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How to Model a One Piece Knife in SOLIDWORKS

How to Model a One Piece Knife in SOLIDWORKS

Learn how to model the flowing shape of a one-piece knife in SOLIDWORKS using surface modeling tools. This step-by-step tutorial covers Surface Extrude, Trim Surface, Boundary Surface, Knit Surface, Thicken, and finishing details.

Inspired by the One Piece Knife designed by Johanna Gauder, this exercise explores how to create a continuous form from a single sheet of metal.

Download the free One Piece Knife SOLIDWORKS tutorial eBook.

Start the SOLIDWORKS Knife Model

I recently saw a beautiful knife that was crafted out of one piece of twisting metal.

It turned out to be the “One Piece Knife” designed by Johanna Gauder. This knife is made out of a stainless steel sheet and its flowing form isn’t interrupted by an added handle. In today’s tutorial, you will discover how to model this knife in SOLIDWORKS yourself.

Hope you like it!

Jan

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

Free SOLIDWORKS One-Piece Knife eBook

Download the free One Piece Knife SOLIDWORKS eBook (PDF).

Disclaimer: This independent educational 3D model is not affiliated with or endorsed by Johanna Gauder. It may not be used for commercial, promotional, advertising, or merchandising purposes.

Open a New Part with the model units set to millimeters

Go to: File > New > Part part icon

Save the File with the following name: One Piece Knife.SLDPRT save icon in solidworks

Create a 2D Sketch on the Right Plane

Select the Right Plane from the Features tree and click on the sketch icon sketch icon

Go to: Tools > Sketch Entities > Circle Circle

Draw a circle concentric to the origin

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Click on the circle and assign a diameter of 20mm, as shown in the image below

One Piece Knife SOLIDWORKS tutorial step 001

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

Create a Surface Extrude

Go to: Insert > Surface > Extrude… Extrude surface in solidworks

Select the circle sketch

Go to the Property manager > Direction1

Select Blind and click on the flip direction Flip direction icon in solidworks icon to reverse the surface extrude direction

Assign an Extrude length of 250mm

Assign a Draft angle Draft angle in surface extrude of 3 degrees and check the Draft outward box

surface extrude in solidworks

Click OK ok icon 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 sketch icon

Go to: Tools > Sketch Entities > Line Line

Draw a horizontal and vertical line as shown in the image below

One Piece Knife SOLIDWORKS tutorial step 003

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Hold the CTRL key and select the vertical line and the origin, then assign the length of 80mm

Use the Surface Trim

Go to:  Insert > Surface > Trim… surface trim

Select the purple section of the surface as shown in the image below

surface trim in solidworks

Go to the property manager and select Remove Selections

Leave the other parameters as default

Click OK ok icon 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

Click on the Normal To Normal To icon icon to switch the view direction

Go to: Tools > Sketch Entities > Spline spline in solidworks

Draw a spline without any midpoints as shown in the image below

2d spline in solidworks

Hold the CTRL key, select the spline and the surface edge1

Then, add a tangent relation Tangent relation in solidworks between them

Again, hold the CTRL key, select the spline and surface edge2

Then, assign another tangent relation Tangent relation in solidworks

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Click on each spline handle and add handle values of 100mm and 300mm as shown in the image below

2d spline in solidworks

Use the Surface Trim

Go to:  Insert > Surface > Trim… surface trim

Select the purple section of the surface as shown in the image below

surface trim in solidworks

Go to the property manager and select Remove Selections and leave the other parameters as default

Click OK ok icon 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 > Spline spline in solidworks

Draw a two point straight spline from the origin up to the next point, as shown in the image below

2d spline in solidworks

Click on the spline endpoints to activate the spline handles

Hold the CTRL key, select the spline and the Surface Edge

Then, assign a tangent relation Tangent relation in solidworks between them

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Click on each handle and assign the dimensions as showed in the image below

2d spline in solidworks

Go to: Tools > Sketch Entities > Spline spline in solidworks

Again, draw a two point straight spline just under the origin up to the vertical surface edge

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

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Click on each handle and assign the dimensions as showed in the image below

2d spline in solidworks

Hold the CTRL key, select the two right endpoints of both splines

Then, assign a parallel relation  between them, as shown in the image below

2d spline in solidworks

Use the Surface Trim

Go to:  Insert > Surface > Trim… surface trim

Click on the purple surface between the two splines as shown in the image below

Surface trim in solidworks

Go to the property manager and select Remove Selections and leave the other parameters as default

Click OK ok icon 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 sketch icon

Click on the Normal To Normal To icon icon to rotate the view 180 degrees

Go to: Tools > Sketch Entities > Spline spline in solidworks

Draw a spline without midpoints as shown in the image below

2d spline in solidworks

Make sure that Point 1 and the Point 2 are coincident to eachother, as showed in the image above

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

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Click on each handle and assign the dimensions as showed in the image below

2d splines in solidworks

Use the Surface Trim

Go to:  Insert > Surface > Trim… surface trim

Click on the purple surface section as shown in the image below

Surface trim in solidworks

Go to the property manager and select Remove Selections and leave the other parameters as default

Click OK ok icon to complete the operation.

Create a Reference Plane (Plane1)

Go to:  Insert > Reference Geometry > Plane… solidworks Reference Plane

Click on the horizontal surface edge (Edge<1>) then click on the existing surface (Face <1>)

The generated plane is highlighted in yellow as shown in the image below

Reference plane in solidworks

Click OK ok icon to complete the operation

Create a 2D Sketch on Plane1

Select Plane1 from the Feature tree and click on the sketch icon

Go to: Tools > Sketch Entities > Line Line

Create a horizontal line and a vertical line

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Assign the dimensions to both lines as showed in the image below

One Piece Knife SOLIDWORKS tutorial step 017

Go to: Tools > Sketch Entities > Spline spline in solidworks

Create a two point spline as shown in the image below

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Add dimensions to the spline as shown in the image below

One Piece Knife SOLIDWORKS tutorial step 018

Use the Planar Surface feature

Go to:  Insert > Surface > Planar… planar surface

The current sketch (Sketch6) automatically gets selected

In the modelling area a yellow enclosed flat surface is generated, as shown in the image below

Planar surface command in solidworks

Click OK ok icon to complete the operation

Create a 3D Sketch

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

Go to: Insert > 3D sketch 3d sketch icon in solidworks

Go to: Tools > Sketch Entities > Center Line center line or click directly on Center Line

Create a vertical construction line with an angle of 15 degrees, as shown in the image below

One Piece Knife SOLIDWORKS tutorial step 020

Go to: Tools > Sketch Entities > Spline spline in solidworks

Draw a spline between Point A and Point B

Hold the CTRL key, select the spline and the highlighted Curved Edge

Add a tangent relation Tangent relation in solidworks between them, as shown in the image below

One Piece Knife SOLIDWORKS tutorial step 021

Hold the CTRL key, select the spline and the diagonal construction line

Assign a tangent relation Tangent relation in solidworks between them, as shown in the image below

One Piece Knife SOLIDWORKS tutorial step 022

Go to: Tools > Dimensions > Smart solidworks Polygon tool

Assign the dimensions to the spline handles as showed in the image below

One Piece Knife SOLIDWORKS tutorial step 023

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

Create a 2D Sketch on the Front Plane

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

Go to: Tools > Sketch Entities > Line Line

Create a vertical line coincident to Point A as shown in the image below

One Piece Knife SOLIDWORKS tutorial step 024

Use a Split Line

Go to:  Insert > Curve > Split Line Split line tool in solidworks

Go to the property manger, Select Projection as a Type of Split

Select the current sketch from the modelling area

The selected sketch is shown as Current Sketch in the Sketch to Project Sketch selection in split line tool in solidworks dialog box

Then, click on the  curved surface (highlighted in blue) from the modelling area to split it

The selected surface is shown as Face<1> in the Face to Split Faces to split in solidworks dialog box

Split line tool in solidworks

Click OK ok icon to complete the operation.

Use the Boundary Surface

Go to:  Insert > Surface > Boundary Surface… Boundary surface in solidworks

Go to the property manager, click on the Direction1 box

Move to the modelling area, click on Edge 1 and Edge 2, as shown in the image below

Boundary surface in solidworks

 Go to the property manager, Click on the Direction2 box

Move to the modelling area, click on Edge 3 and 3D Sketch1, as shown in the image below

Boundary surface in solidworks

Go to the property manager, click on Edge <1> from the Direction 1 dialogue box

Assign the influence – Tangency to Face with Tangent Influence (%): 100

Click on the Edge <2> from the Direction 1 dialogue box

Assign the influence – Tangency to Face with Tangent Influence (%): 100

Go down in Direction 2 dialogue box and click on the Edge <3>

Assign the influence – Tangency to Face with Tangent Influence (%): 100

Click on the 3D Sketch 1 from Direction 2 dialogue box

Assign the influence None

Click OK ok icon to complete the operation.

Use the Knit Surface

Go to:  Insert > Surface > Knit… knit surfaces

Select the three existing surfaces from the modelling area

Go to the property manager and check the merge entities box, as shown in the image below

Knit surface in solidworks

Click OK ok icon to complete the operation.

Use the Thicken feature

Go to: Insert > Boss/ Base > Thicken thicken

Select the existing Knitted surface as Thicken parameter Thicken faces from the modelling area

Go to the property manager, select the first icon one side thicken icon as thickness type

Assign a thickness value Thickness value of 1.5mm  and check the Merge result option

Thicken command in solidworks

Click OK ok icon to complete the operation.

Make a Chamfer

Go to: Insert > Features > Chamfer Chamfer Tool in solidworks

Select the highlighted curved edge of the knife, as highlighted in yellow in the image below

Chamfer tool in solidworks

Go to the property manager and select Angle distance from the chamfer parameters

Assign the chamfer distance offset distance of 1.5mm and the chamfer angle Angular Value of 80 degrees

Leave the other options as default

Click OK ok icon to complete the operation.

Add some Fillets

Go to: Insert > Features > Fillet/Round solidworks Fillet

Select the two tiny straight edges of the knife

The selected edges are highlighted in yellow as shown in the image below

Fillet on edges in solidworks

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

Click OK ok icon to complete the operation.

Add another Fillet

Go to: Insert > Features > Fillet/Round solidworks Fillet

Right click on the Fillet Edge 1

Select Tangency from the pop up menu to select all the tangent edges.

Similarly, right click on the Fillet Edge 2

Select Tangency from the pop up menu to select all the tangent edges.

If some edges are left, select them manually

All selected edges are highlighted in yellow, as shown in the image below

Fillet on edges in solidworks

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

Click OK ok icon to complete the operation.

Use the Move/ Copy Body Tool – to Orient the Knife

Go to: Insert > Features > Move/ Copy… Move-copy bodies

Select the knife from the modelling area, as shown in the image below

Move/copy body feature in solidworks

Go to the property manager and click on the Rotate rotate reference/ translate reference option

Assign rotation values around X, Y and Z Axis

x-angular value X= -95 degrees, y-value Y= 90 degrees, and z- angular value Z= 3 degrees

Leave the translation values as default

Click OK ok icon to complete the operation.

Change the Appearance

Go to: PhotoView 360 > Edit Appearance… Edit appereance in solidworks

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

Double click on the Polished Steel icon

Change appearance in solidworks

Click OK ok icon to apply the new appearance

Go to: View > Display

Select Shaded Shaded mode in solidworks, Shadows In Shaded Mode Shadow in shaded mode , and Ambient Occlusion Real view graphics (If possible)

The whole Knife will look like as shown in the image below

Real View image of the geometry

Save the File again save icon in solidworks

Congratulations, you just finished your own One Piece knife in SOLIDWORKS!

Free SOLIDWORKS One-Piece Knife eBook

Download the free One Piece Knife SOLIDWORKS eBook (PDF).

I hope you liked this LearnSOLIDWORKS tutorial!

Do you want to help me spread this tutorial with your network?

You can do this by using the social media bar on this page. Every share is greatly appreciated. This allows me to reach more people and develop more valuable SOLIDWORKS tutorials for you.

Thanks a million!

Jan

Download the Free One Piece Knife SOLIDWORKS Tutorial

Want to follow these steps at your own pace? Get the free One Piece Knife eBook (PDF).

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