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JamesBurcham1-Visitor
1-Visitor
September 16, 2015
Solved

Center of Gravity Icon?

I wondering if someone can help me with a simple way to display the CG of a model.  I know in the past I have seen models that had a small sphere at the CG, but I have no idea how they placed it.

    scookeAnswer
    1-Visitor
    September 16, 2015

    The easy way.....If you have the right module create a mass properties feature (See attached image) and you can check the create point at COG option at the bottom (Mine is greyed out because we don't have that module.)

    MWSnap002 2015-09-16, 17_34_04.jpg

    The more difficult way....You could probably write some relations that take info from the mass properties parameters and use them to drive the location of your COG point.  See image below.  That means your point will stay at the COG as the model changes.  Then model a surface sphere as suggested at the point.

    MWSnap003 2015-09-16, 17_40_45.jpg

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    10 replies

    DeanLong1-Visitor
    1-Visitor
    September 16, 2015

    It's an old school method....

    Run a mass props and find record the X,Y and Z coordinates. Add a Datum Point at that location, create a revolved surface sphere as large as you like. Add some vector arrows if you wish. I like the sphere method because I can see it from any view orientation.

    If you change your model, just rerun the mass and edit your point's coordinates and the sphere will follow.

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    JamesBurcham1-VisitorAuthor
    1-Visitor
    September 16, 2015

    Thanks for the response,

    The issue I have with that method is that if the CG changes the sphere won't move.  I'm wondering of there is a way to place an indicator that moves with the CG as items are added or removed from an assembly.

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    Chris3
    Chris321-Topaz I
    21-Topaz I
    September 16, 2015

    If you change the analysis to "Feature" you can then have it create a dynamic point that will move.

    In Creo the steps are: Analaysis -> Mass Properties -> Change the drop down to "Feature". Click on the Feature tab and then check Create point (you can also create a CYS)

    After this you can attach anything you want to that point

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    scooke1-VisitorAnswer
    1-Visitor
    September 16, 2015

    The easy way.....If you have the right module create a mass properties feature (See attached image) and you can check the create point at COG option at the bottom (Mine is greyed out because we don't have that module.)

    MWSnap002 2015-09-16, 17_34_04.jpg

    The more difficult way....You could probably write some relations that take info from the mass properties parameters and use them to drive the location of your COG point.  See image below.  That means your point will stay at the COG as the model changes.  Then model a surface sphere as suggested at the point.

    MWSnap003 2015-09-16, 17_40_45.jpg

    Translate
    JamesBurcham1-VisitorAuthor
    1-Visitor
    September 16, 2015

    Looks like I don't have the correct module either, mine is greyed out as well.  That explains why I haven't been able to find an easy way to do this.

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    StephenW
    StephenW23-Emerald III
    23-Emerald III
    September 16, 2015

    I couldn't remember the exact steps so I did a quick search and found this:

    1. If you don't already have one, create a default coordinate

    system in the part.

    2. Calculate part mass properties.

    3. Create a datum point offset from the coordinate system with dimensions. Specify the coordinate system as Cartesian. Enter any arbitrary x, y, and z values.

    4. Create relations to drive the datum point's three translation

    dimensions as follows:

    $d#=mp_cg_x("","coord_sys","") X Translation

    $d#=mp_cg_y("","coord_sys","") Y Translation

    $d#=mp_cg_z("","coord_sys","") Z Translation

    The $ HAS to be in front.

    d# is the dimension number, for assemblies, this will be d#:#.

    Coord_sys is the name of the coordinate system the point is offset from(i.e., for parts: CSYS_PART_DEF, for assemblies: CSYS_ASM_DEF).

    5. Regenerate the part.

    6. Mass properties need to be recalculated after a part change,

    then the part needs to be regenerated to update the relations.

    Steps 5 and 6 need to be repeated after any change to the model

    geometry.

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      JamesBurcham1-VisitorAuthor
      1-Visitor
      September 16, 2015

      Thanks for the replies everyone, I appreciate the help.

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