We’ve all seen them, beautiful vases with amazing organic shapes. Maybe you’re wondering if these kinds of shapes can be modeled in SOLIDWORKS.
This is exactly what we are going to do today. Today we are going to model this beautiful vase in SOLIDWORKS.
This tutorial covers several SOLIDWORKS features such as surface revolve, surface loft, surface extrude, surface mirror, surface knit, surface fill, dome, and many others.
Make sure to give this tutorial a try if you want to learn more about surface modeling in SOLIDWORKS.
Happy modeling! 🙂
Jan
Click here to download this tutorial as a free eBook (PDF).
Click here to download this tutorial as a free eBook (PDF).
Open a New Part with model units set to millimeters
Go to: File > New > Part
Save the File with the following name: Ceramic Vase.SLDPRT 
Create a 2D Sketch on the Front Plane (Sketch1)
Select the Front Plane from the Feature tree and click on the sketch icon 
Click on the Normal To 
icon
Go to: Tools > Sketch Entities > Centerline 
Draw a vertical centerline upwards from the origin
Then draw a horizontal centerline as shown in the image below:
Go to: Tools > Dimensions > Smart 
Assign dimensions to the centerlines, as shown in the image below:
Go to: Tools > Sketch Entities > Spline 
Draw a 2-point spline by using the yellow encircled points of the sketch, as shown in the image below:
Now click on the lower spline handle
And assign a horizontal relation from the property manager as shown in the image below:
Go to: Tools > Dimensions > Smart
Hold the Ctrl key; select the upper spline handle and the vertical centerline
Assign an angular dimension of 45 degrees
Click on the upper spline handle and assign a handle length of 205mm
Click on the lower spline handle and assign a handle length of 140mm, as shown in the image below:
Create a Surface Revolve:
Go to: Insert > Surface > Revolve 
Select the vertical centerline of the sketch as an Axis of revolution
After selecting the axis a 360-degree surface is generated in yellow
Go to the property manager and change the revolution angle into 
90 degrees
Click on the Reverse Direction 
icon, as shown in the image below:
Click OK 
to complete the operation.
Create a 2D Sketch on the Right Plane (Sketch2)
Select the Right Plane from the Feature tree and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Sketch Entities > Centerline
Draw a vertical upward centerline from the origin
Go to: Tools > Dimensions > Smart
Assign a length of 130mm to the centerline, as shown in the image below:
Go to: Tools > Sketch Entities > Line 
Draw a downward inclined line from the upper-end point of the centerline, as shown in the image below:
Hold the Ctrl Key; Select the origin and the lower endpoint of the inclined line
Assign a Horizontal 
relation from the property manager, as shown in the image below:
Go to: Tools > Dimensions > Smart
Assign an angle of 4 degrees between the lines, as shown in the image below:
Use the Split Line Tool
Go to: Insert > Curves > Split Line 
Go to the property manager and choose the Type of Split – Projection
Go down to the Selections menu
The Current Sketch (Sketch2) is automatically selected in the Sketch Selection 
input box
Click on the Faces To Split 
input box
Move to the modeling area and select the revolved face, as shown in the image below:
Click OK to complete the operation.
Create a 2D Sketch on the Front Plane (Sketch3)
Select the Front Plane from the Feature tree and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Sketch Tools > Offset Entities 
Select the upper surface to make an offset
Go to the property manager and assign an offset value of 1mm, as shown in the image below:
Click OK to complete the operation.
Click and drag the left endpoint of the offset entity to extend it, as shown in the image below:
Go to: Tools > Dimensions > Smart
Click on the extended line and assign a 30mm length
Go to: Tools > Sketch Entities > Spline
Draw a 2-point vertical spline by using the yellow encircled points, as shown in the image below:
Click on the spline and drag both handles one by one to activate it
Now click on the lower spline handle
Assign a Horizontal relation from the property manager as shown in the image below:
Go to: Tools > Dimensions > Smart
Hold the Ctrl key, select the upper spline handle and the vertical centerline
Assign the spline dimensions, as shown in the image below:
Use the Split Line Tool
Go to: Insert > Curves > Split Line
Go to the property manager and choose the Type of Split – Projection
Go down to the Selections menu
The Current Sketch (Sketch2) is automatically selected in the Sketch Selection input box
Click on the Faces To Split input box
Move to the modeling area and select Face<1>, as shown in the image below:
Click OK to complete the operation.
Make Reference Points:
Go to: Insert > Reference Geometry > Point 
Select the last icon 
from the property manager
Go to the modeling area and select the highlighted surface edge – Edge<1>
Go to the property manager, select the Evenly Distributed option
Assign the number of points 
to 5, as shown in the image below:
Click OK to complete the operation.
Make a Surface Offset:
Go to: Insert > Surface > Offset 
Click on the blue highlighted surface, as shown in the image below:
Go to the property manager and assign an offset value of 0mm, as shown in the above image
Click OK to complete the operation.
Go to the feature tree, click on the Surface-Offset1 and click on the Eye 
icon to hide it.
Use the Delete Face Tool
Go to: Insert > Face > Delete 
Go to the modeling area and select the two blue highlighted faces, as shown in the image below:
Go to the Property Manager > Options
Select the Delete option
Click OK to delete the selected faces.
Go to the feature tree, click on the Surface-Offset1 and click on the Eye icon to unhide it.
Create a 2D Sketch on the Front Plane (Sketch4)
Select the Front Plane from the Feature tree and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Sketch Entities > 3 Point Arc 
Draw a 3 point arc between the highlighted Edge Point and Point 1, as shown in the image below:
Similarly draw five more arcs adjacent to each other by using these reference points, as shown in the image below:
Select all the 6 arcs and assign the equal relation from the property manager
Go to: Tools > Dimensions > Smart
Click on the first arc and assign the radius 12mm, as shown in the image below:
Make a Surface Extrude:
Go to: Insert > Surface > Extrude 
Sketch4 will be selected automatically if we use the surface extrude without closing the sketch area
Go to the Property Manager, select the Blind option and assign the extrude value 
of 10mm
Then click on the Flip Direction 
icon to reverse the surface extrusion, as shown in the image below:
Click OK to complete the operation.
Make a Fillet
Go to: Insert > Features > Fillet/Round 
Go to the Property Manager > Fillet Parameter
Assign a fillet radius 
of 2mm
Go to the modeling area, select all the edges of the extruded surface
Go to the Property Manager > Fillet Parameters > Profile
Choose the Curvature Continuous option for a smoother result, as shown in the image below:
Click OK to complete the operation.
Make a Surface Loft
Go to: Insert > Surface > Loft 
Go to the property manage and right-click on the profile selection input box
Then click on the Selection Manager from the pop-up options
A selection manager window will appear in the modeling area
Click on the third icon from the selection manager for a Group Selection 
Select the upper edge of the extruded surface
Then a tangency selection icon 
will appear in the modeling area
Click on that icon to select all the tangent edges
Click OK in the selection manager to confirm the selection, as shown in the image below:
Now select Edge <1> to create a surface loft, as shown in the image below:
Go to the Property Manager > Guide Curves
Click on the guide curve 
input box
Go to the modeling area, select Edge<2> as the 1st guide curve
Then select the Edge<3> as the 2nd guide curve, as shown in the image below:
Go to the Property manager > Start/ End Constraints
First, click on the Start Constraint box and select the Tangency To Face option
Set the tangency influence value to 2
Then click on the End Constraint box and select the Tangency To Face option as well
Set the tangency influence value to 3, as shown in the image below:
Click OK to complete the operation.
Go to the modeling area click on the extruded surface,
Click on the Eye icon from the popup to hide that surface
Use the Knit Surface
Go to: Insert > Surface > Knit 
Select all the 4 existing surfaces from the modeling area
Go to the property manager, tick the Merge Entities and the Gap Control checkboxes, as shown in the image below:
Click OK to complete the operation.
Make a Fillet
Go to: Insert > Features > Fillet/Round
Go to the Property Manager > Fillet Parameter
Assign a fillet radius of 3mm
Go to the modeling area, select the highlighted edges of the knitted surface
Go back to the Property Manager > Profile
Choose the Curvature Continuous option for smooth results
Tick the Multi Radius checkbox
Go to the modeling area and assign a separate fillet dimension as shown in the image below:
Click OK to complete the operation.
Create a 2D Sketch on the Top Plane (Sketch5)
Select the Front Plane from the Feature tree and click on the sketch icon
Click twice on the Normal To icon to switch to the Bottom Plane
Go to: Tools > Sketch Entities > Ellipse 
Draw an ellipse from the origin
Hold the Ctrl key, select the yellow encircled points
Assign a Horizontal relation from the property manager, as shown in the image below:
Go to: Tools > Dimensions > Smart
Assign dimensions to the ellipse, as shown in the image below:
Create a Surface Extrude
Go to: Insert > Surface > Extrude
Go to the Property manager > From
Select the Offset option and assign an offset value of 2 mm
Go to the Property manager > Direction1
Select Blind and click on the Flip Direction icon to reverse the extrusion
Assign an extrude length of 10mm, as shown in the image below:
Click OK to complete the operation.
Create a 2D Sketch on the Top Plane (Sketch 6)
Select the Top Plane from the Feature tree and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Sketch Entities > Corner Rectangle 
Draw a corner rectangle starting from the origin point in the XZ quadrant
Go to: Tools > Dimensions > Smart
Assign a length and width of the rectangle, as shown in the image below:
Use the Surface Trim
Go to: Insert > Surface > Trim 
In the property manager, the current sketch (Sketch6) is pre-selected as a Trim tool 
Make sure the selected Trim Type is Standard
Go to the modeling area, select the purple highlighted part of the surfaces
Go back to the property manager and select the Remove Selections, as shown in the image below:
Leave the other parameters as default
Click OK to complete the operation.
Create a 2D Sketch on the Top Plane (Sketch 7)
Select the Top Plane from the Feature tree and click on the sketch icon
Click twice on the Normal To icon to switch to the Bottom Plane
Go to: Tools > Sketch Entities > Line
Draw two vertical lines downward, starting at the yellow encircled points
Hold Ctrl Key, Select both the endpoints of the line and the origin point
Assign a Horizontal relation from the property manager, as shown in the image below:
Use the Split Line Tool
Go to: Insert > Curves > Split Line
Go to the property manager and choose the Type of Split – Projection
Go down to the Selections menu
The Current Sketch (Sketch7) is automatically selected in the Sketch Selection input box
Click on the Faces To Split input box
Move to the modeling area and select the blue highlighted Face<1>, as shown in the image below:
Click OK to complete the operation.
Make a Surface Loft
Go to: Insert > Surface > Loft 
Go to the modeling area and select the first surface Edge <1> (Starting Edge)
Now select the second surface Edge <2> (Ending Edge), as shown in the image below:
Go to the Property Manager > Start/ End Constraints
Click on the Start Constraint box and select the Tangency To Face option
Assign a tangency influence value of 1
Click on the End Constraint box and select the Tangency To Face option as well
Assign a tangency influence value of 1.5 as shown in the image below:
Click OK to complete the surface loft operation.
Create a 2D Sketch on the Front Plane (Sketch8)
Select the Front Plane from the Feature tree and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Sketch Entities > Style Spline 
Draw a 3-point style spline by using the red encircled points of the sketch, as shown in the image below:
Note: Spline endpoints must be coincident with the surface edges
Assign a vertical and tangent relation to the style spline with the corresponding surface edges, as shown in the image below:
Make a Surface Extrude:
Go to: Insert > Surface > Extrude
Sketch8 will be automatically selected if we use the surface extrude without closing the sketch area
Go to the Property Manager, select the Blind option and assign an extrude value of 5mm
Then click on the Flip Direction icon to reverse the surface extrusion, as shown in the image below:
Click OK to complete the operation.
Use the Fill Surface Tool
Go to: Insert > Surface > Fill 
Go to the Property Manager > Patch Boundary
Click on the Patch Boundary 
input box
Go to the modeling area and select the Edge<1>, Edge<2>, Edge<3>, Edge<4>, and Edge<5> as shown in the image below:
Go to the Property Manager > Edge Settings
Select the Tangent option
Tick the Apply to All Edges checkbox and Optimize Surface checkbox
Go down in the Options and tick the Fix Up Boundary checkbox as shown in the above image
Leave the other parameters as default
Click OK to complete the surface fill operation.
Create a 2D Sketch on the Front Plane (Sketch9)
Select the Right Plane from the Feature tree and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Sketch Entities > Style Spline
Draw a 3-point style spline by using the red encircled points of the sketch, as shown in the image below:
Note: Spline endpoints must be coincident with the surface edges
Assign a Vertical 
and Tangent 
relation to the style spline with the corresponding surface edges, as shown in the image below:
Make a Surface Extrude:
Go to: Insert > Surface > Extrude
Sketch8 will be automatically selected if we use the surface extrude without closing the sketch area
Go to the Property Manager, select the Blind option and assign an extrude value of 5mm
Then click on the Flip Direction icon to reverse the surface extrusion, as shown in the image below:
Click OK to complete the operation.
Use the Fill Surface Tool
Go to: Insert > Surface > Fill
Go to the Property Manager > Patch Boundary
Click on the Patch Boundary input box
Go to the modeling area and select the Edge<1>, Edge<2>, Edge<3>, and Edge<4> as shown in the image below:
Go to the Property Manager > Edge Settings
Select the Tangent option
Tick the Apply to All Edges checkbox and Optimize Surface checkbox
Go down in the Options and tick the Fix Up Boundary checkbox as shown in the above image
Leave the other parameters as default
Click OK to complete the surface fill operation.
Use the Knit Surface
Go to: Insert > Surface > Knit
Select each of the 4 existing surfaces from the modeling area
Go to the property manager, tick the Merge Entities and the Gap Control checkboxes, as shown in the image below:
Click OK to complete the operation.
Use the Mirror Feature
Go to: Insert > Pattern/Mirror > Mirror 
Go to the property manager and click on the Mirror Face/Plane 
input box
Open the feature tree and select the Right plane as a mirror plane
Go to the property manager and click on Bodies to Mirror 
input box
Move to the modeling area and select the knitted surface body, as shown in the image below:
Make sure to select the knit surfaces checkbox
Click OK to complete the operation.
Repeat the Mirror Feature
Go to: Insert > Pattern/Mirror > Mirror
Go to the property manager and click on the Mirror Face/Plane input box
Open the feature tree and select the Right plane as a mirror plane
Go to the property manager and click on Bodies to Mirror input box
Move to the modeling area and select the mirrored surface body, as shown in the image below:
Make sure to select the knit surfaces checkbox
Click OK to complete the operation.
Create a Planar Surface
Go to: Insert > Surface > Planar 
Right-Click on any surface edge of the elliptical opening
Click on the Select Tangency option from the pop-up
After selecting all the tangent edges, a planar surface will be created, as shown in the image below:
Click OK to complete the operation.
Create a Planar Surface
Go to: Insert > Surface > Planar
Click on the circular opening of the surface, as shown in the image below:
Click OK to complete the operation.
Use the Knit Surface
Go to: Insert > Surface > Knit
Select each of the three surface bodies from the modeling area
Go to the property manager, select the Create Solid, Merge Entities, and all the Gap Control checkboxes, as shown in the image below:
Click OK to complete the operation.
Go to the Feature Tree > Surface-Revolve1 > Sketch1
Click on the Sketch1 and click on the Eye Icon to unhide it
Create a Surface Revolve:
Go to: Insert > Surface > Revolve
Select the vertical centerline of the sketch as an Axis of revolution 
After selecting the axis a 360-degree surface is generated in yellow, as shown in the image below:
Click OK to complete the operation.
Go to the Feature Tree > Surface-Revolve1 > Sketch1
Click on Sketch1 and click on the Eye icon to hide it
Go to the Feature Tree > Solid Bodies folder
Click on that folder and hit the Eye icon to hide all the solid bodies from the modeling area
Use Move/ Copy Body Tool:
Go to: Insert > Features > Move/ Copy 
Select the revolved surface
Go to the Property Manager > Translate
Assign a value 
of 4mm in the Y direction, as shown in the image below:
Click OK to complete the operation.
Use the Move Face Tool:
Go to: Insert > Face > Move 
Go to the property manager and select the Offset option
Go to the modeling area and click on the revolved surface
Go back to the Property Manager > Parameters
Assign an offset distance of 5mm and select the Flip Direction checkbox, as shown in the image below:
Click OK to complete the operation.
Go to the Feature Tree > Solid Bodies folder
Click on that folder and hit the Eye icon to show all the solid bodies
Use Cut with Surface:
Go to: Insert > Cut > With Surface 
Go to the modeling area and select the revolved surface
An arrow will appear near the selected face
This arrow indicates the Direction of the Cut, as shown in the image below:
Click OK to complete the operation.
Make a Fillet
Go to: Insert > Features > Fillet/Round 
Go to the Property Manager > Fillet Type
Click on the 4th icon to activate the Full Round Fillet 
option
Go to the Property Manager > Items To Fillet
Click on the 1st input box
Go to the modeling area, select the blue Face <1>
Go back to the Property manager > Items To Fillet
Click on the 2nd input box
Go back to the modeling area, select the violet Face <2>
Go back to the Property manager > Items To Fillet
Click on the 3rd input box
Go back to the modeling area, select the pink Face <3>
After selecting the last face a full round fillet is generated in yellow, as shown in the image below:
Click OK to complete the operation.
Go to the Feature Tree > Surface-Extrude2> Sketch5
Click on Sketch5 and hit the Eye icon to unhide the sketch
Create a 2D Sketch on the Elliptical Face (Sketch10)
Select the bottom elliptical face and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Sketch Tools > Offset Entities
Select the ellipse from the Sketch 5
Go to the property manager and assign an offset value of 3mm
Click on the Reverse checkbox to flip the offset direction, as shown in the image below:
Use the Split Line Tool
Go to: Insert > Curves > Split Line
Go to the property manager and choose the Type of Split – Projection
Go down to the Selections menu
The Current Sketch (Sketch10) is automatically selected in the Sketch Selection input box
Click on the Faces To Split input box
Move to the modeling area and select the elliptical Face<1>, as shown in the image below:
Click OK to complete the operation.
Use the Dome Tool
Go to: Insert > Features > Dome 
Select the central elliptical face (Face<1>) at the bottom of the vase
Go to the property manager and assign a dome height of 5mm
Click on the Flip Direction icon to reverse the direction of the dome (make it hollow)
Uncheck the Continuous Dome checkbox, as shown in the image below:
Click OK to complete the dome operation.
Make a Fillet
Go to: Insert > Features > Fillet/Round
Go to the Property Manager > Fillet Parameter
Assign a fillet radius of 1.5mm
Go to the modeling area, select the bottom face (the elliptical strip)
Go to the Property Manager > Fillet Parameters > Profile
Choose the Curvature Continuous option for a smoother result, as shown in the image below:
Click OK to complete the fillet operation.
Change the Appearance
Click on the Appearance 
icon (located on the right side of the windowpane)
Select Appearances (color) > Plastic > Satin Finish
Select the White Satin Finish Plastic 
as shown in the image below:
Click OK to apply the new appearance
Go to: View > Display
Select the Shaded 
and Shadows In Shaded Mode 
The completed geometry will look like as shown in the image below:
Save the File again
Congratulations, you’ve just completed your own Vase in SOLIDWORKS! 🙂
Click here to download this tutorial as a free eBook (PDF).
Did you like this free tutorial and do you want to learn more?
Click here to download Jan’s free SOLIDWORKS workbook.
In this free PDF eBook, we will start modeling an incredible Aston Martin One-77 in SOLIDWORKS.
Happy modeling! 🙂
Jan
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