In today’s SOLIDWORKS tutorial, I will show you how to model the famous Panton Chair in SOLIDWORKS. Although the design of this organic chair dates from the sixties, it’s still a modern design chair.
The designer of this chair is Verner Panton. He was one of the most influential industrial designers of the sixties and seventies. Verner Panton was born in Denmark and later relocated to Switzerland. He became famous for his original and modern furniture designs. The Panton Chair is for sure one of the most recognizable chairs in the world. The design of this chair was inspired by the Zigzag chair of Gerrit Rietveld.
One of the ambitions of Verner Panton was to create a plastic chair molded in one single piece. Panton searched for a long time for a manufacturer of this modern chair. Finally, he found the company Vitra to develop the chair for series production. The Panton chair received many different awards and is now recognized as a classic of modern furniture design. Because the organic shape of this chair looks so interesting, I thought it would be nice to create a SOLIDWORKS tutorial about this chair.
Happy modeling! 🙂
Jan
P.S. I encourage you to share this SOLIDWORKS tutorial with your network.
Click here to download this SOLIDWORKS tutorial as a free eBook (PDF).
Disclaimer: The intellectual property depicted in this 3D model, is not affiliated with or endorsed by the original right holders. This 3D model may not be used for any commercial, promotional, advertising or merchandising use.
Open a New Part with model units set to millimeters
Go to: File > New > Part 
Save the file with the following name: Panton_Chair.SLDPRT 
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 > Centerline 
Draw a vertical centerline coincident to the origin
Go to: Tools > Dimensions > Smart 
Assign a vertical length of 580mm, as shown in the image below
Go to: Tools > Sketch Entities > Centerline
Draw a horizontal centerline starting from the origin
Draw two more horizontal centerlines starting coincidentally with the vertical centerline, as shown below
Go to: Tools > Dimensions > Smart
Assign the dimensions to the centerlines, as shown 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 Feature tree and click on the sketch icon
Go to: Tools > Sketch Entities > Spline 
Draw a spline passing through the red encircled points as showed in the image below
Click on the spline and drag on both spline handles to activate them
Hold the Alt key, and drag the middle two handles to maintain the tangent symmetry
Go to: Tools > Dimensions > Smart
Assign an angular dimension to each handle with their corresponding centerlines, as shown in the image below
Now click on each handle and assign the required handle lengths, as shown in the image below
Click on the Close sketch to close the sketch area
Go to the feature tree, click on Sketch1 and click on the Eye 
icon to hide it
Create a 2D Sketch on the Right Plane
Select the Right Plane from the Feature tree and click on the sketch icon
Go to: Tools > Sketch Tools > Convert Entities 
Click on the existing sketch to convert it into a line, as shown in the image below
Click OK 
to complete the operation
Now click on the converted line
Go to the property manager and tick the For construction checkbox
Go to: Tools > Sketch Tools > Centerline
Draw a horizontal centerline starting from the origin towards left
Go to: Tools > Dimensions > Smart
Click on the horizontal centerline and assign a length of 150mm, as shown in the image below
Go to: Tools > Sketch Tools > Line 
Draw a vertical centerline starting on the left end of the horizontal centerline
Go to: Tools > Dimensions > Smart
Click on the vertical centerline and assign a length of 280mm, as shown in the image below
Go to: Tools > Sketch Entities > Spline
Draw a two-point spline by using the upper points of the vertical lines, as shown in the image below
Click on the spline and drag on both spline handles to activate them
Click on the upper handle and choose the horizontal 
relation from the property manager
Hold CTRL key, select the vertical line of 280mm and the spline
Go to the property manager and choose the equal curvature 
relation, as shown in the image below
Go to: Tools > Dimensions > Smart
Click on the horizontal handle and assign the handle length of 400mm
Click on the vertical handle and assign the handle length of 600mm, as shown in the image below
Click on Close sketch to close the sketch area
Use the Project Curve Tool
Go to: Insert > Curve > Projected 
Go to the property manager and select Sketch on Sketch as a projection-type
Go to the modeling area and click on the Sketch2 and Sketch3
A projected curve is generated in yellow 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 > Centerline
Draw a vertical centerline coincident to the origin and the upper endpoint of the converted sketch
The coincident point is encircled in red in the image below
Draw a horizontal centerline starting from the origin
Draw three more horizontal centerlines starting coincidently with the vertical centerline, as shown below
Go to: Tools > Dimensions > Smart
Assign dimensions to the centerlines, as shown in the image below
Go to: Tools > Sketch Entities > Centerline
Draw a vertical centerline coincident to the horizontal centerline with a length of 360mm
Go to: Tools > Dimensions > Smart
Assign dimensions to the new vertical centerline, as shown in the image below
Click on the 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 > Spline
Draw a spline passing through the red encircled points of the Sketch4, as shown in the image below
Click on the spline and click on both spline handles to activate them
Hold down the Alt key and drag the middle two handles to maintain the tangent symmetry
Go to: Tools > Dimensions > Smart
Assign angular dimensions to each of the handles with their corresponding centerlines, as shown in the image below
Click on each handle and assign the required handle lengths, as shown in the image below
Click on Close sketch to close the sketch area
Go to feature tree, click on Sketch4 and hit the Eye icon to hide it
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 > Spine
Draw a two-point spline starting coincidentally from the lower endpoint of the previous sketch
Hold CTRL key, select the free endpoint of the spline and select the converted sketch
Go to the property manager and assign a Pierce 
relation between them, as shown in the image below
Click on the Normal To 
icon
Click on the spline and click on both spline handles to activate them
Click on the left handle and choose the Vertical 
relation from the property manager
Click on the right handle and choose the Horizontal relation from the property manager
Go to: Tools > Dimensions > Smart
Click on the vertical handle and assign a handle length of 300mm
Click on the horizontal handle and assign a handle length of 600mm
Click on Close sketch to close the sketch area
Create a Reference Plane (Plane1)
Go to: Insert > Reference Geometry > Plane… 
Go to the feature tree, select the Top Plane as a first reference 
Go to the modeling area, click on the encircled point of Sketch5 as a second reference, 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 > 3 Point Arc 
Draw a 3 point arc randomly on the sketch plane in the same orientation as shown in the image below
Hold down the CTRL key, select Point A and the Converted Sketch
Go to the property manager and assign a Pierce relation
Hold down the CTRL key, select Point B and Sketch5
Go to the property manager and assign a Pierce relation, as shown in the image below
Click on the Normal To icon
Click on the spline and drag on both spline handles to activate them
Hold down the CTRL key, select Point B of the arc and the Center point of the arc
Go to the property manager and assign a Horizontal relation, as shown in the image below
Click on Close sketch to close the sketch area
Make a Surface Loft:
Go to: Insert > Surface > Loft 
Go to the Property Manager > Loft > Profiles 
Click on the profiles selection box
Go to the modeling area, select Sketch5 and then the blue projected curve (Curve1)
Go to the Property Manager > Loft > Guide Curves 
Click on the guide curves selection box
Go to the modeling area, select Sketch6 and Sketch7 as a guide curve
Go to the Property Manager > Loft > Start/End Constraints
Open the Start/End Constraints tab
Click on the Start constraint and assign the influence Normal to Profile
Leave the End constraint as default as shown in the image below
Click OK to complete the surface loft 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 > Centerline
Draw a vertical centerline coincident to the origin and the upper end-point of the converted sketch
The coincident points are encircled in red in the image below
Go to feature tree, click on Surface-Loft1 and hit the Eye icon to hide it
Go to: Tools > Sketch Entities > Centerline
Draw a horizontal centerline starting from the origin
Draw a horizontal centerline starting from the top end of the vertical centerline
Draw two more horizontal centerlines starting coincidentally with the vertical centerline
Go to: Tools > Dimensions > Smart
Assign the dimensions to the centerlines, as shown 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 > Spline
Draw a spline passing through the red encircled points of Sketch9, as shown in the image below
Click on the spline and drag on both spline handles to activate them
Hold down the Alt key and drag the middle two handles to maintain the tangent symmetry
Go to: Tools > Dimensions > Smart
Assign an angular dimension to each handle with their corresponding centerlines, as shown in the image below
Now click on each handle and assign the required handle lengths, as shown in the image below.
Click on Close sketch to close the sketch area
Go to feature tree, click on Sketch9 and hit the Eye icon to hide it
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 Tools > Convert Entities
Click on the existing sketch to convert it into a line, as shown in the image below
Click OK to complete the operation
Now click on the converted line
Go to the property manager and tick the For construction checkbox
Go to: Tools > Sketch Tools > Centerline
Draw a horizontal centerline starting from the origin towards left
Go to: Tools > Dimensions > Smart
Click on the horizontal centerline and assign a length of 165mm, as shown in the image below
Go to: Tools > Sketch Tools > Line
Draw a vertical centerline starting from the end of the horizontal centerline
Go to: Tools > Dimensions > Smart
Click on the vertical centerline and assign a length of 280mm, as shown in the image below
Go to: Tools > Sketch Entities > Spline
Draw a two-point spline by using the upper points of the vertical lines, as shown in the image below
Click on the spline and drag on both spline handles to activate them
Click on the upper handle and choose the horizontal relation from the property manager
Hold down the CTRL key, select the vertical line of 280mm and the spline
Go to the property manager and choose the equal curvature relation, as shown in the image below
Go to: Tools > Dimensions > Smart
Click on the horizontal handle and assign a handle length of 400mm
Click on the vertical handle and assign a handle length of 600mm, as shown in the image below
Click on Close sketch to close the sketch area
Use the Project Curve Tool
Go to: Insert > Curve > Projected
Go to the property manager and select Sketch on Sketch as a projection-type
Go to the modeling area and click on Sketch9 and Sketch10
Then a projected curve is generated in yellow as shown in the image below
Click OK to complete the operation
Create a Reference Plane (Plane2)
Go to: Insert > Reference Geometry > Plane…
Go to the feature tree, select the right plane as a first reference
Go to the property manager and assign an offset distance of 150mm, as shown in the image below
Click OK to complete the operation
Go to feature tree, click on Surface-Loft1 and hit the Eye icon to unhide it
Create a 2D Sketch on Plane1
Select Plane1 from the Features tree and click on the sketch icon
Go to: Tools > Sketch Entities > Line
Draw a diagonal line as shown in the image below
Hold down the CTRL key, select Point A and the New Projected Curve
Go to the property manager and assign a Pierce relation
Hold down the CTRL key, select Point B and the Surface Edge
Go to the property manager and assign a Pierce relation, as shown in the image below
Click on Close sketch to close the sketch area
Go to feature tree, click on Plane2 and hit the Eye icon to unhide it
Use the Surface Loft
Go to: Insert > Surface > Loft
Go to the Property Manager > Loft > Profiles
Click on the profiles selection box
Go to the modeling area, select the surface edge (Edge<1>) and then the projected curve (Curve2)
Go to the Property Manager > Loft > Guide Curves
Click on the guide curves selection box
Go to the modeling area, select the straight line (Sketch11) as a guide curve
Leave the Start/End Constraints as default, as shown in the image below
Click OK to complete the surface loft operation
Use the Knit Surface
Go to: Insert > Surface > Knit… 
Go to the modeling area, select the two existing loft surfaces
Go to the property manager and check the Merge entities box, 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 and click on the second icon 
to activate variable fillets
Go to the modeling area, select the yellow highlighted surface edge, as shown in the image below
Click on the upper unassigned fillet box and assign a variable radius 
18mm
Click on the lower unassigned fillet box and assign a variable radius 2mm
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 
option
Open the feature tree and select the Front plane as the mirror plane
Go to the property manager and click on the Bodies to Mirror 
option
Move to the modeling area and select the knitted surface body, as shown in the image below
Click OK to complete the operation.
Use the Thicken
Go to: Insert > Boss/ Base > Thicken 
Select the existing Knitted surface as Thicken parameter 
from the modeling area
Go to the property manager, select the first icon as thickness type
Assign a thickness value of 
5mm, 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 > Corner Rectangle 
Draw a rectangle starting from the origin
Go to: Tools > Dimensions > Smart
Assign the dimension as shown in the image below
Click on Close sketch to close the sketch area
Make an Extrude Cut
Go to: Insert > Cut > Extrude… 
or click on Extrude Cut
Select the rectangular 2D sketch
Go to the Property Manager > Direction 1
Assign the extrude cut type Through All – Both, as shown in the image below
Click OK to complete the operation.
Make another fillet
Go to: Insert > Features > Fillet/Round
Select both highlighted edges, as shown in the image below
Go to the property manager and assign a fillet radius of 2.5mm
Click OK to complete the operation.
Make another fillet
Go to: Insert > Features > Fillet/Round
Select the flat bottom surface, as shown in the image below
Go to the property manager and assign a fillet radius of 1mm
Click OK to complete the operation.
Change the Appearance
Go to: PhotoView 360 > Edit Appearance… 
Select Appearances (color) > Plastics > High Gloss > Red High Gloss Plastic
Double click on the Red High Gloss Plastic 
icon
Click OK to apply the new appearance.
Go to: View > Display
Select Shaded 
, Shadows In Shaded Mode 
, and Ambient Occlusion 
(if possible)
The completed panton chair will look like the image below
Save the File again
Congratulations, you’ve just created your own Panton Chair in SOLIDWORKS!
I hope you liked this free SOLIDWORKS tutorial. Do you also want to learn an alternative way to model the Panton chair using blueprints? Then make sure to download the free eBook below.
Click here to download this free eBook (PDF).
I hope you liked this blogpost!
Do you want to help me spread this SOLIDWORKS 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
20 comments. Leave new
It’s awesome training guid for solidworks students to be a proffesional designer…….such ammezzing tutorials …..plz keep it up……
I am just learning SolidWorks, I hope to use this website for my training.
The pictures of the chair are really nice and beautiful: very modern! Great work!
Can I get help from this website if I ask for something about solidworks here? When I face any problem during designing in solidworks I seek help from someone or I search online. But most of the time, online help is not of much use because it cannot satisfy my specific query on a particular problem. I wish that this website will help me in this regard.
Hi Nazrul, you can always ask things at this website. I am sure I can help you with most points (or one of the other readers) I am currently developing a forum to post your questions about SolidWorks. Until that time you can drop your questions here! 🙂
Hello, Can I ask one question? What is the difference in content between Chopper Tutorial and E-book which is coming soon?
Hi Teresa,
The diiference is that I am currently developing a new tutorial for PhotoView360 and some more detailed SolidWorks starter tutorials. More information is comming soon 🙂
Hai mr Jan, could you help me to drawing chair in solidwork? tq
Hi Jonathan,
Send me your questions and I will take a look at it!
I actually found this more entretaining than James Joyce.
hi! i ‘m sathish
i think its very useful so i want free solidworks E-book may i download i’m already subscribed…………
Hi Satish,
Subscribe again and you’ll immediately have access to the free SolidWorks Panton tutorial.
Regards Jan
thanks man:),the material is gr8
really nice! The pictures of the chair are really nice and beautiful Great work!
Hi jan
tank a lot for your tutorial
these days , you dont send tutorial for me
may be you forget me
jan, I work with solidworks about 2 years and I like making tutorial or work with you.
could you help me?
again I say , Ilike solidworke and make tutorial
have good time.
Hi Mostafa,
Thanks for your message! I recommend you to take a look at my free Ebook section to find my latest SolidWorks tutorials: https://learnsolidworks.com/ebooks/ 🙂
very very nice………….. jan your tutorials are very perfect….please keep it up…..
thanks! 🙂
do you have channel on youtube ????
case I want to learn sold work and to be profisanl just like ??
Sure! Here’s a link to my Youtube channel: https://www.youtube.com/playlist?list=PLfP7xTlogaFoVj4vm8cPGvmDZdCkg_srN