Center of gravity of a body

[elihuisland]

I believe that some center of gravity calculations are in error.  For example, when I want to place a joint origin on the face of an extruded disc, the center of gravity is correctly shown at the disc center.  Similarly, if I draw a circle with one side sliced off, then extrude a D-profile shaft, the face center of gravity is correctly shown offset from the disc center. 

However, suppose I draw the same disc.  Then I draw a smaller offset disc inside.  I extrude the larger disc, with a resulting off-center hole in it.  The C.G of the body should clearly be offset as well.  ( i.e, a disc with a hole drilled off center is no longer balanced)  But when I go to place a joint origin on the disc face, the C.G. is shown at the disc center!  Something wrong here!

[Mike.Grau]

Hi @elihuisland,

Thanks for raising our attention to this.

It sounds a bit tricky to exactly reproduce what you are describing.

Could you may share a Screencast with us? That would be great.

Thanks,

[elihuisland]

Thanks, Mike.  At your suggestion I posted a screencast with the link below.  (It's my first).  In it I tried to illustrate the point that the C.G on the face of a disc should move off center when asymmetric cuts are made to the disc.  The illustration shows attempting to attach joint origins to C.G.s on the faces of 3 examples.  A plain disc, or a disc with a slice taken off seem to act appropriately, with the C.G moving off center to compensate for the missing mass from the slice.  However, removing mass off center by cutting a hole in the disc does not displace the C.G from the center of the disc face.  It seems that it should.  Thanks for your consideration.

[Mike.Grau]

Hi @elihuisland,

Thank you so much for sharing the screencast with us.

Currently, we do not display the properties of sketches like the COG of a circle with features.

I think this might be a great point for our IDEA station with the link here. http://forums.autodesk.com/t5/ideastation-request-a-feature-or/idb-p/125

You would look for a feature which allows you to select certain sketch entities and compute the COG of these.

But we do have this feature for components and bodies. If you right-click on a body and select "Properties",

you will see the "Properties" window with the "Center of Mass" which is the COG.

By having a closer look at the shown values those look correct but measuring those who show up once you assign the "Joint Origin" it becomes confusing,

I will get in touch with our Development Team and investigate further into this.

We´ll keep you updated about that.

Thanks,

[elihuisland]

Thanks, Mike.  I appreciate your investigation.  Per your note, I later converted the bodies in the Screencast above into components, with the same results I reported.  Also per your note, I did an experiment:  Draw a semicircle of radius 1" centered at the origin.  Extrude a 1" body, convert to a component, so we have a half-circular disc.  Examine the Properties (I pasted the results below).  "Properties" correctly lists the center of mass at y= 0.424 .

Here's a link to the file:  http://a360.co/2dqSSLV

You get the same result, y= 0.424,  with a manual calculation from a table of C.G. properties.   However, if you use "measure" , the small square that appears on the face of the component is at y = 0.500.  According to the Fusion 360 tutorials, the small square is supposed to indicate the face centroid.  That should also be the y-axis center of mass in this example, but is not.  I earlier used inserting joint origins as a way to get the square indicator to appear, but "measure" also does the same.  I still think there is a bug. 

Semicircle 1
Area 8.283 in^2
Density 4.624 ouncemass / in^3
Mass 7.264 ouncemass
Volume 1.571 in^3
Physical Material Stainless Steel AISI 304

Bounding Box
Length 1.00 in
Width 1.00 in
Height 2.00 in
World X,Y,Z 0 in, 0 in, 0 in
Center of Mass 0.5 in, 0.424413 in, 0 in

Moment of Inertia at Center of Mass (ouncemass in^2)
Ixx = 2.324
Ixy = 0.00
Ixz = 0.00
Iyx = 0.00
Iyy = 2.421
Iyz = 0.00
Izx = 0.00
Izy = 0.00
Izz = 1.113

Moment of Inertia at Origin (ouncemass in^2)
Ixx = 3.632
Ixy = -1.541
Ixz = 0.00
Iyx = -1.541
Iyy = 4.237
Iyz = 0.00
Izx = 0.00
Izy = 0.00
Izz = 4.237

[jeff_strater]

Hi @elihuisland,

I think that there are a couple of different concepts being described here.  There is the "mass properties" of a design/component, which does correctly show the correct center of mass:

And the second concept is the joint command, and the "snap points" that are created in the command to give you convenient places to attach the joint:

The Joint Snap Points are not intended to indicate center of mass of the selected face.  They are just intended to show some convenient places to attach a joint, including one "near the middle" of the selected face.   

There is a project in our backlog to put a work point at a body center of mass, which could then be used for a joint, but understand that in the above case, the CG will be inside the middle of the component, not on the surface.

Hope this helps clear up some of the confusion.

Jeff

[elihuisland]

Jeff,

Thanks for your very prompt reply!  The Fusion 360 instructional materials, "Choose the Appropriate Joint Locations"  says "Vertices appears as dots, mid-points appear as triangles, the centers of circles and arcs appear as plus signs and the centroid of a body appears as a square." (my emphasis) (http://fusion360.autodesk.com/learning/learning.html?guid=GUID-2C7DE501-13D6-416A-A203-F070D11FA889 )

A centroid is the center of gravity of a two dimensional figure.  For extruded components, the centroid of a face should have the same projected coordinates as the center of gravity of the solid below it.  (i.e, if the component is extruded along the z-axis, the x and y coordinates of the centroid on the extrusion face should be the same as the C.G.)

If the little square that appears is not a centroid, please let the instructional materials reflect that.  It's otherwise misleading, especially if a design relies on a part being balanced.

Thanks again, I'm loving your program and point this stuff out to be helpful!

Best,

Carl (elihuisland)

[eschermuppet]

Hmmm, From reading this, I'm guessing that using the center of gravity in a body as a constraint for center of a hole in it would be right out, then.  

I'm a total noob here, but came from google search looking to see if it's possible to set up a constraint on either the centroid of a sketch of a closed spline or the CoG of the resulting extruded body as the center of a fixed diameter circle that would move around as changes are made to the underlying sketch or to the body itself  (ex: by punching random holes or redistributing weight, cutting fillets an chamfers, scaling etc.)

Right clicking the body to look at its properties, saving them to notepad, then downloading some code from GitHub that will enable me to create a point at that coordinate, then iterating as I make changes to my model is about the worst workflow I could possibly dream up.

[MichaelAubry]

I'm a total noob here, but came from google search looking to see if it's possible to set up a constraint on either the centroid of a sketch of a closed spline or the CoG of the resulting extruded body as the center of a fixed diameter circle that would move around as changes are made to the underlying sketch or to the body itself  (ex: by punching random holes or redistributing weight, cutting fillets an chamfers, scaling etc.)

Here's the script I made (w/ generous help from our API team and my intern) to create a reference COM point in Fusion:

The link is just the simple script code: https://twitter.com/michael_aubry/status/748198788532166657

The .zip attachment is a bit more comprehensive as will install an icon in the fusion window:

Just rerun the script to update.  I'm not sure you'll be able to setup reliable references to that point but it's for sure worth a look. Excited to see what you come up with!

Mike

[eschermuppet]

Thanks, will take a look!

[andy.c]

Hello,

I have tried to use this add-in and I get this error message:

Failed:

Traceback (most recent call last):

File "C:/Users/andyc/AppData/Roaming/Autodesk/Autodesk Fusion 360/API/AddIns/CenterOfMassPoint/CenterOfMassPoint.py", line 73, in notify

baseFeature = rootComp.features.itemByName('Center of Gravities')

^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^

File "C:\Users/andyc/AppData/Local/Autodesk/webdeploy/production/b0c303e70bd97cfdc195adab65922cfeffcb363a/Api/Python/packages\adsk\fusion.py", line 21644, in itemByName

return _fusion.Features_itemByName(self, name)

^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^

RuntimeError: 2 : InternalValidationError : fragment

Any chance you can look into this? Thank you.