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Unable to place center of gravity point

Amethyst

Unable to place center of gravity point

What I need is a centroid point to a closed area in a sketch.  It doesn't appear this is possibly directly.

If you build a solid feature off of the sketch you can visualize the center of gravity through choosing X section Mass Properties.

COG.JPG

Unfortunately I can't appear to save the result.

If I go the Feature tab the option to save the result is not available (it is greyed out).

COG NO.JPG

Would anyone have an idea of how to get this to work properly?

9 REPLIES 9

Re: Unable to place center of gravity point

To use analysis features, you need an "advanced" license (can't remember the names right off hand). Then you can create a feature.  COG coordinate system

There is another method that takes just a little more work.  Center of Gravity in Drawings


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: Unable to place center of gravity point

If you click on the "i" button you will get something that you can save.  However, you can leave that window open to cut and past the numbers into your Point - Offset Coordinate System.


Creo is an endless adventure: Always more to learn.

Re: Unable to place center of gravity point

As Stephen alluded to up above to be able to actually drop points from the analysis you have to have the BMX license.

This seems insane that you have to use this crazy work around to actually place a centroid point in a sketch.  Oh, and by the way you need to purchase an otherwise un-needed software add on to do the crazy work around.

There is absolutely no reason this shouldn't be in the product's base functionality.

Re: Unable to place center of gravity point

By any chance would there be a way to get a centroid point in a sketch by using relations or even a UDF?

Re: Unable to place center of gravity point

Hi Paul,

to obtain a point automatically placed at COG you have to create an offset datum point starting from the default coordinate system and then add theese simple strings to the relations:

$d1 = mp_cg_x("","DEF_CSYS","")

$d2 = mp_cg_y("","DEF_CSYS","")

$d3 = mp_cg_z("","DEF_CSYS","")

where d1, d2 and d3 are the names for the point offset dimensions and DEF_CSYS is the name of the default coordinate system.

Note: you need some geometry and mass property to validate the relations.

Video Link : 6953

Ciao Gabriele

Re: Unable to place center of gravity point

Hi, It's not so difficult to generate the COG. Create a new Csys from the part or Assembly origin Csys in the X value you simply type pro_mp_cogx in the Y you put in the value pro_mp_cogy and in the Z you type in pro_mp_cogz. These come from your reported mass properties in Tools/Parameters.

CaptureCOG.PNG

Re: Unable to place center of gravity point

Hello

This question is posed for decades (I started with the)

version Proe 13) and there is still not a direct function to ask a

Center of gravity directly.

Kind regards.

Denis.

Re: Unable to place center of gravity point

Thanks Roy and Gabriele for your ideas.

I would like to test these out.  I will confess that this is a little confusing to me.

In Roy's example he appears to be able to place a COG offset datum on the fly (more or less).  He uses the mass property values and applies the X, Y and Z values to the offset datum that was built.

I have not really used relation values in Creo yet, however what Gabrielle shows makes me wonder whether you could use the relation table within a sketch and apply the COG to the enclosed area in a sketch instead of building an extrude to establish the COG? Is this possible or does the mass properties have to be applied to geometry outside of a sketch?

Highlighted

Re: Unable to place center of gravity point

Hello Paul,

to my knowledge Creo can not find the centroid of plane areas.

What i have done is to create a template (part or assembly) where the COG relations (created similar to previous replies in this thread) are present from the beginning. By doing this d2 is always X, d3 is always Y and d5 is always Z.

After i have created all the features in the part or assembled all the parts in my assembly i drag the group (COG_DATUM) to the end and regenerate. Then a CSYS and a Point will be created at COG with CSYS_DEF as the reference. Then in drawings i can attach the COG symbol to the point and lock it to the view.

Best Regards

COG1.jpg COG Group ShownCOG2.jpgFeature created

COG3.jpg Analysis -> Mass Properties is shown

COG4.jpg COG Group is moved down and regenerated. Dimensions are shown and can be compared to Mass Properties.