Top -
Down Design
PART
B
Before we copy our reference geometry make sure the Model Tree
displays the features of assembled components. 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. Display all features of the Skeleton model by clicking on the plus sign to the left of the
model name in the Model Tree.
Step #6: Copy Geometry to components
First
we do the CRANK-SHAFT:
We work in the assembly. Select the CRANK-SHAFT in the Model Tree and right-click it. From the pop-up window select Activate and
then Insert – Shared Data – Copy Geometry….
The dashboard for this feature is now displayed.
Select in the Model Tree from the Skeleton
Model the Publish Geometry feature we called PUB_GEOM_CRANK and finish by clicking on the Check-icon in the dashboard. Since this is not an empty
part, but has features already built. We find the Copied Geometry is located at the very end of the Model Tree.
Drag it upwards to the datum features as far as it will go; just below the RIGHT datum plane. Next drag the RIGHT datum plane below the Copy Geometry feature and also drag the ALIGNMNT_DTM feature just below the RIGHT datum. Next perform following steps:
· Redefine the ALIGNMNT_DTM datum. Right-click the feature and select Edit
Definition.
In the Datum
Plane window Delete the Offset definition. Select the copied geometry for
the Crank and in the Datum Plane
window set it to Through and add also the CRANK_SHAFT axis, set to Normal. Done, click OK. Now drag the RIGHT
datum feature below the ALIGNMNT_DTM in the Model Tree.
· Redefine the RIGHT
datum. Right-click the feature and select Edit
Definition.
Select the ALIGNMNT_DTM and specify an offset of +5.5mm. Done, click OK.
· As before redefine TOP
datum. Again use the line segment for Crank
set to Normal and CRANK_SHAFT axis,
set to Through.
· Finally redefine FRONT
datum. Use again the line segment for Crank
set to Through and CRANK_SHAFT axis,
set to Through.
· Delete the PRT_CSYS_DEF coordinate system and recreate it based on the Crank line-segment and
the CRANK_SHAFT axis. Do not forget to rename the default name and
drag it below the FRONT datum in the Model Tree.
· Reactivate the assembly and regenerate it.
Next we
do the ROD:
Repeat above procedure for the ROD. Select the Publish
Geometry named PUB_GEOM_ROD.
We find the Copied Geometry is located below the coordinate system in the Model Tree.
Drag it upwards to the top, as far as it will go; just below the RIGHT datum plane. Next drag the RIGHT datum plane below the Copy Geometry feature and then
perform following steps:
· Again we redefine the RIGHT datum. Right-click the feature and select Edit
Definition.
Select the copied geometry for the Rod and in the Datum Plane
window set it to Through and add also the CRANK_PIN axis, set to Normal. Done, click OK.
· Similarly redefine TOP
datum. Again use the line segment for Rod,
set to Normal and CRANK_PIN axis, set
to Through.
· Finally redefine FRONT
datum. Use again the line segment for Rod,
set to Through and CRANK_PIN axis, set
to Through.
· Delete the PRT_CSYS_DEF coordinate system and recreate it based on the Rod line segment and
the CRANK_PIN axis. (Do not forget to rename the default name.)
· Reactivate the assembly and regenerate it. This will
fail, because the original placement was based on the old csys of this component. We are now able to use Published Geometry to place the Rod properly into the Assembly. In the new window Menu Manager
select:
Fix Model – Component – Confirm | Redefine – Failed Feat
Now in the Dashboard click on Placement and Delete the Placement Set and a New Set will open; align the Rod CRANK_PIN axis with the Crank-Shaft
CRANK_PIN axis. And as a New Constraint align the Rod RIGHT
datum with the Crank-Shaft ALIGNMNT_DTM. Now add as a further Constraint aligning the Rod
PISTON_PIN axis with the Skeleton
PISTON_PIN axis. Click Check and now back in the Menu
Manager window select Done/Return,
you must first scroll down by clicking on the inverted triangle. And finally
click on Yes.
Finally,
we do the PISTON:
Again we repeat above procedure. Here the Publish Geometry
feature is called PUB_GEOM_PISTON.
· We redefine the RIGHT
datum. Right-click the feature and select Edit
Definition.
Select the copied geometry for the Piston and in the Datum Plane
window set it to Through and add also the CYLINDER axis, set to Through. Done, click OK.
· Similarly redefine TOP
datum. Again use the line segment for Piston,
set to Normal and PISTON_PIN axis,
set to Through.
· Finally redefine FRONT
datum. Select the CYLINDER axis, set
to Through and PISTON_PIN axis, set to Through.
· Delete the PRT_CSYS_DEF coordinate system and recreate it based on the CYLINDER and the PISTON_PIN
axes. (Do not forget to rename the default name.)
· Reactivate the assembly and regenerate it. This again
will fail, because the original placement was also based on the old csys of this component. Again we are now able to use Published Geometry to place the Piston properly into the Assembly. In the new window Menu Manager
select:
Fix Model – Component – Confirm | Redefine – Failed Feat
Now in the Dashboard click Placement and Delete the Placement Set and a New Set will open; align the Piston CYLINDER axis with the Skeleton
CYLINDER axis. And as a New Constraint align the Piston PISTON_PIN axis with the Rod
PISTON_PIN axis. Click Check and now back in the Menu
Manager window select Done/Return,
you must first scroll down by clicking on the inverted triangle. And finally
click on Yes.
Save the assembly file to transfer the work to all the
component files.
To transfer
the shared geometry to all the component files you must first save the
assembly. We now have all references one needs to completely build all the
important parts of the assembly in part
mode.
Important Note:
When in part-mode and
creating features, while entering the Sketcher do not forget to select copied
geometry as references.
Step #7: Complete CRANK SHAFT in Part
Mode:
This part needs special attention because it has all
its geometry already built. We open the CRANK-SHAFT part in a separate window and verify the Copy Geometry feature is at the top of the Model Tree. See
Figure
5 below.
· We redefine the Crank protrusion. Right-click the
feature and select:
Edit
Definition – Placement – Edit…
Sketch
– References…
The References window pops
up. Select in graphics window the blue line segment forming the copied geometry
for the Crank and next the CRANK_PIN axes also. Verify that they appear in the References window.
The circle will not be at its proper location. Make
the center of circle coincident with the end point of the line segment from the
copied geometry. You will need to delete the position dimension of the circle
center ( 12.5mm ) See Figure 6 below for more details. Exit Sketcher and in the
Dashboard verify the feature build direction is as intended. Correct it, if
necessary and then exit by clicking Check-icon.
· Finally, verify the offset direction of ALIGNMNT_DTM datum is still as intended? Regenerate and save the
part. The part as now modified will adapt properly to any changes made to the
Skeleton model.
|
Figure 5 |
Figure 6
Redefining Crank Protrusion Location |
Note: You will find complete drawings of our three
parts on the ENGN1740 website via the Project Link.
Step #8: Complete PISTON in Part Mode:
This is still an empty part. All its geometry will
have to be built. Open the PISTON part and
verify the Copy
Geometry feature is in the Model Tree.
· We will now build the base-feature which is a cylinder
in the standard way. Use RIGHT as the Sketching
plane, select the Revolve tool.
When entering the Sketcher select for References
the blue line segment forming the copied geometry for the Piston, also the PISTON_PIN and CYLINDER axes.
Create a vertical center line coincident with the
y-axis and now use the Rectangle tool and create a rectangle which has one side
coinciding with the reference line segment and the other side with the central
axis. Make certain no dimensions are automatically created. None are required!
If you see any, delete your profile and start again. Exit and complete the
feature in the regular way.
· Next we make the hole for the piston pin. Select the RIGHT datum and pick the Hole tool.
Primary Reference:
RIGHT datum
Type: Simple Coaxial Diameter:
6
Secondary Reference: PISTON_PIN axis
Extrude in Both
directions Blind a total distance of 45.
· Convert part into a shell. Remove bottom face. Note
the part has a non-uniform wall thickness. The piston top has a thickness of 4, the rest is 1.5mm thick.
· Round the shell’s inside edges with a 1.5 radius.
· Make 11mm wide cut in inner boss to accommodate rod.
· Make circular cut for piston ring.
· Finish with several chamfers and the round 0.5mm. Save the
finished part.
Step #9: Complete ROD in Part Mode:
This is again an empty part. All its geometry will
have to be built. Open the ROD part and verify
the Copy
Geometry feature is in the Model Tree.
· We will now build the base-feature which is a linear
extrusion. Use RIGHT as the Sketching
plane, select the Extrude tool.
When entering the Sketcher select for References
the blue line segment forming the copied geometry for the Rod and also the CRANK_PIN axis. Use both end points of the reference geometry
line segment to snap the circles for sketching the profile. The large circle is
at the end which meets the CRANK_PIN axis.
Complete in the usual way. Extrude symmetrically in both directions a total of 10mm.
· Make a blind cut on one face. Make sure your
dimensions for the Cutting profile is based on references to the base-feature.
· Now mirror the cut onto the other face.
· Complete part by adding Rounds and Chamfers. Save the
finished part.
See below a view of the completed assembly.
Figure
7 Compressor Assembly