123 solidworks surface tutorial cover

free solidworks tutorial -surface

type : tutorial ebook - PDF

whats in for audience: exercise solidworks surface tools by designing a shaver

target feature of tutotrial: solidworks surface

features used in tutorial:

  • solidworks sketch
  • solidworks 3d-sketch
  • solidworks surface loft
  • solidworks filled surface
  • solidworks knit surface
  • solidworks surface fillet
  • solidworks extrude

difficulty level: advanced

provided by: SolidWorksAdvisor (SWA)

price: free solidworks tutorial PDF book



download solidworks tutorial ebook

download the solidworks model


or you can read the tutorial below:

solidworks surface tutorial


Here we are going to design a schematic of this shaver:

123 solidworks surface tutorial 1

The purpose of this tutorial is to teach how to use solidworks surface tools so I don’t address all the details of a shaver here but you can get familiar with lots of surface tools.

This is an advanced tutorial so I don’t cover the solidworks basic skills like opening a new sketch or defining a plane etc… if you are a novice I recommend you to read the solidworks beginner tutorials first.

And here is my constant primary question before starting any tutorial from you as a designer:

Take another good look at the product, from where should you start to design?

Do you recognize any particular approach to get this done?

Try to answer the questions then start reading the tutorial.

When I look at the shaver I see these curves and sections:

123 solidworks surface tutorial 2

This is my recommended approach. Define all those sections and add the sidelong curves then loft them all together to make the basic shape. We need 7 sketches and 5 planes to make the above wireframe. In the following pages I’ll guide you to do it.

Sketch 1

  • On the top plane
  • Use solidworks slot tool to draw it
  • The centerline is mid-pointed on the origin

123 solidworks surface tutorial 3


  • Reference: top plane
  • Distance: 12 mm

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  • On the plane1
  • Draw by slot
  • Centerline mid-pointed on the origin

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  • Reference plane1
  • Distance 70mm

123 solidworks surface tutorial 5 2


  • On plane2
  • Draw with solidworks slot
  • Middle point of centerline has a horizontal relation with origin on 5mm distance

123 solidworks surface tutorial 6


  • Reference plane 2
  • Distance 35mm

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Sketch 4

  • On plane3
  • Draw with solidworks slot
  • Middle point of centerline has a horizontal relation with origin on 5mm distance

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  • Reference1: plane 3
  • Reference2: centerline of the sketch 4
  • Angle: 135deg

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When you are defining a diagonal plane with respect to another plane you need a rotation axis which is centerline of the slot in the sketch 4 in our example.


  • Reference plane 4
  • Distance 65mm

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Sketch 5

  • On plane 5
  • Draw a equilateral triangle first then fillet the vertexes
  • The lowest vertex has a vertical relation with the origin point

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Hide the planes. This is what we have done so far in isometric view. see those marked points in the following picture. We will use them to locate the sidelong curves but you don’t have them in your sketches right now because I added them manually and you will do so:

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To add these points to your sketches just open each sketch for editing then select the “point” tool in sketch toolbar and move your cursor to specified locations then solidworks shows the midpoint as the default option and you need to click to place the new point:

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Now we are going to add the first two guide curves using spline. Open a new sketch on the front plane and draw these two splines:

  • Run the spline command and click on each of the previous sketches
  • Pierce the spline points on the sketches using add relation tool
  • There are four free points just for controlling the curvature of the splines

Get the following result:

123 solidworks surface tutorial 14

Exit the sketch and save your work. The first two guide curves are planar which means you can draw them in one single plane-the front plant in our example here- but the next two guide curves are not planar, in fact they are 3d curves and we need to use the solidworks 3d-sketch tool.

Open a new 3d-sketch. if you don’t know how then just navigate to the sketch button on the sketch toolbar and click on the tiny triangle then choose 3d-sketch:

123 solidworks surface tutorial 15

You can sketch on multiple planes simultaneously in 3d-sketch mode. If you haven’t use this tool before then here is one of my 3d-sketch tutorials.

Select spline and draw these two splines. Its more than easy just run the spline tool and click on the points:

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It’s time to make our first surface using loft tool. Save your work before we proceed. Run the “lofted surface” from the surface toolbar:

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Surface loft window appears on the left. Select sketch1 to sketch5 as the profiles then select the four splines as the guide curves and see the preview:

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If you see the same result then click ok and save your work.

Wherever there is a boundary you can fill it with a surface. There is a boundary in our model and we need to close it with a surface so click on the filled surface button:

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the “surface-fill” window appears on the property manager just click on the boundary shown in the above picture then click ok.now you have a surface on the top:

123 solidworks surface tutorial 20

This is what we have done so far:

123 solidworks surface tutorial 21

When you add multiple surfaces to your part they are not connected as one single surface so the lofted surface is not connected to the filled surface here. We need to fillet the sharp edge at the top but first we need to connect the loft and filled surfaces. Solidworks knit surface tool will do the job for us. Just run the knit surface tool and select the surfaces then click ok:

123 solidworks surface tutorial 22

Now we have one integrated surface and we can do the fillet.

Run the fillet command. Select the edge and specify the radius then click ok:

123 solidworks surface tutorial 23

All we create by solidworks surface tools dont have any thickness. As the name implies they are only surfaces with zero thickness so if we want to perform other solidworks tools on this part we need to thicken it. its so easy just run the thicken command, choose the surface in the graphic area, set the thickness amount then click ok.

123 solidworks surface tutorial 24

Now the part has 0.5mm thickness. The surfacing is over and we work on the appearance of the model from now on.

Make it look like a shaver, add three shaving areas on the top using the extrude tool. Select the top face of the part and draw the sketch then extrude it:

123 solidworks surface tutorial 25

Add a power button(optional). Draw a sketch on the front plane using free splines then extrude it by the mid-plane condition:

123 solidworks surface tutorial 26

This is my finished model:

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I know that the color of your model is not like mine but you can change the color of any segment of the part separately. For example click on the top surface of the part in the working area and select the appearance then select “face1” then change the color in the color window. If you select the “thicken1” instead of “face1” then you will change the color of all the thicken surfaces.

123 solidworks surface tutorial 28

Mission accomplished. We have ourselves a shaver here:

123 solidworks surface tutorial 29

I’m done here but if you feel like that you need a more specified model then just go on and add some other features to your model. For example you can add a plug on the bottom of the model for charging. It’s all up to you from here on.




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