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Tutorial - How to create raised text on a curved surface

david_grossdavid_gross Member Posts: 10 ✭✭
edited October 2015 in Using Onshape

This tutorial is for creating raised lettering/sketches on a curved surface.  The surface can be a cylinder, sphere, cone, dome or any other non-plane configuration. I hope you will find this useful!

1.       Choose a sketch plane from which you want to project the lettering.  This can be one of the three native planes or a user-created plane.  Note that there is a front and a back side to a plane, where lettering will appear normal on the front side and in reverse on the back side.  This applies to both native planes and user-created planes. You can tell which side you are on by the direction of the plane name (for native planes) or by sketching text on the plane. If you want to project from the front side, then the lettering will appear normal, but if you want to project lettering from the back side, you will need to create a reverse-direction plane.


  • david_grossdavid_gross Member Posts: 10 ✭✭

    2.       To create a reverse-direction plane, first make sure you have an existing sketch line coincident with the new plane or create a new sketch to draw one. Click the Plane icon to create a new plane and select type Line Angle in dropdown. Select the desired sketch line and enter 0 degrees for the angle. Now create a new sketch on this plane and insert some text. If it is in the proper direction, you can proceed. If not, go back and edit the plane and enter angle of 180 degrees to flip it. The text should now be in the proper direction.  I have not discovered any rule to know which direction a plane will be when created so it is easiest just to start with 0 degrees and sketch on the plane to find the orientation. You can also tell by the orientation of the sketch label which appears on the sketch plane when in sketch mode.

  • david_grossdavid_gross Member Posts: 10 ✭✭

    3.       Now place the text that you want to project on the desired plane. I have placed the text on a plane behind the surface to be projected on but you could also create the sketch plane in front of the surface. The “text” does not need to be just text but can be any closed sketch or sketches  like a logo, shape or spline as I have done for the word “Wizard”.

  • david_grossdavid_gross Member Posts: 10 ✭✭

    4.       Now you will need to create a new surface (not a solid) which is offset from the surface where the text will be by the height of the text. Otherwise the text will just project to the surface and be invisible. Here I have created another domed surface offset by 1 mm.

  • david_grossdavid_gross Member Posts: 10 ✭✭
    5.    Now you are ready to extrude your text sketch. Click the Extrude icon and choose options Solid, Add, select type ‘Up to face’ and select the text sketch or portions of the sketch you want to extrude. For the ‘Up to face’ criteria, select the offset surface. This will be the maximum extrusion distance from the sketch plane. If the text extrudes the wrong direction, click the flip arrow to correct it. For Merge scope criteria (bottom box), select the part to merge the text into. You should now have text extruding from the sketch plane to the offset surface. If this is what you want, you are done. However, if you want to extrude the text only from the part surface or hide the extrusion within the body of the part, go on to the next step.

  • david_grossdavid_gross Member Posts: 10 ✭✭

    6.       In the Extrude dialog box, click the box for ‘Second end position’, choose option ‘Up to face’ and select the desired face where you want the text to start as the criteria. This will be the minimum extrusion distance from the sketch plane. Here I have chosen the front surface of the hub. Now hide the offset surface and you should have text that is raised above the surface by the offset distance.

  • david_grossdavid_gross Member Posts: 10 ✭✭

    7.       The above steps are for a sketch plane behind the surface that you want the text to extrude from.  If the sketch plane is in front of the surface, just reverse the faces in the Extrude tool so that the first end position is the part face that the text is on and the second end position is the offset surface. It helps to remember these as maximum extrude distance for first end position and minimum extrude distance for second as above.  This is shown in the picture below.

  • david_grossdavid_gross Member Posts: 10 ✭✭

    8.       Note that you can also select the New option rather than Add for the extrusion, which will create a new part for each letter or closed sketch portion. This can create a lot of new parts so it is best to just select Add for the extrusion so it will merge with the existing solid. An exception is if you want to change the appearance of the text such as color, in which case it needs to be created as new part(s).

    That's it!  Please comment if you have any tips/suggestions/improvements for doing this.  Happy texting!

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    edited October 2015
    That's impressively clear, informative and useful.
    The tip for creating a reverse plane is particularly handy, until such time as Onshape implement a "flip plane" control.
    Muchos kudos, and thanks VERY much!
  • david_grossdavid_gross Member Posts: 10 ✭✭
    edited October 2015
  • david_grossdavid_gross Member Posts: 10 ✭✭
    Thanks Andrew!  You are welcome.
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,440 PRO
    This is very useful tutorial until we can sketch directly to curved surface. Thanks @david_gross for taking time to produce exact and clear instructions for this 'workaround'.

  • shashank_aaryashashank_aarya Member Posts: 265 ✭✭✭
    @david_gross This is an excellent information! Thanks very much!
  • owen_craigowen_craig Member Posts: 5
    How did you hide the offset plane? I am unable to hide it and reveal the text on the surface. 
  • owen_craigowen_craig Member Posts: 5
    How did you hide the offset surface? 
  • NoloWSUNoloWSU Member Posts: 1
    You hide the offset surface by scrolling down to the bottom box where shows Parts and then below parts will be Surfaces.
    When you created the offset it created a new surface.
    You cannot hide it from the Offset Surface entity. 

    @david_gross Great tutorial! Very helpful. 
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