This exercise was carried out with version 27.0 (Vertex 2021).
Table of Contents
In this exercise you will learn to
A 32-tooth blade circular saw blade with a frame and separate carbide blades (an assembly) is modeled. Every other tooth is right-handed and every other tooth is left-handed.
Add a series of polar features and polar parts.
Simple assembly creation.
Creating a pattern of part using the feature pattern from the part.
Enter the label (which is also the name of the model and by default will be the name of the drawing).
Enter the archive information by clickingArc.Data.
Select the project for model.
OK.
Model the circular saw blade body
New Sketch > To vertical (XZ) plane.
Sketch the shape
Sketch three circles, diameters 50, 220 and 236 (outermost with the line style: Guide).
Sketch a vertical line (type: Guide line) ending in a medium-sized circle (= endpoint coincident with it).
Sketch oblique lines (type Guide line) ending in a medium-sized circle (= endpoint coincident with it).
Add a symmetry constraints for oblique guide lines with respect to the vertical line.
Add an angle constraints of 22.5° between the oblique guide lines.
At the end of each guide line, sketch a section line of the guide line and add a perpendicular constraint with the line on the line. (see adjacent bottom figure)
These guide lines are used when sketching tooth frames.
Operation
Boss > Extrude.
In Both Directions
Lenght: 2.
The 22.5 ° degree comes from modeling two teeth at once in this exercise.
Model a pair of teeth
New Sketch > To vertical (XZ) plane.
If the model looks angular, adjust the setting Draft Accuracy.
You can find it on the View tab, in the Settings group
Angle tolerance: 5.
You can only adjust this value if you are not in skecth mode.
Sketch the shape
Sketch three arcs, in the figure A.
The outermost arcs begin to tangentially from the ends of the guide lines.
Sketch a polylines, in the figure B.
The line starting from the arc coincides with the guide line.
Add Equal Radius constraint for all three arcs, in the figure C.
Add Tangential constraint between lines and arcs, and between the center arc and the guide geometry, in the figure C.
Add Perpendicular constraints, in the figure D.
Add Distanceconstraints, in the figure E.
Click on the lines when you add the distance constraint 4.
Add Radius constraints, in the figure E.
Add Coincident constraint between the center of the arc and the vertical guide line, in the figure F.
Add Angle constraints, in the figure G.
If the sketch is not fully defined, then add the necessary Coincidentconstraint, in the figure H.
Close the shape, sketching the polyline, in the figure I.
Without this line, you cannot extrude.
Operation
Boss > Extrude.
In Both Directions
Lenght: 2.
Create a pattern of teeth
Select the last feature from the feature tree.
Right-click function: Feature pattern.
Polar.
Circle/direction, Number: 16.
Angle: 360 (= Default).
Radius: 25. (This does not matter much. The program draws a guide line of the given radius on the model).
OK.
Model the thermal expansion groove
New Sketch > To vertical (XZ) plane.
Sketch the shape
Sketch a circle and a polyline.
The ends of the polyline coincide with the circle.
Add Symmetryconstraint between the vertical lines and the guide line.
Use the Delete section of Line to remove a piece from the circle.
Add Dimension constraints.
Groove width: 1.
Radius: 2.
Distance: 24.
Operation
Cutout > Extrude.
In Both Directions
Thru All
Create a polar pattern from the thermal expansion groove
Select the last feature from the feature tree.
Right-click function: Feature pattern.
Polar.
Circle/direction, Number: 4.
Angle: 360 (= Default).
Radius: 25. (This does not matter much. The program draws a guide line of the given radius on the model).
Search the library for visualization material: Metals > Steel > Polished Nickel.
OK.
Save the blade body
File > Save or click or press
Create a new part (carbide tooth)
File > New > Part.
Enter the label (which is also the name of the model and by default will be the name of the drawing).
Enter the archive information by clickingArc.Data.
Select the project for the model.
OK.
Create the feature
New Sketch > To vertical (XZ) plane.
Sketch the shape
The function: Polyline.
Add the Dimension constraints, shown in the figure.
Add the Coincidentconstraints, shown in the figure.
Operation
Boss > Extrude.
In Both Directions
Lenght: 2.8.
Resize the auxiliary plane
Restore plane Vertical(XZ) Plane if it is hidden.
Select Vertical(XZ) Plane.
Right-click function: Change Size.
Enter the new size: 10.
Create the draft to the tooth (So that the blade cuts well)
Click the two faces to be drafted.
Right-click function: Draft.
Click a reference face (whose dimensions do not change)
In the Dialogue Draft.
Angle: 5.
Remove.
OK.
Draft, Remove or Add
The dimensions of the part remain at the clicked reference level.
Remove = Remove the geometry from the reference level.
Add = Add the geometry from the reference level.
Add a new configuration and give name
Add a new configuration.
Click Configurations.
Right-click function: Add Configuration.
Name the configurations.
Click the Configuration in the feature tree.
Right-click function: Properties.
Enter the name of the configuration in the menu that opens: Left-handed and other Right-handed.
OK.
Mirror the part
The function: Mirror (Mirror the whole geometry of the part).
Click to the face that acts as the mirror plane.
Deselect the dialog: Original Geometrt Stays.
OK.
Save the tooth
File > Save or click or press
Create a new assembly
File > New > Assembly.
Enter the label (which is also the name of the model and by default will be the name of the drawing).
Enter the archive information by clickingArc.Data.
Select the project for the model.
OK.
Add the blade body
Right-click function: Add > Model.
Find the model, for example, in the History > Recent branch (or under the right project).
Double-click the part.
Place this first part to the origo of the assembly
Instead of an indication, press the "Done" button (= V key of middle mouse button or Right-click function: OK.)
Use the Esc key to abort the addition of parts
If you press the V key or select the Right-click function OK, the program interrupts the addition of the selected part and asks you to select the next part to be added.
The program locks the first part in place by default, so you can't drag it.
Use a browser to add parts
The Add > Model function described above opens the so-called a model addition browser whose functions are trimmed to add parts to the assembly.
If you are using a universal browser that opens with the B key, click the part and drag it a short distance and release the mouse selection button to add the part to the assembly.
Double-clicking in the universal browser (B) does not add the part, instead it opens the model in separate window.
Add two teeth to the assembly
Right-click function: Add > Model.
Find the model, for example, in the History > Recent branch.
Click the tooth part and drag it a short distance and release the mouse selection button.
The program asks you to select a configuration.
Select the first configuration.
Select the location of the tooth.
V key return to select a new model
Click the tooth part and drag it a short distance and release the mouse selection button.
The program asks you to select a configuration
Select the second configuration.
Select the location of the tooth.
Esc (Stop adding parts).
Position the parts
Function: Coincidence (in the Ribbon).
Click the face of the body and face of tooth you want to add the considency.
Order 1) and 2) then 3) and 4).
Note that you can select the face behind the edge if the cursor is slightly outside the edge and there are no other faces under the cursor.
Add a constraints for both teeth.
OK:stop adding constraints.
Drag teeth
Click the tooth and hold down the mouse select button and drag the tooth.
The tooth slides according to constraints (as if it were moving on rails).
Place the centerline of the tooth on the centerline of the body
We can take advantage of the coincidency constraint and auxiliary levels because we extruded both the body and the tooth In both directions.
If we had not done so, then our teeth would have to be placed with a distance constraints.
Put the parts in place:
Restore the auxiliary geometry if it is hidden (G key).
First select body and tooth (Remember Ctrl key)
Right-click function: Constraints > Coinsidence.
The program stains the first part with attention color.
Click the auxiliary plane.
The program stains the second part with attention color.
Click the auxiliary plane.
The program announces: Assembly is fully defined!
Make a pattern of the first tooth
In this exercise, a teeth pattern is added to using the features pattern of the body.
Click to the first tooth, either from the model or feature tree.
Right-click function: Pattern.
In the Pattern Data dialog, change the location of the pattern: From New pattern to Fase from feature pattern.
Click on a face of feature.
The program deactivates the dialog fields (except for the Deleted field).
OK completes the pattern.
Make a pattern of the secont tooth
You can do the pattern in exactly the same way as above.
Or you can use a part in a pattern to create a new, similar pattern.
In the Pattern Data dialog, change the location of the pattern: From New pattern to Part from pattern.
The file also contains sub-models: Blade frame VX_PART10A and tooth VX_PART10B.
Exercise 10: Circular saw blade
Version compatibility
This exercise was carried out with version 27.0 (Vertex 2021).
Table of Contents
In this exercise you will learn to
A 32-tooth blade circular saw blade with a frame and separate carbide blades (i.e., an assembly) is modeled. Every other tooth is right-handed and every other tooth is left-handed.
To add a series of polar features and polar parts.
Simple assembly creation.
Creating a pattern of part using the feature pattern from the part.
Enter the label (which is also the name of the model and by default will be the name of the drawing).
Enter the archive information by clickingArc.Data.
Select the project where the model will be saved.
OK.
Model the circular saw blade body
New Sketch > To vertical (XZ) plane.
Sketch the shape
Sketch three circles, diameters 50, 220 and 236 (outermost with the line style: Guide).
Sketch a vertical line (type: Guide line) ending in a medium-sized circle (= endpoint coincident with it).
Sketch oblique lines (type Guide line) ending in a medium-sized circle (= endpoint coincident with it).
Add a symmetry constraints for oblique guide lines with respect to the vertical line.
Add an angle constraints of 22.5° between the oblique guide lines.
At the end of each guide line, sketch a section line of the guide line and add a perpendicular constraint with the line on the line. (see adjacent bottom figure)
These guide lines are used when sketching tooth frames.
(from sketch to operation selection).
Operation
Boss > Extrude.
In Both Directions
Lenght: 2.
The 22.5 ° degree comes from modeling two teeth at once in this exercise.
Model a pair of teeth
New Sketch > To vertical (XZ) plane.
If the model looks angular, adjust the setting Draft Accuracy.
You can find it on the View tab, in the Settings group
Angle tolerance: 5.
You can only adjust this value if you are not in skecth mode.
Sketch the shape
Sketch three arcs, in the figure A.
The outermost arcs begin to tangentially from the ends of the guide lines.
Sketch a polylines, in the figure B.
The line starting from the arc coincides with the guide line.
Add Equal Radius constraint for all three arcs, in the figure C.
Add Tangential constraint between lines and arcs, and between the center arc and the guide geometry, in the figure C.
Add Perpendicular constraints, in the figure D.
Add Distanceconstraints, in the figure E.
Click on the lines when you add thedistance constraint 4.
Add Radius constraints, in the figure E.
Add Coincident constraint between the center of the arc and the vertical guide line, in the figure F.
Add Angle constraints, in the figure G.
If the sketch is not fully defined, then add the necessary Coincidentconstraint, in the figure H.
Close the shape, sketching the polyline, in the figure I.
Without this line, you cannot extrude.
Operation
Boss > Extrude.
In Both Directions
Lenght: 2.
Create a pattern of teeth
Select a last feature from the feature tree.
Right-click function: Feature pattern.
Polar.
Circle/direction, Number: 16.
Angle: 360 (= Default).
Radius: 25. (This does not matter much. The program draws a guide line of the given radius on the model).
OK.
Model the thermal expansion groove
New Sketch > To vertical (XZ) plane.
Sketch the shape
Sketch a circle and a polyline.
The ends of the polyline coincide with the circle.
Add Symmetryconstraint between the vertical lines and the guide line.
Use the Delete section of Line to remove a piece from the circle.
Add Dimension constraints.
Groove width: 1.
Radius: 2.
Distance: 24.
Operation
Cutout > Extrude.
In Both Directions
Thru All
Create a polar pattern from the thermal expansion groove
Select a last feature from the feature tree.
Right-click function: Feature pattern.
Polar.
Circle/direction, Number: 4.
Angle: 360 (= Default).
Radius: 25. (This does not matter much. The program draws a guide line of the given radius on the model).
Search the library for visualization material: Metals > Steel > Polished Nickel.
OK.
Save the blade body
File > Save or click or press
Create a new part (carbide tooth)
File > New > Part.
Enter the label (which is also the name of the model and by default will be the name of the drawing).
Enter the archive information by clickingArc.Data.
Select the project where the model will be saved.
OK.
Create the feature
New Sketch > To vertical (XZ) plane.
Sketch the shape
The function: Polyline.
Add the Dimension constraints, shown in the figure.
Add the Coincidentconstraints, shown in the figure.
Operation
Boss > Extrude.
In Both Directions
Lenght: 2.8.
Resize the auxiliary plane
Restore plane Vertical(XZ) Plane if it is hidden.
Select Vertical(XZ) Plane.
Right-click function:Change Size.
Enter the new size: 10.
Create a draft to the tooth (So that the blade cuts well)
Click the two faces to be draf.
Right-click function:Draft.
Click a reference face (whose dimensions do not change)
In the Dialogue Draft.
Angle: 5.
Remove.
OK.
Draft, Remove or Add
The dimensions of the part remain at the clicked reference level.
Remove = Remove the geometry from the reference level.
Add = Add the geometry from the reference level.
Add a new configuration and enter a name for the configuration
Add a new configuration.
Click Configurations.
Right-click function: Add Configuration.
Name the configurations.
Click the Configuration in the feature tree.
Right-click function: Properties.
Enter the name of the configuration in the menu that opens. For one Left-handed and for the other Right-handed.
OK.
Mirror the part
The function: Mirror (Mirror the whole geometry of the part).
Click to the face that acts as the mirror plane.
Deselect the dialog: Original Geometrt Stays.
OK.
Save the tooth
File > Save or click or press
Create a new assembly
File > New > Assembly.
Enter the label (which is also the name of the model and by default will be the name of the drawing).
Enter the archive information by clickingArc.Data.
Select the project where the model will be saved.
OK.
Add the blade body
Right-click function: Add > Model.
Find the model, for example, in the History > Recent branch (or under the right project).
Double-click the part.
Place this first part at the origo of the assembly
Instead of an indication, press the "Done" button (= V key of middle mouse button or Right-click function: OK.)
Use the Ecs key to abort the addition of parts
If you press the V key or select the Right-click function OK, the program interrupts the addition of the selected part and asks you to select the next part to be added.
The program locks the first part in place by default, so you can't drag it.
Use a browser to add parts
The Add > Modelfunction described above opens the so-called a model addition browser whose functions are trimmed to add parts to the assembly.
If you are using a universal browser that opens with the B key, click the part and drag it a short distance and release the mouse selection button to add the part to the assembly.
Double-clicking in the universal browser (B) does not add the part, instead it opens the model.
Add two teeth to the assembly
As above or
Press B to open the universal browser.
Find the model, for example, in the History > Recentbranch.
Click the tooth part and drag it a short distance and release the mouse selection button.
The program asks you to select a configuration.
Select the first configuration.
Select the location of the tooth.
V key return to select a new model
Click the tooth part and drag it a short distance and release the mouse selection button.
The program asks you to select a configuration
Select the second configuration.
Select the location of the tooth.
Esc (Stop adding parts).
Position the parts in place
Function: Coincidence (in the Ribbon).
Click the face of the body and face of tooth you want to add the considency.
Order 1) and 2) then 3) and 4).
Note that you can select the face behind the edge if the cursor is slightly outside the edge and there are no other faces under the cursor.
Add a constraints for both teeth.
OKstops adding constraints.
Drag teeth
Click the tooth and hold down the mouse select button and drag the tooth.
The tooth slides according to constraints (as if it were moving on rails).
Place the centerline of the tooth on the centerline of the body
We can take advantage of the coincidency constraint and auxiliary levels because we extruded both the body and the tooth In both directions.
If we had not done so, then our teeth would have to be placed with a distance constraints.
Put the parts in place:
Restore the auxiliary geometry if it is hidden (G key).
First select body and tooth (Remember Ctrl key)
Right-click function: Constraints > Coinsidence.
The program stains the first part with attention color.
Click the auxiliary plane.
The program stains the second part with attention color.
Click the auxiliary plane.
The program announces: Assembly is fully defined!
Make a pattern of the first tooth
In this exercise, a teeth pattern is added to using the features pattern of the body.
Click to the first tooth, either from the model or feature tree.
Right-click function: Pattern.
In the Pattern Data dialog, change the location of the pattern: From New pattern to Fase from feature pattern.
Click on a face of feature.
The program deactivates the dialog fields (except for the Deleted field).
OK completes the pattern.
Make a pattern of the secont tooth
You can do the pattern in exactly the same way as above.
Or you can use a part in a pattern to create a new, similar pattern.
In the Pattern Data dialog, change the location of the pattern: From New pattern to Part from pattern.
