NAME: ______DATE: ______PERIOD: ___
Updated: 3-7-14WEK
ENGINEERING DESIGN W/ Solid Works
Oxford Area High School
Lesson
Miniature Machinist Vise
Machinist Vise #1
“BASE FEATURE”
You will begin this lesson by creating the new “Assembly”.
1. Click New , Click Part., Click OK.
Next: Set up measurement units to be in “inches” – 3 Decimals (ANSI)
1. Click on “Options” icon.
2. Click on “Document Properties” tab.
3. Now click “Units”.
4. Under “Unit system” click on “IPS”. Hit
NEXT:
1. Click on the “Features toolbar” tab. Then click on
Extruded Boss/Base icon.
2. Move the pointer over the TOP plane to highlight it, then select it.
The display changes, so that the TOP plane is facing you.
Your sketch opens on the: TOP plane.
Savethe part as: Machine Vise #1.sldasm
Top-Down Assembly
-This lesson will guide us through some techniques of creating new parts in the context of assembly, or Top Down mode.
-By using the existing geometry of other parts such as their locations, features and sizes, to construct new components, is referred to as In-Context-Assembly. This option greatly helps capturing your design intents and reduces the time it takes to do a design change. The parts update within themselves based on the way they were created.
-While working in the top down assembly mode, every time a face or a plane is selected as a sketch plane to create a feature of the new part, the system automatically creates an INPLACE mate to reference the new part.
-The Inplace mates can be suppressed so that components can be moved or repositioned and the Inplace mates can also be deleted so that new mates can be added to establish new relationships with other components.
-When a part is being edited, the Edit Component icon is selected and the part’s color changes to blue or magenta, depends on the color settings in the system options.
-Upon successful completion of this lesson, you will have a better understanding of the 2 assembly methods in SolidWorks: the traditional Bottom Up assembly (where parts are created separately, then inserted into an assembly document and get mated together), and the dynamic Top Down assembly (where the parts can be created together, in the context of an assembly).
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Tools Needed:
Insert Sketch Sketch Mirror Dimension
Fillet/Round Offset Entities Edit Part Component
Base/Boss Extrude Planes Rectangle
Circle Convert Entities Center point Arc
Add Geometric Relations Loft
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1. Starting with a new assembly:
-Select File / New / Assembly.
-Click Cancel to exit the Begin Assembly mode.
NEXT:
Go to “Save As”
Set up a New Folder and give it the title “Machinist Vise”
In this folder, save the new assembly document as: Machinist Vise #1.sldasm
2. Creating the Base part:
-Select Insert / Component / New Part.
1.
2. 3.
-Select the FRONT plane from the FeatureManager tree to reference the new part (Inplace 1).
-The system creates a new part using its default name [Part1^Assembly]<1>.
-To rename the part, right click on its default name select Rename Part.
-Enter: Base as the new name for the 1st part.
-The new part has the default Blue color.
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-A new sketch has been created automatically from the previous step.
-Sketch the profile as shown below, keep the Origin on the lower right hand side.
-Add the Dimensions
or Relations needed to
fully define the sketch.
3. Extruding the Base:
- Click or select Insert / Boss-Base / Extrude. Origin
- Direction 1: Mid-plane
- Extrude Depth: .750 in.
- Click OK.
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4. Adding the Side Mounting Flanges:
- Select the bottom face of the base and open a new sketch.
- Sketch the profile below; use the Mirroroption to keep the sketch entities symmetrical with the Centerline.
- Add dimensions as shown.
5. Extruding the Side Mounting Flanges:
- Click or select Insert / Boss-Base / Extrude.
- Direction 1: Blind (Reverse)
- Extrude Depth: .200 in.
- Click OK.
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6. Adding the side cuts:
- Select the face as indicated, and click or select Insert/Sketch.
- Sketch a Centerlinestarting at the origin and click Dynamic Mirror
7. Extruding the side cuts:
Select this face
- Click or select Insert / Cut / Extrude.
- Direction 1: Up-To-Surface
- Select the face as indicated.
-Click OK.
Save as Machinist Vise #1
In the dialog box, type Machinist Vise #1, add Your initials and today’s date, for the File name. Example: Machinist Vise #1, WEK 12-25-15
Add your information and Print your: Machinist Vise #1
Update the following information: Drawn By: (Your Name)
Title: Machinist Vise #1
“BASE FEATURE”
Date:(Today’s date)
Period:(Your class period)
Score: ____/100
Machinist Vise #2
“FIXED JAW LOFT”
Save as Machinist Vise #2
In the dialog box, type Machinist Vise #2, add Your initials and today’s date, for the File name. Example: Machinist Vise #2, WEK 2-5-15
8. Creating a new work plane:
- Select the face* as shown and click the down arrow on and select or go to Insert / Reference Geometry / Plane.
- Click Offset Distance
- Enter .150 in. (The new plane is set away from the face.)
- Click OK.
Select this face*
9. Creating the Fixed Jaw, sketch 1 of 4:
- Select the new plane and click or select Insert / Sketch.
- This will best be drawn in the Left Side View.
- Insert a rectangle approx. 2 inches above the origin.
- Add dimensions to fully position the sketch as shown.
- Exit the sketch or select Insert / Sketch.
10. Creating the 2nd profile, sketch 2 of 4:
- Select the face** as indicated and click or select Insert / Sketch.
Select this face**
- Hold down the CONTRL (Ctrl) key and select the 4 edges as shown
- On the Sketch-Tools toolbar click on Convert Entities
- The 4 selected edges are converted into a new 2D rectangle.
- Exit the sketch or select Insert / Sketch.
11. Creating the 1st Guide Curve, sketch 3 of 4:
- Select the FRONT plane, and click or
select Insert / Sketch.
- Sketch a Centerpoint-Arc . - Add the Relations as shown below.
Pierce
Tangent
Pierce
- Exit the sketch or select Insert / Sketch.
12. Creating the 2nd Guide Curve, sketch 4 of 4:
- Select the FRONT plane and clickor select Insert / Sketch.
- Sketch another Centerpoint-Arc.
approximately as shown.
*Pierce Tangent
Pierce
- Add the Relations needed to fully define the sketch.*
- Exit the Sketch or select Insert / Sketch.
13. Creating the Fixed Jaw loft:
- Click or select Insert / Boss-Base / Loft.
- Select the 2 sketch profiles as labeled (Profile 1 and Profile 2) .
- Expand the Guide Curve section and select the Guide Curve #1
and Guide Curve # 2 .
- Expand the Start/End Constraints section.
- Select Normal To Profile for both options.
- Click OK .
- The resulted loft with two guide curves.
Save Machinist Vise #2.
Print in Isometric
Add your information and Print your: Machinist Vise #2.sldasm
Update the following information: Drawn By: (Your Name)
Title: Machinist Vise #2
“Fixed Jaw loft”
Date:(Today’s date)
Period:(Your class period)
Score: ____/100
Machinist Vise #3
“FIXED JAW CLAMP”
Save as Machinist Vise #3
In the dialog box, type Machinist Vise #3, add Your initials and today’s date, for the File name. Example: Machinist Vise #3, WEK 2-5-15
14. Creating the Fixed Jaw Clamp:
- Select the FRONT plane from the FeatureManager tree and click or select Insert / Sketch.
- Sketch a Rectangleand add Dimensions and Relations as indicated.
15. Extruding the Fixed Jaw Clamp:
- Click or select Insert / Boss-Base / Extrude.
- Direction 1: Mid-Plane
- Extrude Depth: 1.250 in.
-Click OK .
Add your information and Print your: Machinist Vise #3.sldasm
Update the following information: Drawn By: (Your Name)
Title: Machinist Vise #3
“Fixed Jaw Clamp”
Date:(Today’s date)
Period:(Your class period)
Score: ____/50
Machinist Vise #4
“LEAD SCREW HOLE”
Save as Machinist Vise #4
In the dialog box, type Machinist Vise #4, add Your initials and today’s date, for the File name. Example: Machinist Vise #4, WEK 2-5-15
16. Creating the Lead Screw Hole:
- Select the face as indicated and open a new sketch
- Sketch a Circle and add the dimensions and relations as shown.
17. Extruding the Lead Screw Hole:
- Click or select Insert/Cut/Extrude
- Direction 1: Through All
- Click OK
Save As MV #4
18. Adding Fillets
- Click Fillet or select Insert/Features/Fillets-Rounds.
- Enter .032 for Radius.
Select the edges shown below for Edges to Fillet
- Click OK
- The Base part is shown in Front and Back Isometric views
19. Saving your work: MV #4 and print
- Select File/Save As/ Save
- Click to exit the Edit Component mode.
Add your information and Print your: Machinist Vise #4.sldasm
Update the following information: Drawn By: (Your Name)
Title: Machinist Vise #4
“Lead Screw Hole”
Date:(Today’s date)
Period:(Your class period)
Score: ____/50
Machinist Vise #5
“THE MOVABLE JAW BASE”
Save as Machinist Vise #5
In the dialog box, type Machinist Vise #5, add Your initials and today’s date, for the File name. Example: Machinist Vise #5, WEK 2-5-15
20. Creating a new component: the Movable Jaw Base
- Select Insert/Component/New Part.
- Select the face indicated as sketch plane for the new component (Inplace2).
- A new part and a new sketch are created in the Feature Manager tree.
- Rename the component to Movable Jaw.
- A new part is created in the FeatureManager tree and the sketch pencil is activated.
An INPLACE mate _ is also created for the new component to reference its location.
21. Using the Offset Entities command:
- Select the 4 edges of the model (as shown) and click Offset Entities.
- Enter .010 in. for offset value.
- Sketch the rest of the profile and add the dimensions or relations needed to fully define the sketch.
Note:
The mirror option can be
Used to help speed up the
process and keep the profile
symmetrical at the same time.
22. Extruding the Movable Jaw Base:
- Click on the features toolbar or select Insert/Base/Extrude
- Direction 1: Blind and reverse direction
- Extrude Depth: 1.000 in
- Click OK
- The Slide Jaw is viewed from the front and the back isometric views.
Save: M.V. #5 and print
Add your information and Print your: Machinist Vise #5.sldasm
Update the following information: Drawn By: (Your Name)
Title: Machinist Vise #5
“THE MOVABLE JAW BASE”
Date:(Today’s date)
Period:(Your class period)
Score: ____/50
Machinist Vise #6
“ADDING THE SUPPORT WALL TO THE BASE”
Save as Machinist Vise #6
In the dialog box, type Machinist Vise #6, add Your initials and today’s date, for the File name. Example: Machinist Vise #6, WEK 2-5-15
23. Adding the support wall:
- Select the indicated face and open a new sketch or select Insert/Sketch.
- Sketch the profile and add dimensionsas shown below to fully define the sketch.
24. Extruding the Support Wall:
- Clickon the Features toolbar or select Insert / Base / Extrude.
- Direction 1: Blind and reverse direction _.
- Extrude Depth: .375 in.
- Click OK.
- The Support wall is built with a guide hole.
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25. Creating a new work plane:
- Select the face as indicated and clickor select Insert / Reference Geometry / Plane.
- Enter .150 in. in the Offset Distance box and place the new plane on the outside.
Add your information and Print your: Machinist Vise #6.sldasm
Update the following information: Drawn By: (Your Name)
Title: Machinist Vise #6
“SUPPORT WALL”
Date:(Today’s date)
Period:(Your class period)
Score: ____/50
Machinist Vise #7
“MOVABLE JAW LOFT”
Save as Machinist Vise #7
In the dialog box, type Machinist Vise #7, add Your initials and today’s date, for the File name. Example: Machinist Vise #7, WEK 2-5-15
26. Creating the Slide Jaw, 1st sketch:
- Open a new sketchor select Insert / Sketch
- Sketch a rectangleand add the dimensionsshown to fully define the sketch.
- Exit the sketchor select Insert / Sketch.
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27. Creating the Slide Jaw, 2nd Sketch:
-Select the indicated face and open a new sketch or select Insert / Sketch.
- Sketch a rectangleas shown.
- Add dimensionsto fully define the sketch.
- Exit the Sketchor select Insert / Sketch.
28. Creating the Guide Curve to connect the two sketches:
-Select the RIGHT plane of the part, from the FeatureManager tree.
- Clickto open a new sketch, or select Insert / Sketch.
Guide Curves
- Guide curves are used to control the profile from twisting as the sketch is swept along the path.\
- Guide curves are also used in Sweep to shape the 3D features.
- Each profile is PIERCED or coincident with the guide curve.
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- Sketch either a Centerpoint Arc or a 3-Point Arc _ that connects two sketches.