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Bolt circle centerline

Discussion in 'General Discussion' started by Larry, Jun 3, 2020.

  1. Larry

    Larry Member

    Did a quick search of the forum, nothing I could find in the help files either...

    In the Part view, I have a series of holes inserted with the "Circular Feature Pattern". In the Drawing view I wish to dimension these holes with a circular center-line (bolt circle, dashed), and an angle.

    Selecting "insert centers" only places the radial portion of the center, not the overall bolt circle (dashed).

    Any suggestions appreciated.

  2. Hunter

    Hunter Senior Member

    I would also greatly appreciate to know how to do this! And something not requiring sketches in drawing views.
  3. DavidJ

    DavidJ Alibre Super User Staff Member

    Do you have Circular hole pattern PCD checked in the Detailing ?
    If so just insert centres into the view.
    Hunter likes this.
  4. Larry

    Larry Member

    Thanks David,

    The "File Properties" set-up is the same as you indicate - what I get is the radial portion of the center-line, the full bolt circle doesn't appear.

    The only change I see is that if the "Show Tangent For Centers" is checked, then an orthogonal (to the radial) center is placed.

    Perhaps it has to do with the way it was created in the Part view. The first hole was placed using orthogonal dimensions, then the pattern was placed using the "Circular Feature Pattern". Maybe Alibre got confused.
  5. Hunter

    Hunter Senior Member

    Ahhh, I didn't think to look there - still getting used to the autogeneration built-ins that Alibre has on offer. I'm starting to use the autodims more and more too, you just need to model your 3D correctly and then it works surprisingly well.

    Thanks, David
  6. DavidJ

    DavidJ Alibre Super User Staff Member

    Larry - were your holes really 'holes', or were they 'cuts' ?

    The automatic PCD thing only works for holes.
  7. simonb65

    simonb65 Alibre Super User

    Does it also rely on using a hole radial pattern operation too? i.e the holes can't just be individually placed.
  8. DavidJ

    DavidJ Alibre Super User Staff Member

    Correct - the OP mentioned he'd used circular feature pattern.
    simonb65 likes this.
  9. Larry

    Larry Member


    No, not cuts. I have found a way to create what I need: but, it seems that this has to be specified when the view is first created from the Part file.

    Attempting to add the bolt circle afterwards doesn't seem to work.

    Thanks again,

    BeEdHa likes this.
  10. simonb65

    simonb65 Alibre Super User

    Didn't read that fully David. I was just looking for verification myself. Thanks.
  11. Larry

    Larry Member

    Revisiting this... included is a practice part with some circular slots for which I'd like to generate centerlines. Should look much as the sample .jpg image with radial centerlines for each slot, and a circular (bolt circle) centerline.

    Is there a way to do this from the part file included ? Or is there a preferred way to generate the sketch such that it is possible ? Thanks.


    Attached Files:

  12. DavidJ

    DavidJ Alibre Super User Staff Member

    Add centres to the arc at each end of each slot - then edit centre marks to get the 'direction' correct. Have tweaked you drawing to show the idea.

    The lines are trickier - I had to apply an unwanted constraint, then undo it, to get the needed nodes to display permanently. Then I could constrain the lines co-incident with the nodes at arc ends.

    Attached Files:

    Last edited: Jun 24, 2020
  13. wazzu83

    wazzu83 Member


    I used a different approach. In 2d Drawing workspace / sketch in view mode ...

    1. Added 2 points
    2. Constrained each to arcs at end of a slot with concentric constraint
    3. Added 1 point
    4. Constrained to center of major or minor arc radius (either gives same result) with concentric constraint
    5. Draw circle / change layer to CL layer
    6. Constrain to center (point in step 4)
    7. Constrain circle path to slot center (either point in step 2)
    8. Draw CL in "V" shape with vertex at center / change layer to CL layer
    9. Constrain centerlines to arc centers
    10. Use Circular Pattern tool to rotate "V" pattern around the part.

    Attached Files:

  14. idslk

    idslk Alibre Super User

    "Thousand ways to rome" ;-)

    Attached Files:

    DavidJ likes this.
  15. HaroldL

    HaroldL Alibre Super User

    Either method is a lot of extra work to create something that should be native in Alibre. In the meantime maybe someone could/should write a script.
  16. Larry

    Larry Member

    Thanks all... do appreciate the replies, and the thought/effort that went into them

    DavidJ, I did already try the method of tweaking the centerline (cross) orientation - I'll now give a go with the idslk and wazzu83 methods. Both ideas seem to give the results required.

    I do agree with HaroldL though, this should be built into the software.

  17. NateLiqGrav

    NateLiqGrav Alibre Super User

    Alibre Script has no print/drawing ability and the API is vastly lacking in its print/drawing ability.
  18. HaroldL

    HaroldL Alibre Super User

    That's too bad. Another Alibre deficiency.:(

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