How to model a Deodorant Roller in SOLIDWORKS?

When I studied Product Design & Engineering I received an amazing SOLIDWORKS tutorial from my SOLIDWORKS teacher Daan Haeyen. In this tutorial Daan showed me how to model a deodorant roller in SOLIDWORKS. Because I learned a lot about surface modeling with this tutorial I thought it would be great to reproduce and share it today with you.

In this tutorial I’ll show you the following features:

• Draw a 2d sketch
• Insert a blueprint
• Surface Revolve
• Surface Sweep
• Surface Loft
• Surface Fill
• Surface Knit
• Fillet
• New Axis
• Revolved Cut

Hapy modeling!

Jan

P.S. I encourage you to share this tutorial with your network.

Open a new part with model units set to millimeters

Go to: File > New > Part

Create a 2D sketch

Select the Right Plane in the feature tree (menu at the left side) and create a sketch by clicking on the 2D Sketch icon 

The display changes so the Right plane faces you.

Insert a reference picture

For this tutorial, we use a blueprint of the Deo roller to approach the organic shape as good as possible.

Click here to download a reference picture and save it into your SOLIDWORKS folder

Go to: Tools > Sketch Tools > Sketch Picture 

Go to your SOLIDWORKS folder and select the picture “SIDEVIEW_DEOROLLER.Jpg”

Click: Open

Change the dimensions and position of the picture with the menu as shown in the picture.

Select ‘’Full image’’ in the Transparency tab and change the transparency into 0.40

Click OK 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Insert a second reference picture

Select the Front Plane in the feature tree (menu at the left side) and create a sketch by clicking on the 2D Sketch icon 

Download the picture here and save it into your SOLIDWORKS folder

Go to: Tools > Sketch Tools > Sketch Picture 

Go to your SOLIDWORKS folder and select the picture “FRONTVIEW_DEOROLLER.Jpg”

Click: Open

Change the dimensions and position of the picture with the menu as shown in the picture.

Select ‘’Full image’’ in the Transparency tab and change the transparency into 0.40

Click OK 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the two centerlines as shown in the picture 

Change the dimensions by clicking at the dimension button 

Fix the two lines with the Fix icon 

Draw the two lines as shown in the picture 

Change the dimensions by clicking at the dimension button 

Draw a spline without any midpoints 

Select one of the straight lines, hold down the control key and select the spline

Click at the Tangent icon as shown in the picture 

Repeat this action for the other side of the spline

Change the length of the arrows to approach the curve of the blueprint

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create a Surface Revolve

Go to Insert > Surface > Revolve or click at the Revolve icon 

Click at the blue Centerline to define the Axis of Revolution 

Use the One-Direction option 

Set the Revolution Angle to 360 degrees 

Click OK 

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the line as shown in the picture 

Change the dimensions by clicking at the dimension button 

Make sure that the angle of the line is equal to the front curve of the deoroller

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch4

Double click at Sketch4 in the feature tree and rename it to GUIDELINE_FRONT

Create another 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the line as shown in the picture 

Change the dimensions by clicking at the dimension button 

Make sure that the angle of the line is equal to the back curve of the deoroller

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch5

Double click at Sketch5 in the feature tree and rename it to GUIDELINE_BACK

Create a 2D sketch

Select the Front Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw a spline without midpoints as shown in the picture 

Change the length of the lower arrow to approach the curve of the blueprint

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch6

Double click at Sketch6 in the feature tree and rename it to GUIDELINE_SIDE

Create a 2D sketch

Select the Top Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the centerline as shown in the picture 

Connect the centerline with the endpoints of GUIDELINE_FRONT and GUIDELINE_BACK

Draw a spline with four points as shown in the picture 

Connect three points with GUIDLINE_FRONT, GUIDELINE_BACK and GUIDELINE_SIDE

Draw the fourth point somewhere in the space as shown in the picture

Make the Spline symmetric

Select the right point, hold down the Control key, select the centerline and select the left point.

Click at the Symmetric option in the menu 

Click OK 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch7

Double click at Sketch7 in the feature tree and rename it to PROFILE

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw a line, starting at Origin 

Change the length of the line to 58 mm 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch8

Double click at Sketch8 in the feature tree and rename it to PATH

Create a Surface Sweep 

Go to Insert > Surface > Sweep or click at the Sweep icon 

Select the PROFILE sketch in the Feature Tree as Sweep Profile

Select the PATH sketch in the Feature Tree as Sweep Path

Select GUIDLINE_FRONT, GUIDELINE_BACK and GUIDELINE_SIDE in the Feature Tree as Sweep Guides

Click OK 

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the line as shown in the picture 

Change the dimensions by clicking at the dimension button 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Trim the upper side of the Surface Sweep

Go to: Insert > Surface > Trim or click at the Trim icon 

Click in the Trim tool box 

Select the line of the new Sketch9 as shown in the picture.

Select the “Remove selections” option.

Select the purple surface above the line as shown in the picture. 

Surface Split Options: Natural

Click OK 

Create a Surface Loft 

Go to Insert > Surface > Loft or click at the Surface icon 

Click in the Profiles box 

Select the two edges as shown in the picture

Make sure that the green balls are both on the same end as shown in the picture

If not, click and drag them to the other side of the sketch

Make the Loft Curvature

Click at the Start/End Contraints box

Set the Start constraint to Curvature To Face as shown in the picture

Set the End constraint to Curvature To Face as shown in the picture

You can optimize the shape of the Loft by changing the Length of the Curvature arrows

Click OK 

Fill the bottom of the Deoroller

Go to: Insert > Surface > Fill or click at the Fill icon 

Click OK 

Knit the surfaces and create a solid body

Go to Insert > Surface > Knit or click at the Surface Knit icon 

Click in the Selections box and select the 4 blue surfaces 

Select the ‘’Try to form solid’’ option

Select the “Merge entities” option

Deselect the ‘’Gap Control’’ option

Click OK 

Create a fillet on the edge of the bottom

Go to: Insert > Features > Fillet/Round or click at the Fillet icon 

Select the edge as shown in the picture.

Change the Radius into 2 mm 

Click OK 

Create a new Axis

Go to: Insert > Reference Geometry

Select the Cylindrical/Conical Face option

Select the blue surface as shown in the picture

Click OK 

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the rectangle using the 3 Point Corner Rectangle option as shown in the picture and detail 

Change the dimensions by clicking at the dimension button 

Create a Revolved Cut

Go to: Insert > Cut > Revolve or click at the Cut Revolve icon 

Axis of revolution : Select Axis1.

Click OK 

Save  the file with the following name: Deoroller.SLDPRT

Congratulations, you just finished the Deodorant Roller!

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I hope you liked this LearnSOLIDWORKS tutorial!

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Thanks a million!

Jan