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Positioning on the face of a surface with snaps

Discussion in 'Using Alibre Design' started by gtz01, Apr 8, 2021.

  1. gtz01

    gtz01 Member

    Suppose that I have an extruded object I want to make a sketch on.


    Something common I might do is create a sketch to cut a hole on either side, or at the midpoint of the object. So, using the measuring tool I can take the lengths of the sides of this object and figure out where the midpoint is, offsetting it from the origin using construction lines.


    But this seems like "reaching around your head to touch your nose". It would be far easier if I could snap a construction line to the midpoint of the surface in question and then project a construction line from that point. Additionally, this would make finding the midpoint of shapes that are not linear far easier.

    Is there a way to do this that doesnt involve this way?
     
  2. HaroldL

    HaroldL Alibre Super User

    Start your sketch then select either the face or the edge then use Project to Sketch to create Reference geometry. You can then sketch from the circle to the Mid point of the edge reference line.

    P-to-S.png
     
    Last edited: Apr 8, 2021
    gtz01 likes this.
  3. OTE_TheMissile

    OTE_TheMissile Alibre Super User

    I'll often do something similar to what Harold suggested. In my case, if I wanted the circle to always be at the geometric center of the feature, the first thing I'd do in the Sketch is draw a reference line diagonally across the part, then Coincident constrain the endpoints to either of the parallel edges. That will cause the edges themselves to appear as reference lines with their own endpoints, so I'll Coincident constrain the endpoints of the diagonal line I drew with those so they stay exactly at the corners of the part.

    Then I draw a circle on the midpoint of my diagonal line and I'm done.

    Untitled.png

    I've also done it in the other direction where if the circle in the center of the part is more critical than the body of the part, (i.e., if the part is symmetrical in both directions) I'll start by centering the rectangular Sketch around the origin, then draw the circle Sketch directly on the origin.
     
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  4. Oldbelt

    Oldbelt Senior Member

    Keep it simple
     

    Attached Files:

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  5. idslk

    idslk Alibre Super User

    Hello @gtz01 ,

    have you taken a look to the reference videos? This one will show you one solution (of a lot) for your question...
    Btw. you can put images from the snipping tool directly into your posts without using the gallery...

    Regards
    Stefan
     
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  6. OTE_TheMissile

    OTE_TheMissile Alibre Super User

    Or if you REALLY want to look clever...

    Untitled.png
     
  7. DV410

    DV410 New Member

    I make a habit of always trying to draw things centered on the origin for this reason and also in that it often makes assembly constraints easier.

    Drawing the box, use the drop-down to choose the "Rectangle by Center"
    Click the origin, size the box and then add a horizontal or verticle constraint.
    Extrude, but choose by Type = Midplane

    This puts the box centered on the origin.
    Then, add a sketch on the face and the origin is in the center ready for a circle to be snapped to.

    I feel that this is fewer clicks than drawing diagonals and can aid in further processing later.

    Centered box.PNG
     

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