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Making a truncated cone with holes removed

Firstly. I am new to OnShape but not new to modeling. I am attempting to make a shape that is a truncated cone (surface only) with circular holes cut in the cone around the circumference at 45 degree increments. (Firearm muzzle with holes in it). My attempt was to:
  1. Draw profile
  2. Revolve
  3. New Sketch
  4. Draw Circles
  5. Select the Circle Faces 
  6. Extrude/Remove (symmetrical to get 2 for one remove)
     If I pick anything other than "New" for the extrude it fails (Shows red cylinder). 

Even trickier is that I must have circles cut in the cone at increments of 45 degrees around the circumference of the revolve. 

So far it appears as if this is beyond the capabilities of OnShape but hopefully I'm wrong. Suggestions?

Comments

  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 3,954
    Hi Russell - any particular reason it needs to be a surface? If you model your cone as a solid it will work perfectly. At the moment it sounds like you are trying to do a solid extrude/remove feature on a surface which will not work. 
    Director, Technical Services, EMEAI
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 632
    Use a split face followed by a circular face pattern.  From here you just need to delete the split faces.

    1. Draw your cone and a sketch of where you want your holes to be.


    2. Select split and change to split face.  Add the surface as the face to split.


    3. Select the entire sketch from the feature list to be the entity to split with.  This will project the sketch in both directions and split the surface.  If you don't like that it goes both directions, you can extrude the surfaces out and add those to your entities to split with.


    4. Start a circular pattern and select face pattern.  Cross select everything to get all of the faces and then click on the cone to remove that selection (we don't want to pattern the cone).


    5. Select one of the edges of the cone for the axis of pattern, set the pattern angle to be 45 degrees and the count to be 180/45 (half-way around since we split at the back already).


    6. Start a delete face feature and box/cross select all of the faces.  Again, select the cone that we don't want to delete.


    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • russell_thorburnrussell_thorburn Member Posts: 2
    edited January 2016
    Thanks. I was mistaken. I actually did want a solid.I ended up simply using a series of translations and boolean subtractions to get what I wanted. Thanks so much for the help anyway as I learned something new from your answer. :-)  

    OnShape really is a fantastic product. It's exactly what I've been looking for.
  • MrDiLizioMrDiLizio Member Posts: 7
    I've made a video showing how to make the truncated cone - Hope it helps!

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