Part #2 | How to model an organic Rim in SOLIDWORKS?

Last week we started to model an organic rim in SOLIDWORKS. In part #1 of this 2 part mini-series, you discovered how to model the outer layer of the rim. In today’s tutorial, we will continue with the inner layer of the rim. You will discover many interesting features throughout this tutorial.

I hope you like it! 🙂

Jan

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

Click here to download this SOLIDWORKS tutorial as a free eBook (PDF).

Did you miss the first part of this tutorial? Click here to get started with part #1 of this series.

Create a 2D Sketch on the Front Plane

Select the Front Plane from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Entities > Corner Rectangle

Draw a corner rectangle from the origin to the upper right direction

Go to the property manager and check the For construction checkbox

Go to: Tools > Dimensions > Smart

Assign the dimensions to the length and width, as shown in the image below

Go to: Tools > Sketch Entities > Corner Rectangle

Draw another corner rectangle from the origin to the lower right direction

Go to the property manager and tick the For construction checkbox

Go to: Tools > Dimensions > Smart

Assign the dimensions to the length and width, as shown in the image below

Go to: Tools > Sketch Entities > Spline

Draw a two-point spline without the midpoints, as shown in the image below

Click on the spline and drag on both handles to activate them

Hold the Ctrl key, select the top handle and the vertical center line

Assign an angular dimension of 140 degrees

Similarly, select the bottom handle and the horizontal center line

Assign an angular dimension of 90 degrees, as shown in the image below

Click on the top handle and assign a handle length of 140mm

Click on the bottom handle and assign a handle length of 140mm, as shown in the image below

Create a Revolved Surface

Go to: Insert > Surface > Revolve… or click directly on Revolved Surface

Select the center line of the sketch which is passing through the origin, as shown in the image below

Click OK to complete the revolve operation.

Use the Thicken Tool

Go to: Insert > Boss/ Base > Thicken

Select the revolved surface as a Thicken parameter from the modeling area

Go to the property manager, select the third icon  as a thickness type

Assign a thickness value of  1.5mm, as shown in the image below

Click OK to complete the revolve operation.

Create a 2D Sketch on the Top Plane

Select the Top Plane from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Entities > Circle

Draw a circle concentric to the origin

Go to the property manager and tick the For Construction checkbox

Go to: Tools > Dimensions > Smart

Click on the circle and assign a diameter value of 265mm

Go to: Tools > Sketch Entities > Center Line

Draw a horizontal centerline starting from the origin to the circle, as shown in the image below

Draw the three center lines as shown in the image below

Go to: Tools > Dimensions > Smart

Assign dimensions to the center lines, as shown in the image below

Go to: Tools > Sketch Entities > Ellipse

Draw an ellipse starting from the middle of the 80mm center line up to its endpoints

Go to: Tools > Dimensions > Smart

Assign dimensions to the ellipse, as shown in the image below

Click on the Close sketch icon  to close the sketch area.

Make an Extrude Cut

Go to: Insert > Cut > Extrude… or click on Extrude Cut

Select Sketch6 from the feature tree

Go to the Property Manager >> Direction 1

Select the Through All option and click on the Flip Direction icon, as shown in the image below

Click OK to complete the extruded cut command.

Use the Fillet

Go to: Insert > Features > Fillet/Round

Select both edges of the elliptical cut-out, as shown in the image below

Go to the property manager and assign a fillet radius  of 0.75mm

Click OK to complete the fillet operation.

Create a Circular Pattern

Go to: Insert > Pattern/Mirror > Circular Pattern

Select the inner circular edge as a reference direction

Assign the number of instances  18 with an equal spacing of 360 degrees

Go down in the property manager, select Features and Faces

Go to the feature tree and select Cut-Extrude3 and Fillet6, as shown in the image below

Click OK to complete the operation.

Create a 2D sketch on the Top Plane

Select the Top Plane from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Entities > Circle

Draw a circle concentric to the origin

Go to the property manager and tick the For Construction checkbox

Go to: Tools > Dimensions > Smart

Click on the circle and assign a diameter value of 140mm

Go to: Tools > Sketch Entities > Center Line

Draw a horizontal radial line starting from the origin up to the circle, as shown in the image below

Draw the three center lines as shown in the image below

Go to: Tools > Dimensions > Smart

Assign dimensions to the center lines, as shown in the image below

Go to: Tools > Sketch Entities > Ellipse

Draw an ellipse starting from the middle of the 44mm center line up to its endpoints

Go to: Tools > Dimensions > Smart

Assign dimensions to the ellipse, as shown in the image below

Click on the Close sketch icon  to close the sketch area.

Make an Extrude Cut

Go to: Insert > Cut > Extrude… or click on the Extrude Cut

Select Sketch7 from the feature tree

Go to the Property Manager >> Direction 1

Select the Through All option and click on the Flip Direction icon, as shown in the image below

Click OK to complete the extrude cut operation.

Use the Fillet

Go to: Insert > Features > Fillet/Round

Select the inner face of the elliptical cut-out, as shown in the image below

Go to the property manager and assign a Fillet radius  of 0.75mm

Click OK to complete the fillet operation.

Create a Circular Pattern

Go to: Insert > Pattern/Mirror > Circular Pattern

Select the inner circular edge as a Reference direction

Assign a number of instances of  18 with equal spacing 360 degrees

Go down in the property manager, select Features  and Faces

Go to the feature tree and select Cut-Extrude4 and Fillet7, as shown in the image below

Click OK to complete the operation.

Use the Move/ Copy Body feature

Go to: Insert > Features > Move/ Copy…

Select the existing solid body from the modelling area

Go to the property manager and click on the Rotate  option

Go to the feature tree and select Origin as a rotating reference

Assign the rotation values about the X, Y and Z Axis

X= 0 degrees,  Y= 10 degrees, and  Z= 0 degrees

Click OK to complete the operation.

Create a 2D Sketch on the Top Plane

Select the Top Plane from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Entities > Center Line

Draw an upward vertical center line starting from the origin

Go to: Tools > Dimensions > Smart

Click on the center line and assign a vertical length of 27.5mm, as shown in the image below

Go to: Tools > Sketch Entities > Circle

Draw a circle at the top end of the center line

Go to: Tools > Dimensions > Smart

Click on the circle and assign a diameter value of 7mm, as shown in the image below

Click on the Close sketch icon  to close the sketch area.

Make an Extrude Cut

Go to: Insert > Cut > Extrude… or Click on the Extrude Cut

Select Sketch8 from the feature tree

Go to the Property Manager >> Direction 1

Select the Through All option and click on the Flip Direction icon, as shown in the image below

Click OK to complete the extruded cut operation.

Use the Fillet

Go to: Insert > Features > Fillet/Round

Select the inner surface of the circular cut-out, as shown in the image below

Go to the property manager and assign a Fillet radius  of 0.75mm

Click OK to complete the fillet operation.

Create a Circular Pattern

Go to: Insert > Pattern/Mirror > Circular Pattern

Select the inner circular edge as reference direction

Assign a number of instances of  18 with equal spacing 360 degrees

Go down in the property manager, select Features  and Faces

Go to the feature tree and select Cut-Extrude5 and Fillet8, as shown in the image below

Click OK to complete the operation.

Go to the Feature Tree >> Solid Bodies(2) >> CirPattern3

Click on the CirPattern3 and then click on the Show  icon, as shown in the image below

Create a 2D Sketch on the Top Plane

Select the Top Plane from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Entities > Circle

Draw a circle starting from the origin

Go to: Tools > Dimensions > Smart

Click on the circle and assign a diameter of 200mm, as shown in the image below

Make an Extrude Cut

Go to: Insert > Cut > Extrude… or click on Extrude Cut

Select the circular sketch from the modeling area

Go to the Property Manager >> Direction 1

Select the Through All-Both option and tick the Flip side to cut checkbox, as shown in the image below

Click OK  to complete the extruded cut operation.

Create a 2D Sketch on the Bottom face

Click on the circular bottom edge of the solid body and click on the sketch icon

Go to: Tools > Sketch Tools > Offset Entities

Select the inner circle of the circular strip

Go to the Property manager >> Offset Entities >> Parameters

Assign an offset distance  of 0.5mm, as shown in the image below

Click OK  to complete the operation.

Make an Extrude Boss/Base

Go to: Insert > Boss/Base > Extrude… or click on the Extrude Boss/Base

Select the offset circular sketch from the modeling area

Go to the Property Manager >> Direction 1

Select the Blind option and click on the Flip Direction icon

Assign an extrude length of 16mm, as shown in the image below

Make sure that the Merge result checkbox is ticked in the property manager

Click OK  to complete the extruded cut operation.

Use the Dome Tool

Go to: Insert > Features > Dome

Click on the upper circular face of the extruded boss

Go to the property manager and assign a dome height of 5mm, as shown in the image below

Leave other options as default

Click OK  to complete the dome operation.

Use the Fillet

Go to: Insert > Features > Fillet/Round

Select the highlighted circular edge of the solid body, as shown in the image below

Go to the property manager and assign a Fillet radius  of 2.5mm

Click OK to complete the fillet operation.

Create a 2D Sketch on the Top Plane

Select the Top Plane from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Entities > Center Line

Draw an upward vertical center line starting from the origin

Go to: Tools > Dimensions > Smart

Click on the center line and assign a vertical length of 12mm, as shown in the image below

Go to: Tools > Sketch Entities > Circle

Draw a circle at the top end of the center line

Go to: Tools > Dimensions > Smart

Click on the circle and assign a diameter value of 8mm, as shown in the image below

Click on the Close sketch icon  to close the sketch area.

Make an Extrude Cut

Go to: Insert > Cut > Extrude… or click on the Extrude Cut

Select the Sketch8 from the feature tree

Go to the Property Manager >> Direction 1

Select the Through All option and click on the Flip Direction icon, as shown in the image below

Click OK to complete the extruded cut operation.

Use the Fillet

Go to: Insert > Features > Fillet/Round

Select the inner surface of the circular cut-out, as shown in the image below

Go to the property manager and assign a Fillet radius  of 1mm

Click OK to complete the fillet operation.

Create a 2D Sketch on the Top plane

Select the Top Plane from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Tools > Offset Entities

Select the circular face of the solid body, as shown in the image below

Go to the Property manager >> Offset Entities >> Parameters

Assign the offset distance  of 2mm and tick the Reverse checkbox

Click OK to complete the operation.

Click on the Close sketch icon  to close the sketch area.

Make an Extrude Cut

Go to: Insert > Cut > Extrude…   or click on Extrude Cut

Select the offset circular sketch from the modeling area

Go to the Property Manager >> Direction 1

Select the Through All-Both option, as shown in the image below

Click OK to complete the extruded cut operation.

Create a Circular Pattern

Go to: Insert > Pattern/Mirror > Circular Pattern

Select the inner circular edge as a Reference direction

Assign a number of instances of  5 with equal spacing 360 degrees

Go down in the property manager, select Features and Faces

Go to the feature tree and select Cut-Extrude4 and Fillet7, as shown in the image below

Click OK to complete the operation.

Create a 2D Sketch on the Front Plane

Select the Front Plane from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Entities > Line

Draw a diagonal line, as shown in the image below

Go to: Tools > Sketch Entities > Center Line

Draw two vertical center lines at the ends of the diagonal line

Draw a solid line to connect both ends of the vertical line, as shown in the image below

Go to: Tools > Dimensions > Smart

Assign dimensions to all the lines, as shown in the image below

Go to: Tools > Sketch Entities > Line

Draw the following lines, as shown in the image below

Go to: Tools > Dimensions > Smart

Assign dimensions to all new lines, as shown in the image below

Go to: Tools > Sketch Tools > Offset Entities

Go to the Property manager >> Offset Entities >> Parameters

Assign an offset distance  of 2mm

Tick the Reverse checkbox, Select Chain checkbox and Cap Ends (Arc) checkbox

Go to the sketch area and click on one of the solid lines to select all lines, as shown in the image below

Click OK to complete the operation.

Go to: Tools > Sketch Entities > Center Line

Draw a vertical center line starting from the origin, as shown in the image below

Click on the Close sketch icon  to close the sketch area.

Create a Revolve

Go to: Insert > Boss/Base > Revolve… or click on Revolved Boss/Base

Select the center line of the sketch which is passing through the origin, as shown in the image below

Make sure that Merge result checkbox is ticked in the property manager

Click OK  to complete the revolve operation.

Use the Fillet

Go to: Insert > Features > Fillet/Round

Select the highlighted circular edge of the solid body, as shown in the image below

Go to the property manager and assign a Fillet radius  of 6.5mm

Click OK to complete the fillet operation.

Repeat the Fillet

Go to: Insert > Features > Fillet/Round

Select the highlighted circular edges of the solid body, as shown in the image below

Go to the property manager and assign a Fillet radius  of 3mm

Click OK to complete the fillet operation.

Make another Fillet

Go to: Insert > Features > Fillet/Round

Select the highlighted tapered faces of the solid body, as shown in the image below

Go to the property manager and assign a Fillet radius  of 10mm

Click OK to complete the fillet operation.

Change the Appearance

Go to: PhotoView 360 > Edit Appearance…

Select Appearances (color) >> Metal >> Steel >> Polished Steel

Double click on the Polished Steel  icon

Go to the property manager, select the brown color from the color pallete, as shown in the image below

Go to: View > Display

Select Shaded , Shadows In Shaded Mode  , and Ambient Occlusion

Save the File again

Congratulations, you just finished your organic rim. 🙂

I know it was a lot of work (so was writing this tutorial!) but I hope you learned a few new things about SOLIDWORKS.

Click here to download this SOLIDWORKS tutorial as a free eBook (PDF).

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Thanks a million ?

Jan