In this project you will use curves to model the profile of this part, extrude the curves then model the shafts.
You will then prepare it for use in an assembly by creating a reference set of just the solid.
Prerequisites
Create reference sets
The Dimensions of the Part (Units in m.m.)
The Methods Used in This Project to Model the Part
In this project you will
- Use basic curves (two circles and two arcs) to create the overall shape of this part.
- Trim the curves to create the finished profile.
- Extrude the profile.
- Add a boss to the larger end and the smaller end, chamfer their bottom edges, add blends to Various edges.
- Mirror the bosses and their associated features.
- Create holes through the bosses at both ends of the part.
Task 1. Begin With a Standard Metric Part File
Open the standard metric part file, standard_mm, from the project sub-directory. If you want, you can save this part file in your own directory using a name such as test_2.
The standard part file uses the following layer standards:
- Solid geometry on layers 1 through 20.
- Sketch geometry on layers 21 to 40
- Curve geometry on layers 41 to 60
- Reference geometry on layers 61 to 80
- Sheet bodies on layers 81 to 100
- Drafting objects on layers 101 to 120
Start the Modeling application.
Task 2. Planning the Construction of the Part
The finished part will look like this.
For the curved, plate-like shape of this part, you can extrude a profile made from curves.
Then you can add the bosses, blends, chamfers, and holes to finish the part.
Task 3. Prepare to Create the Profile on a Layer Reserved for Curves
You will want the profile of curves to be placed on a layer reserved for curves.
For this project, layers 41 through 60 are reserved for curves.
Change the work layer to layer 41.
Task 4. Change the View
Since you will be creating the profile on the XC-YC plane of the WCS, it would be helpful if you were looking straight "down" onto this plane.
Change the view to a TOP view.
The instructions will refer to the "top" and "bottom" of the profile (top being in the +YC direction).
Task 5. Create the Lower End of the Profile
You can use a circle to define the lower end of this profile.
Create a circle at this location.
- Choose the Basic Curves icon or choose InsertCurveBasic Curve.
- Choose the Circle icon on the Basic Curves dialog.
- In the XC field, key in 0, then Tab.
- In the YC field, key in 0, then Tab.
- In the Radius field, key in 38.
- Check all the values in the tool bar. Change any wrong values.
- Press Enter/Return.
Task 6. Define the Upper end of the Profile
You can define the upper end of this profile with a smaller circle.
Create a smaller circle above the first.
- Choose the Circle icon to start a new circle.
- In the XC field, key in 50, then Tab.
- In the YC field, key in 175 then Tab.
- In the Radius field, key in 19, then press Enter/Return.
- Fit the view.
Task 7. Create the Left Side of the Profile
There is an arc tangent to each circle that defines the left side of this profile.
You decide that you will create both arcs, then trim later to create the finished profile.
Create a fillet that is tangent between the two circles. Be sure the fillet will not trim the circles as you create it.
If the system does not construct this fillet the way you want it, Undo it and try again with slightly different
selection points on each circle.
? Choose the Fillet icon.
? Choose the 2 Curve Fillet icon on the Curve Fillet dialog.
? Turn both trim options off.
? In the Radius field, key in 130.
? Select the upper left side of the top circle (avoiding control points).
? Select the lower left side of the bottom circle.
? For the approximate center of this fillet, indicate between the two circles.
Task 8. Create the Right Side of the Profile
The arc on the right side will complete the basic shape of this profile.
Use the same method to ceate a fillet that is tangent between the right side of the two circles.
? In the Radius field of the Curve Fillet dialog, key in 115.
? Select the lower right side of the top circle (about where you would expect the tangency to appear).
? Select the upper right side of the bottom circle.
? For the approximate center of this fillet, indicate between and to the right of the two circles.
Task 9. Trim the Upper Circle
Now you are ready to trim away the section of the circle you don't need.
Trim the top circle to the two arcs (fillets).
- Be sure that you will trim bounding objects.
? Choose Back on the Curve Fillet dialog.
? Choose the Trim icon on the Basic Curves dialog.
? Be sure that the Trim Bounding Objects option is on.
? On the Trim Curve dialog, be sure the selection step is set to First Bounding Object.
? For the first bounding object (working in a counter clockwise direction), select the upper end of the right arc (fillet).
? Be sure the selection step has changed to Second Bounding Object.
? For the second bounding object, select the upper end of the left arc (fillet).
? Be sure the selection step has changed to String to Trim.
? For the string to trim, select the lower left side of the smaller circle.
Task 10. Trim the Lower Circle
You can do the same thing on the bottom circle.
Trim the bottom circle to the two arcs (fillets).
? Choose Back on the Trim Curve dialog.
? Choose the Trim icon on the Basic Curves dialog.
? For the first bounding object (working counter clockwise), select the lower end of the left arc (fillet).
? For the second bounding object, select the lower end of the right arc (fillet).
? For the string to trim, select the upper left side of the larger circle.
This completes the profile.
Task 11. Change the View and the Work Layer
You are ready to create the plate-like solid portion of this part.
This means that you will want to have the solid on a layer reserved for solids. For this project layers 1
through 20 are reserved for solid geometry.
Change the work layer to layer 1.
Replace the current view with a trimetric view.
Task 12. Create the Curved Plate
Eventually the part will consist of a curved plate (extruded from the profile), bosses, chamfers, blends and
holes.
Your next task, then, is to extrude the profile you have just completed.
Extrude the profile this distance and direction.
? Choose the Extruded Body icon from the Form Feature toolbar or choose InsertForm Feature
Extrude.
? Select all the curves in the profile (use Chain Curves.
? When the whole profile is highlighted, OK the Extruded Body dialog.
? Choose the Direction, Distance option.
? If the direction arrow points upward from the profile, choose OK to accept the default direction.
Otherwise reverse the default direction.
? For the Start Distance, use zero.
? For the End Distance, use 18.
? Use zero for the offset and taper values.
? OK the dialog.
Task 13. Display Only the Solid
For your work on the solid, you won't want the curves to be displayed.
Make the layer with the curves, layer 41, Invisible.
Optional: Change the view to show Gray Thin Hidden Edges.
Task 14. Planning the Next Construction Steps
Eventually you will need to have these bosses on the curved plate (each with a hole completely through it). You have decided that you will create the large and small bosses first, add the blends and chamfers, then mirror both bosses (and their associated features) to the lower face of the plate.
Task 15. Create a Boss at the Large End of the Plate
Create this boss on the top face of the plate at its larger end.
The position of the boss is coincident with the arc center of the rounded end of the plate.
? Choose the Boss icon from the Form Feature tool bar or choose InsertForm FeatureBoss.
? Select the top face of the solid near the larger end.
? On the Boss dialog, in the Diameter field, key in 60.
? In the Height field, key in 25.
? Use a zero taper angle.
? OK the dialog.
? On the Positioning dialog, choose the Point Onto Point icon.
? Select the top, front edge of this end of the plate
? On the Set Arc Position dialog, choose Arc Center.
Task 16. Create the Boss at the Small End of the Plate
Create this boss on the top face of the plate at its smaller end. Its position is coincident with the arc center of this end of the plate.
? Select the top face of the solid near the smaller end.
? For the Diameter, key in 25.
? For the Height, key in 18.
? Use a zero taper angle.
? OK the dialog.
? On the Positioning dialog, choose the Point Onto Point icon.
? Select the top, rounded edge of this end of the plate.
? On the Set Arc Position dialog, choose Arc Center.
Task 17. Blend the Bottom Edges of Both Bosses
When you mirror the bosses, you will want to mirror any blends with them.
Blend the bottom edges of both bosses.
? Choose the Edge Blend icon from the Feature Operation tool bar or choose InsertFeature
OperationEdge Blend.
? In the Default Radius field, key in 4.
? Select the bottom edge of each boss.
? OK the dialog.
Task 18. Chamfer the Top Edges of the Bosses
You will also want to chamfer the top edge of each boss so that it, too, will be included in the mirror operation.
Create a chamfer on the top edge of each boss.
? Choose the Edge Chamfer icon from the Feature Operation tool bar or choose Insert Feature
OperationChamfer.
? On the Chamfer dialog, choose the Single Offset option.
? Select the top edge of each boss.
? OK the dialog.
? In the Offset field, key in 2.
? OK the dialog.
Task 19. Blend the Top Edge of the Plate
You must also blend some edges. You can begin with the top edge of the plate.
Blend all of the top edge of the plate.
? Choose the Edge Blend icon from the Feature Operation tool bar or choose InsertFeature
OperationEdge Blend.
? In the Default Radius field, key in 2.
? Turn the Add Tangent Edges option on.
? Select anywhere along the top edge of the plate.
? Apply the dialog.
Task 20. Blend the Bottom Edge of the Plate
The bottom edge of the plate must also be blended.
Blend the bottom edge of the plate.
? Be sure the radius is 2 mm.
? Be sure the Turn the Add Tangent Edges option on.
? Select anywhere along the bottom edge of the plate. OK the dialog.
Task 21. Preparing to Mirror the Bosses and Their Associated Features
In order to mirror all of the bosses, blends, chamfers, you will need to have a mirror plane.
You feel that a datum plane constructed between the top and bottom face of the plate would be a good way to provide one.
You will want to place this reference feature on a layer reserved for them.
Change the work layer to layer 61.
Create a datum plane that is centered between the top and bottom faces of the plate.
? Choose the Datum Plane icon from the Form Feature tool bar or choose InsertForm Feature
Datum Plane.
? Optional: Set the Filter to Face.
Select the top face of the plate, then the bottom face.
? Be sure the constraints are Center Plane and Parallel Plane.
? OK the dialog.
Task 22. Mirror the Bosses Along With Their Associated Features
Change the work layer back to layer 1.
Mirror the two bosses and all the blends and chamfers associated with those bosses.
? Choose the Instance Feature icon from the Feature Operation tool bar or choose InsertFeature OperationInstance.
? On the Instance dialog, choose the Mirror Feature option.
? On the Mirror Feature dialog, be sure the Feature To Mirror selection step is highlighted.
? In the Features in Part list box, choose the features you want to mirror (use Shift+MB1, select the
first and last features you need).
Choose the Add arrow to move the selected features into the Features in Mirror list box.
? Choose the Mirror Plane selection step icon (use MB2).
? For the mirror plane, select the datum plane.
? OK the dialog.
Task 23. Create a Hole Through the Bosses at the Large End
You need a hole through the bosses at each end of this part.
Create a hole all the way through the upper and lower bosses (and the plate) at the larger end.
? Choose the Hole icon from the Form Feature tool bar or choose InsertForm FeatureHole.
? Choose the Simple icon.
? For the placement face, select the top face of the larger boss on the top of the plate.
? For the thru face, select the lowest face of the larger boss on the bottom of the plate.
? For the Diameter, key in 45.
? OK the Hole dialog.
? On the Positioning dialog, choose the Point Onto Point option.
? For the target object, select the inner edge of the chamfer on the top boss.
? On the Set Arc Position dialog, choose Arc Center.
Task 24. Create a Hole Through the Bosses at the Small End
You also need a hole all the way through the smaller bosses.
Create another hole all the way through the bosses (and the plate) at the smaller end of this part.
? Be sure the Hole dialog is up.
? For the placement face, select the top face of the smaller boss.
? For the thru face, select the lower face of the smaller boss on the bottom of the plate.
? For the Diameter, key in 16
? On the Positioning dialog, choose the Point Onto Point icon.
? For the target object, select the inner edge of the chamfer on the top boss.
? On the Set Arc Position dialog, choose Arc Center.
Task 25. Create a Reference Set
Since this part will be added to an assembly, you will want to include a reference set in the part file that includes only the solid, not the datum plane
In this company, the standard reference set name for solids is "SOLID".
Create a reference set named SOLID. Add to it only the solid body.
? Choose AssembliesReference Sets.
? Choose the Create icon.
? On the Create Reference Set dialog, key in the name, SOLID.
? OK the dialog.
? Select the solid body (check the Status Line).
? OK the Class Selection dialog.
? Cancel the Reference Sets dialog.
For any clarifications and suggestions,please contact me at any time.
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