Top -
Down Design
PART
A
Introduction
Top down design means many things. The main thing is
that you begin designing your project while
in the assembly. This means you are creating component
parts and subassemblies relative to each other in the assembly. Sometimes external references are
created between components in the assembly to satisfy design intent. Sometimes
geometry is copied from one part to another so more than one user can work on
the assembly at the same time. Often a 'skeleton' model is used to capture
critical design intent and other information about the assembly. This 'top
level' information is passed 'down' to the components of the assembly, thus the
term 'top‑down'. This method of assembly design is a powerful way to
control and benefit from the associative and parametric nature of Pro/ENGINEER.
The Skeleton Model
As mentioned above, often a 'skeleton' part is used to
define the original design intent of the design. This part usually contains
datum geometry such as planes and curves to define the design intent. Kinematic
motion can be applied to this model along with other design criteria needed for
the design. In 2D CAD, a design was often started as a 'layout'. The 3D
skeleton model serves this same purpose, to 'layout' the design before creating
any solids. The skeleton should contain important design information that will
be copied to the necessary components of the assembly. Furthermore, the
skeleton model is very efficient because it contains minimum solid geometry. All
this allows a designer to control a large assembly without the overhead of
always having the assembly in session. Because the skeleton regenerates
quickly, changes to the design can easily be accomplished, and regeneration of
the assembly can be delayed until absolutely necessary. All this allows a
designer to control a large assembly without the overhead of always having the
assembly in session. Because the skeleton regenerates quickly, changes to the
design can easily be accomplished, and regeneration of the assembly can be
delayed until absolutely necessary. Skeleton parts can be excluded from mass
property calculations and bill of material reports. An assembly model can have
only one skeleton, and it must be the first component of the assembly. Skeletons
can be excluded from drawing views and in simplified representations of the
assembly. Assembly features cannot intersect the skeleton part, even if the
skeleton part has solid features present.
We will use our Compressor project, a
piston rod crank assembly, to demonstrate the concept. This example
consists of one top-level skeleton model that will drive the dimensions and
orientation of the principle components of the assembly. It is sometimes
practical to break up the datum features into two or more PublishGeom features. A
great deal of forethought is required and it may often become necessary to go
back to the skeleton models to add more information for the positioning,
orientation, etc., of components later on.
Procedure
The procedure is to build the assembly structure using
mostly empty parts in our assembly initially. Only the crank-shaft exists at
this point. Before starting with the assembly we need to make one important
part containing the reference, or layout geometry.
It is
important that all files of the Top-Down Design project are in one and the same
directory folder. After starting Pro/E set the working directory to the Project-folder.
Step #1: Create the Assembly file
First we can create our assembly file. This is similar
to creating a part file, but we select Assembly
as the Type. Name it COMP_ASMB. Do not forget to use the appropriate start template
file.
Step #2: Create the Skeleton Part in the Assembly
Use Create component in assembly mode tool for the Skeleton part.
In Component Create window select the Skeleton
Model type. You must accept the
default name of COMP_ASMB_SKEL, and in the Creation Options window use Copy
From Existing and brows to select skl_mmns.prt as
the start template; click OK. Now you
will see the skeleton model as the first component in the assembly. You must save the assembly now to actually
create the skeleton model part file.
|
Figure 1
Skeleton Model Geometry |
Figure
2 Skeleton Model Feature Tree Figure 1 on the left shows simple datum curve features
representing the principal components reference geometry. |
Above the Model Tree
click on Model Tree Settings Tree Filter, in the Model Tree Items window under Display
check Features and Suppressed Objects. Next, click OK or Apply.
Notice the place where the skeleton part is located in
the model tree. It is put at the very beginning right after the assembly part
and before the datum planes.
Step #3: Modify the COMP_ASMB_SKEL part in Part Mode
To complete the skeleton part we open the COMP_ASMB_SKEL part in its own separate window. First verify
assembly components are able to copy its skeleton features. Edit Setup Ref Control | Accessible must be set to All, or at least to Skeleton
Model.
Figure 2 above
shows the Model
Tree of the completed COMP_ASMB_SKEL. The datum curves and the axes, additional datum
plane and local coordinate systems have been created. At the very end are the Published Geometry
features. For a picture of the completed part see Figure 3 below. Note: There will be no COMP_ASMB_SKEL part to open unless you have saved your assembly
first. Now perform the following steps:
·
To create our
reference geometry we first select the RIGHT datum plane and use the Sketch tool to
create the Datum line segments, as shown in Figure
1. Use the Sketch tool to first draw
only the line segment of the crank and exit it. Repeat the tool and draw next
the lines for both, the rod and the cylinder. To draw the Rod segment first create a Sketcher reference of the Crank end-point. In the Model Tree
change the names to CRANK
and ROD_PISTON.
·
Add a Datum axis at the intersection of TOP
and FRONT. Call it CRANK_SHAFT.
·
Create a Datum axis at the point of intersection between the crank and
rod line segments. The new axis is parallel to the global x-axis. Call it CRANK_PIN.
·
Create a Datum axis at the point of intersection between the rod line
segment and the global y-axis. The new axis is parallel to the global x-axis.
Call it PISTON_PIN.
·
Add a Datum axis at the intersection of FRONT and RIGHT. Call it CYLINDER.
·
For placement of
the cylinder-head part add an Offset Datum plane.
Offset distance is 76 from the TOP
datum. Call it CYL_HEAD.
·
Add a relation:
The Offset
Dimension for the CYL_HEAD_DTM is equal to the sum of the Crank Radius plus the Rod
Length and cylinder top surface offset. See our lay-out sketch for our
relation defining the location of the Cylinder_Head Datum.
If we want to
assemble empty parts (parts without any actual geometry) and this assembly is
to simulate kinematic motion, we need to define local coordinate systems for
each of the moving components in order to properly assemble them. We will place
the local coordinate systems on the datum curves in the skeleton part. When the
datum curves change location the coordinate systems will reorient themselves
accordingly.
Adding Local Coordinate Systems
·
The first
coordinate system is created for the piston at the top end of the connecting
rod and will have the same orientation as the global Csys.
Use the Datum Coordinate
System tool. The Coordinate System window pops up. When in the Origin-tab section select in the graphics window the upper
end point of the line segment forming the rod. Next select the Orientation-tab and click in the first Use
to determine X field and pick the SKL_RIGHT datum plane, now select the next Use
to project Y field and pick SKL_TOP
datum plane. Click OK and the new coordinate system has been created.
Verify proper orientation of the three axes. If one needs to correct the triads
orientation use Flip and/or select different axes by clicking the down arrow
button. Change its name to Piston_CS.
·
The next
coordinate system we will create is for the connecting rod at the joint with
the crank. Its y-axis will need to be aligned with the line segment forming the
rod.
Again use the Datum
Coordinate System tool. Select the
vertex between the crank and connecting rod. In the Orientation-tab click in the first Use
field and select the SKL_RIGHT datum plane; click in the next Use field and select the datum curve forming the rod.
Click OK and this Csys is now created. Change its name to Rod_CS.
·
The final
coordinate system is located at the same position as the global coordinate
system, but is aligned with the line segment representing the crank. Proceed as
before, but remember its y-axis will need to be aligned with the line segment
forming the crank. Change its name to Crank_CS.
·
Save this part. (COMP_ASSMB_SKEL)
|
Figure 3 Completed
Skeleton Model |
Figure
4 |
Adding
Publishe Geomtry Features
First we create this feature for the Crank: Insert Sharde Data
Publish Geometry
·
Select the Reference tab and click in the text window under Chain. Now in the graphics window select the line segment
representing the crank. Next activate
the text window under References. Now select the two axes, CRANK_SHAFT and CRANK_PIN. Finally,
under the Properties tab change the name to PUB_GEOM_CRANK and save it by clicking on the Check-icon.
·
Repeat procedure
for the Rod: Chain - select line
segment for the rod. References - CRANK_PIN
and PISTON_PIN. Name - PUB_GEOM_ROD.
·
Once more for the
Piston: Chain - select line segment for the piston. References - CYLINDER
and PISTON_PIN. Name - PUB_GEOM_PISTON.
This completes the modifications to the skeleton
model. Save the file and close this window. Next we will again work in the
assembly, but before that we need to get the crank-shaft part file.
Step #4: Add CRANK-SHAFT to assembly
This part has already been built as HW#2, but it is
best to use a known version. Use fetch_proe
09CRANK-SHAFT.PRT to fetch it from
the server. Open it and then we need to create in the part an offset datum plane
to enable us to properly align it in the assembly. Add a Datum plane, call it ALIGNMNT_DTM and offset it -5.5mm from RIGHT datum. Now we
use Save a Copy
to save it into the Project folder as CRANK-SHAFT.PRT.
Make the assembly window active and note all changes
we have made to the skeleton part have been updated here. Use Add Component to assembly tool and select the Crank-Shaft part.
·
Now align part
crank-shaft axis to assembly axis called CRANK_SHAFT.
·
Next align part
crank-pin axis to assembly axis called CRANK_PIN.
·
Finally add a New Constraint and align part ALIGNMNT_DTM plane with SKL_RIGHT datum.
Step #5: Create ROD in assembly
Use Create component in assembly mode tool
for the ROD
part.
In Component Create window select Part and Solid. In the Name field type ROD and click OK. Use our standard part template to create each
part. Assemble by aligning part csys to Assembly Rod_CS csys.
Step #6: Create PISTON in assembly
Similar to Step #5 create the PISTON
part and assemble to Piston_CS csys.
Figure 4 above shows the Assembly Model
Tree with all currently assembled
components.
Now save the assembly once more!
Remember any changes and additions in the assembly
will not propagate to the individual part files unless the Assembly is first
saved!
See Top-Down Design PART B for the
continuation of the procedure.
Skeleton
Model Layout
Offset Datum Plane for Cylinder Head
P
O
= 12
20
Length = 76
(temporarily)
rod length R
Relations:
Length = C + R+ O
45o
crank C
Initial Layout Dimensions:
|
Initial |
Crank C |
Rod R |
Piston Radius P |
|
Layout |
12 |
38 |
18 |