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.
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 ![]()
Save the File with the following name: One Piece Knife.SLDPRT ![]()
Create a 2D Sketch on the Right Plane
Select the Right Plane from the Features tree and click on the sketch icon ![]()
Go to: Tools > Sketch Entities > Circle ![]()
Draw a circle concentric to the origin
Go to: Tools > Dimensions > Smart ![]()
Click on the circle and assign a diameter of 20mm, as shown in the image below

Click on the Close sketch icon
to close the sketch area.
Create a Surface Extrude
Go to: Insert > Surface > Extrude… ![]()
Select the circle sketch
Go to the Property manager > Direction1
Select Blind and click on the flip direction
icon to reverse the surface extrude direction
Assign an Extrude length
of 250mm
Assign a Draft angle
of 3 degrees and check the Draft outward box

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 horizontal and vertical line as shown in the image below

Go to: Tools > Dimensions > Smart ![]()
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… ![]()
Select the purple section of the surface as shown in the image below

Go to the property manager and select Remove Selections
Leave the other parameters as default
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 ![]()
Click on the Normal To
icon to switch the view direction
Go to: Tools > Sketch Entities > Spline ![]()
Draw a spline without any midpoints as shown in the image below

Hold the CTRL key, select the spline and the surface edge1
Then, add a tangent relation
between them
Again, hold the CTRL key, select the spline and surface edge2
Then, assign another tangent relation ![]()
Go to: Tools > Dimensions > Smart ![]()
Click on each spline handle and add handle values of 100mm and 300mm as shown in the image below

Use the Surface Trim
Go to: Insert > Surface > Trim… ![]()
Select the purple section of the surface as shown in the image below

Go to the property manager and select Remove Selections and leave the other parameters as default
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 > Spline ![]()
Draw a two point straight spline from the origin up to the next point, as shown in the image below

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
between them
Go to: Tools > Dimensions > Smart ![]()
Click on each handle and assign the dimensions as showed in the image below

Go to: Tools > Sketch Entities > Spline ![]()
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 ![]()
Click on each handle and assign the dimensions as showed in the image below

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

Use the Surface Trim
Go to: Insert > Surface > Trim… ![]()
Click on the purple surface between the two splines as shown in the image below

Go to the property manager and select Remove Selections and leave the other parameters as default
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 ![]()
Click on the Normal To
icon to rotate the view 180 degrees
Go to: Tools > Sketch Entities > Spline ![]()
Draw a spline without midpoints as shown in the image below

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 ![]()
Click on each handle and assign the dimensions as showed in the image below

Use the Surface Trim
Go to: Insert > Surface > Trim… ![]()
Click on the purple surface section as shown in the image below

Go to the property manager and select Remove Selections and leave the other parameters as default
Click OK
to complete the operation.
Create a Reference Plane (Plane1)
Go to: Insert > Reference Geometry > 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

Click OK
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 ![]()
Create a horizontal line and a vertical line
Go to: Tools > Dimensions > Smart ![]()
Assign the dimensions to both lines as showed in the image below

Go to: Tools > Sketch Entities > Spline ![]()
Create a two point spline as shown in the image below
Go to: Tools > Dimensions > Smart ![]()
Add dimensions to the spline as shown in the image below

Use the Planar Surface feature
Go to: Insert > Surface > Planar… ![]()
The current sketch (Sketch6) automatically gets selected
In the modelling area a yellow enclosed flat surface is generated, as shown in the image below

Click OK
to complete the operation
Create a 3D Sketch
Select the Front Plane from the Feature tree and click on the sketch icon ![]()
Go to: Insert > 3D sketch ![]()
Go to: Tools > Sketch Entities > 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

Go to: Tools > Sketch Entities > Spline ![]()
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
between them, as shown in the image below

Hold the CTRL key, select the spline and the diagonal construction line
Assign a tangent relation
between them, as shown in the image below

Go to: Tools > Dimensions > Smart ![]()
Assign the dimensions to the spline handles as showed in the image below

Click on 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 ![]()
Create a vertical line coincident to Point A as shown in the image below

Use a Split Line
Go to: Insert > Curve > Split Line ![]()
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
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
dialog box

Click OK
to complete the operation.
Use the Boundary Surface
Go to: Insert > Surface > Boundary Surface… ![]()
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

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

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
to complete the operation.
Use the Knit Surface
Go to: Insert > Surface > Knit… ![]()
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

Click OK
to complete the operation.
Use the Thicken feature
Go to: Insert > Boss/ Base > Thicken ![]()
Select the existing Knitted surface as Thicken parameter
from the modelling area
Go to the property manager, select the first icon
as thickness type
Assign a thickness value
of 1.5mm and check the Merge result option

Click OK
to complete the operation.
Make a Chamfer
Go to: Insert > Features > Chamfer ![]()
Select the highlighted curved edge of the knife, as highlighted in yellow in the image below

Go to the property manager and select Angle distance from the chamfer parameters
Assign the chamfer distance
of 1.5mm and the chamfer angle
of 80 degrees
Leave the other options as default
Click OK
to complete the operation.
Add some Fillets
Go to: Insert > Features > Fillet/Round ![]()
Select the two tiny straight edges of the knife
The selected edges are highlighted in yellow as shown in the image below

Go to the property manager and assign a Fillet radius
of 1mm
Click OK
to complete the operation.
Add another Fillet
Go to: Insert > Features > Fillet/Round ![]()
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

Go to the property manager and assign a Fillet radius
of 0.75mm
Click OK
to complete the operation.
Use the Move/ Copy Body Tool – to Orient the Knife
Go to: Insert > Features > Move/ Copy… ![]()
Select the knife from the modelling area, as shown in the image below

Go to the property manager and click on the Rotate
option
Assign rotation values around X, Y and Z Axis
X= -95 degrees,
Y= 90 degrees, and
Z= 3 degrees
Leave the translation values as default
Click OK
to complete the operation.
Change the Appearance
Go to: PhotoView 360 > Edit Appearance… ![]()
Select Appearances (color) >> Metal >> Steel >> Polished Steel
Double click on the Polished Steel icon

Click OK
to apply the new appearance
Go to: View > Display
Select Shaded
, Shadows In Shaded Mode
, and Ambient Occlusion
(If possible)
The whole Knife will look like as shown in the image below

Save the File again ![]()
Congratulations, you just finished your own One Piece knife in SOLIDWORKS!
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).







6 Comments. Leave new
Thanks for choosing my knife, looks pretty amazing 🙂
You’re very welcome Johanna! I simply love the simplicity of your design 🙂
Great tutorial, unfortunately I stuck on Surface- Trim 4:
“Rebuild Errors: Cannot partition surface, the trim tool and target do not intersect. If the trim tool is a 3D sketch, make sure the 3D sketch segments are coincident to the surface you are trimming.”
Hi Tomasz, thanks for your message. Make sure that your trim line is fully intersecting the entire surface you want to tri. It doesn’t matter if the line is longer than the surface.
Hope this helps! 🙂
Jan
Awesome tutorial Jan, however I got stuck at Insert > Boss/ Base > Thicken. After I insert the 1.5mm value the merge results option does not show up.
Try to reverse the direction of thicken. Hope it helps.