint move in a plane with respect to each other. Rotation is about an axis perpendicular to the plane. |
|
Bearing |
3 |
1 |
Combination of a ball joint and a slider joint. |
Connections differ from the traditional
Pro/ASSEMBLY approach. The primary differences are summarized below:
·
The types of
allowable placement constraints are limited based on the type of connection
being created.
·
Multiple placement
constraints are grouped together to define single connections.
·
The placement
constraints defined do not fully constrain the model. Based on the type of
connection, the component is allowed to move in specific ways.
· Multiple connections can be added to a component. This is how you could close a loop in your system. The first connection is used to place the component and the second connection is referred to as the loop connection
A completed
mechanism may be moved in two ways. One way is to select Drag tool
icon and
then select a certain component to be dragged. By moving the mouse
around, this component and the components connected to it will move according
to their connection definitions.
A mechanism may
also be moved by defining a driver with the Servo Motors
tool icon and running a
motion analysis. A motion analysis may be defined and run by selecting Run an Analyses tool – New | Run.
Drivers
prescribe the motion of a connection or component by defining their position,
velocity or acceleration. Drivers can be applied to connections, points
or planes and may be used to drive the motion of a mechanism.
The results of
a motion analysis may be played back by selecting Replay previously run analyses tool.
Mechanism Design can analyze
the results of a motion analysis to check for interferences, as the mechanism
is moving. To do this, select the appropriate interference checking
option in the Playbacks dialog box.
With
Pro/MECHANISM we have the capability to generate motion envelopes. Motion
envelopes are entities that encompass the space of motion the mechanism moves
through.
To create a
motion envelope, run a Motion study. Select from the Playbacks window Export results to
an *FRA file icon.
This will create necessary frames file. Upon returning from Mechanism
select File – Save a Copy… and select as Type
Motion Envlp. Select the Frames file when prompted.
Set the quality level of the envelope. Higher quality require longer generation
time. Finally select Preview
or Create. When Create
is selected, the envelope will be save as a Pro/ENGINEER part file.
An Example
As an example
we will use the Compressor Assembly we have built recently. Load this file into
Pro/E and select Mechanism
from the Applications
pull-down menu. Next select View
– Highlight Bodies. Notice all of the assembly is
highlighted in green indicating all parts are rigidly connected to ground since
we have used the default connection type, which is Fixed.
This model can’t be made into a Mechanism
without changing all placement constraints in the assembly. Return to standard
Pro/E by selecting Applications
– Standard. To preserve our existing assembly with
our Top-Down relations and geometric links, we will first create a sub-folder
and place a copy of our assembly into it. All required modifications will then
be performed in that folder. This is an important step, follow it carefully.
File
– Save a Copy… and create a new sub-folder Motion
by pulling down from Organize
and selecting New
Folder. Name the copy of our assembly Compr_M
and
click OK.
In the new window Assembly Save a Copy
enter _M
into the Use Suffix text area. Now
select all the components in the Tree-window
on the left and then click the Generate New Names button to the
right of the Suffix–window. This
will rename the components with the _M
suffix. Click OK.
We now have a renamed assembly in a sub-folder called Motion. Use Set Working Directory…
to go to this sub-folder. Do a Close
Window and erase Not Displayed…. Now we open
the new assembly file Compr_M.
To convert this
model into a Mechanism the model
needs to be redefined with Mechanism
Design Connections. First verify the Model Tree and
if necessary move the components so that they are in the following order: CRANK-SHAFT_M,
ROD_M,
PISTON_M,
PISTON-RING_M and PISTON-PIN_M.
Since our Top-Down design
concept is based on Copied Geometry
in fixed positions based on our skeleton model we need to break the dependency
of the copied geometry in each part before we can make our new connections. In
the assembly Model Tree expand CRANK-SHAFT_M part and right-click Copy
Geometry, select
Edit Definition. In the Dashboard click on Options and in pop-up window
uncheck the Dependent box and exit by clicking
the Check button on the right. Repeat
these steps for the COPY GEOMETRY features of ROD_M, PISTON_M,
PISTON-RING_M and
PISTON-PIN_M
also. We will now suppress the two parts, PISTON-RING_M and
PISTON-PIN_M.
Next save the assembly.
Redoing the
connection definitions:
Select the CRANK-SHAFT_M part in the Model Tree,
right-click it and then select Edit Definition. The regular "Component
Placement"
Dashboard will appear with our regular constraints. Click on Placement to open up this window. We
need to delete the alignment constraint for the crank-shaft Crank-pin axis. Next uncheck the Allow Assumptions box, this will enable the Convert constraints to Mechanism
connection
icon, click it. Notice the connection type converts to Pin and the Status
becomes Connection
Definition is Complete. Click on Check to exit the Dashboard. The
component is now placed in the assembly to freely rotate around the Crank-shaft axis. See figures below for
details.
|
Deleting Crank-pin alignment constraint |
Uncheck Allow Assumptions |
|
Conver Constraints to Mechanism connection |
The three figures, above and to the left show the
completed axial and translational alignment for the Crank-shaft. When the Placement Status indicates ‘Connection
Definition Complete’ exit the Dashboard
by clicking the Check icon on the right. Notice also in the Model Tree an
open square to the left of CRANK-SHAFT_M
indicating a mechanism connection. The connection has some degree of freedom,
it is able to move. |
Repeat the process for ROD_M aligning it with the crank pin axis. As Translation reference use the component RIGHT datum on ROD_M and the CRANK-SHAFT_M’s ALIGNMENT_DTM datum.
Do the same with the PISTON_M, which needs to be aligned with the rod at the piston pin axis. For the PISTON_M part to function properly as a mechanism it requires also one additional connection of the Type CYLINDER constraint. Here we align the Piston’s Cylinder axis with the Cylinder axis of the skeleton part.
When all connections are completed select again Mechanism from the Applications menu. Notice all the
connection icons on the model.
To
test these connections select Edit – Connect… – Run. A
window will pop up with the following message:
"The mechanism assembly succeeded. The
requested assembly tolerance was 0.001. The actual assembly error is
1.11e-015. Do you want to accept the assembled configuration and
reposition the bodies in the database?"
If Yes
is selected, the bodies in the model will be repositioned such that the
assembly connections have been aligned according to their definition and
constraint references. If No is selected, the bodies in the model
are returned to their original position. Select Yes.
Moving the Mechanism by hand:
Select the
Drag tool
icon on right and click on the rod or crank. Now you can drag the component by
moving the mouse pointer. Click again and Done Sel to leave the mechanism in
its new position.
Moving the Mechanism with a Driver:
Select Define Servo Motors tool icon to
bring up a dialogue box named "Servo Motor Definition".
Type "crank" for the Name of the driver. Select as Driven Entity the Motion Axis called Connection_1.axis_1.
Fill out the Profile tab by
selecting Velocity as Specification, Initial Angle
= 0.00. Select Magnitude to be Constant and enter 36 as angular
velocity "A" (deg/second). The driver is now fully
defined. Select Ok to finish the
definition of this driver.
The model is now ready for a motion analysis. To
define and run a motion analysis, select tool Define
an Analyses to bring up the "Analysis Definition" dialogue box. Check that Type is set as Kinematic. Keep
all the settings in this new dialogue box as default and check under the Motor tab that
our crank moter is selected. Select Run to start the analysis. The model
display will start moving as the analysis is running. Once the model has finished running, select Ok to exit "Analyses" dialogue box. The motion analysis results are
now available for playback.
Select tool Replay previously run analyses to activate the "Playbacks" dialog box. In this dialogue
box the results set may be selected (there is only one results set in our case)
for playback, results sets may be saved for later use and results set from
before can be loaded for playback.
|
Compressor
Mechanism Showing Connections
and Driver |
Select Play Current result
set
icon. After a few seconds an "Animate" video
tool appears. Press the Play button to start the animation.
Once finished with animating the model, select Close to exit the
"Animate" video
tool. In the "Playbacks" dialogue box select Save icon to save
the results set. This way after reentering Mechanism Design with this
model at a later time the results will be available again by selecting Restore from the
"Playbacks" dialog
box without the need to run the motion analysis again. Select Close to exit the
"Playbacks" dialog
box |
