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davehaigh13-Aquamarine
13-Aquamarine
November 14, 2014
Question

sketcher known dim in Creo 2

  • November 14, 2014
  • 6 replies
  • 1421 views
How do you create a known dim in Creo 2.0?

David Haigh
Phone: 925-424-3931
Fax: 925-423-7496
Lawrence Livermore National Lab
7000 East Ave, L-362
Livermore, CA 94550

    6 replies

    M
    mlocascio1-Visitor
    1-Visitor
    November 14, 2014
    David,



    Are you referring to the idea of looking up (or showing) the dimension ID so
    that you can use it in a created dimension?



    Mike Locascio


    D
    davehaigh13-AquamarineAuthor
    13-Aquamarine
    November 14, 2014
    If you switch dims in the sketcher it supposed to have the symbol kd#

    You can then use it in a sketcher relation

    David Haigh
    M
    mlocascio1-Visitor
    1-Visitor
    November 14, 2014
    That's the idea. BUT it's NOT a "kd#" - it should be an "sd#"



    MPL


    D
    davehaigh13-AquamarineAuthor
    13-Aquamarine
    November 14, 2014
    From the help:
    sketcher_known_dim_on_ref_entity
    yes*, no
    Controls the type of dimension created for normal dimensions with only background geometry selected as references.
    yes-Creates known dimensions, for example kd#.
    no-Creates reference dimensions, for example, ref#.

    But I just want to create it not set a config to create it.
    Known dim's have been in ProE since the single digit revs of the software.

    David Haigh
    D
    davehaigh13-AquamarineAuthor
    13-Aquamarine
    November 14, 2014
    From Wildfire 4 help topic collection. How do I create one of these in Creo?

    About Known Dimensions
    A known dimension is a dimension for a single reference entity or between two
    reference entities. A known dimension is represented by the dimension symbol prefix
    kd#. In the Sketcher mode, you can use the references and known dimensions to
    create a relation.
    To Create Known Dimension
    1. Click Dimension on the Sketcher toolbar. Alternatively, click Dimension on the
    shortcut menu.
    2. Select two edges, two vertices, or datum entities.
    3. Middle-click at the required location to place the known dimension.
    To Create Known Dimension (OFF)
    1. Ensure that the Intent Manager is OFF on the Sketch menu.
    2. Click Sketch > Dimension. The DIMENSION menu appears.
    3. Click Known.
    4. Select two edges, two vertices, or datum entities.
    5. Middle-click at the required location to place the known dimension.
    To Use Known Dimensions (OFF)
    Known dimensions allow you to establish meaningful parametric dependencies when
    creating a section of a feature.
    1. Ensure that the Intent Manager is OFF on the Sketch menu.
    2. Sketch and dimension as usual.
    3. Create Known dimensions on part geometry that will be used to drive the
    feature section.
    4. From the Sketch menu, select Relation.
    5. Add relations connecting Normal section dimensions with the Known ones.
    6. When the system updates the section, values of normal dimensions change
    according to the relations.
    Dimensions driven by Sketcher relations cannot be modified directly. To access
    Sketcher relations, choose Redefine and Section. You can also do it in Part mode
    by choosing Relations, Feat Rel, selecting the feature, and choosing Section.

    David Haigh
    D
    dmartin11-Garnet
    11-Garnet
    November 14, 2014

    In general, you want to avoid Relations in sketches (aside from Variable Section Sweeps).


    But if you are writing a Relation in Sketcher, you can use Known Dimensions in them. A Known Dimension is simply a dimension that you create in Sketcher on model geometry, not on sketch geometry like lines, arcs, circles, and splines.


    For example, create a block and then create a sketch on one of the block's surfaces. When you go into Sketcer, before creating any entities, create a dimension from one side of the block to the other. That is a Known Dimension.


    I avoid Relations in sketches because I've seen them give permanent yellow regen status, and they are very hard to detect unless you search for them deliberately. About the only ways I know to find them are to Edit Definition of a sketch and then go to Tools > Relations, or in Part Mode open the Relations dialog box, change the Look In filter to Feature or Section, and select a sketch.



    David R. Martin II


    Senior CAD Application Specialist


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