Define Assembly Axis coincident with Center Of Mass

[Rob]

I'm looking to create a pivot point at exactly the Assembly COM.

So far I have achieved this by creating a COM feature in the assembly and then creating an assembly sketch with a single sketch point that I drag coincident to the COM point then using this point and a Plane to define the Axis.

This works but the sketch point does not update when the COM moves.

To get an update I have to delete the sketch point coincident relation and reapply it, which is insanely tedious.

Is there a nicer way to do this? Seems like there should be.

[mattpeneguy]

I'm looking to create a pivot point at exactly the Assembly COM.

So far I have achieved this by creating a COM feature in the assembly and then creating an assembly sketch with a single sketch point that I drag coincident to the COM point then using this point and a Plane to define the Axis.

This works but the sketch point does not update when the COM moves.

To get an update I have to delete the sketch point coincident relation and reapply it, which is insanely tedious.

Is there a nicer way to do this? Seems like there should be.

I just put a center of mass in an assembly yesterday. I hardly ever use it, but what you are asking should work.
Just tried selecting the COM and a sketch point and yep, I can't make a relation. I get it this may be intentional, as I can see some horrible circular reference scenarios, but when's that ever stopped SW? SW's motto should be "always giving the users enough rope to hang themselves".
Hey @gupta9665, it appears the COM is accessible in the API, but I'm guessing it won't update and any macro you made assigning the axis to the COM via macro would require re-running the macro? Maybe this could be handled by a Macro feature that would update with each rebuild?
http://help.solidworks.com/2012/English ... ple_vb.htm

[Glenn Schroeder]

I just put a center of mass in an assembly yesterday. I hardly ever use it, but what you are asking should work.
Just tried selecting the COM and a sketch point and yep, I can't make a relation. I get it this may be intentional, as I can see some horrible circular reference scenarios, but when's that ever stopped SW? SW's motto should be "always giving the users enough rope to hang themselves".
Hey @gupta9665, it appears the COM is accessible in the API, but I'm guessing it won't update and any macro you made assigning the axis to the COM via macro would require re-running the macro? Maybe this could be handled by a Macro feature that would update with each rebuild?
http://help.solidworks.com/2012/English ... ple_vb.htm

I tried it. It wouldn't let me apply a relation by Ctrl+ selecting the sketch point (or end point of a line) and the CoM, but it would let me drag it to the CoM and apply a relation that way. I moved a component, which of course caused the CoM to move. The sketch point did not move with it, even after a Ctrl+Q rebuild. I opened the sketch, and it showed the Coincident relation, but it still didn't update.

[Rob]

I just put a center of mass in an assembly yesterday. I hardly ever use it, but what you are asking should work.
Just tried selecting the COM and a sketch point and yep, I can't make a relation. I get it this may be intentional, as I can see some horrible circular reference scenarios, but when's that ever stopped SW? SW's motto should be "always giving the users enough rope to hang themselves".
Hey @gupta9665, it appears the COM is accessible in the API, but I'm guessing it won't update and any macro you made assigning the axis to the COM via macro would require re-running the macro? Maybe this could be handled by a Macro feature that would update with each rebuild?
http://help.solidworks.com/2012/English ... ple_vb.htm

Thanks Matt

I was hunting the correct API calls unsuccessfully but you showed me the way..

I ended up creating two planes to define the axis and then update the plane offsets based on the current COM.

It's a hack for sure but its working..

Code: Select all

Option Explicit

Dim swApp As SldWorks.SldWorks

Sub main()

    Set swApp = Application.SldWorks
    
    Dim swModel As SldWorks.ModelDoc2
    Set swModel = swApp.ActiveDoc
    
    Dim swMassProperty As SldWorks.MassProperty
    Set swMassProperty = swModel.Extension.CreateMassProperty
    
    Dim vComPts As Variant
    vComPts = swMassProperty.CenterOfMass
    
    Debug.Print vComPts(0), vComPts(1), vComPts(2)
    
    Dim swDimension As SldWorks.Dimension
    
    Set swDimension = swModel.Parameter("D1@COMPlaneXZ")
    
    swDimension.SystemValue = Abs(vComPts(1))
    
    Set swDimension = swModel.Parameter("D1@COMPlaneYZ")
    
    swDimension.SystemValue = Abs(vComPts(0))
    
    swModel.EditRebuild3

End Sub

[edit] I added the macro to the design binder so it's pretty convenient now

image.png (4.91 KiB) Viewed 2837 times

[GrahamK]

I could be clever and say Catia as this will do exactly what you want

What you can try is:

Create COM
Then create 3 global variables which you can assign the values in XYZ of COM (make sure you set to automatically rebuild)
Create 3 planes paralel to Front, top, Right and link to the 3 global variables.
Create point of intersection of these 3 planes.

If the COM changes this will update the global variables which in turn updates the planes and then the point.

[SPerman]

It's a hack for sure but its working..

That should be SW motto.

[Rob]

I could be clever and say Catia as this will do exactly what you want

What you can try is:

Create COM
Then create 3 global variables which you can assign the values in XYZ of COM (make sure you set to automatically rebuild)
Create 3 planes paralel to Front, top, Right and link to the 3 global variables.
Create point of intersection of these 3 planes.

If the COM changes this will update the global variables which in turn updates the planes and then the point.

Perfect Graham!!

This is basically what my macro did but via equations!
SW warns about a potential circular ref, but that's fair enough

[colt]

Another way is to create massless part that you can mate to the cg. Then you can mate to that object. It seems to follow the cg accurately on rebuild.

[DanPihlaja]

I could be clever and say Catia as this will do exactly what you want

What you can try is:

Create COM
Then create 3 global variables which you can assign the values in XYZ of COM (make sure you set to automatically rebuild)
Create 3 planes paralel to Front, top, Right and link to the 3 global variables.
Create point of intersection of these 3 planes.

If the COM changes this will update the global variables which in turn updates the planes and then the point.

That is a great idea.

The only issue that I see is when/if one of the distances goes into the negative or becomes 0. How do you determine positive/negative direction?

[Rob]

That is a great idea.

The only issue that I see is when/if one of the distances goes into the negative or becomes 0. How do you determine positive/negative direction?

I had the same concern, so I mated so that the assembly origin was at an extreme corner

[Rob]

Another way is to create massless part that you can mate to the cg. Then you can mate to that object. It seems to follow the cg accurately on rebuild.

Capture.PNG

Up there for thinking, down there for dancing!

[Alin]

I'm looking to create a pivot point at exactly the Assembly COM.

So far I have achieved this by creating a COM feature in the assembly and then creating an assembly sketch with a single sketch point that I drag coincident to the COM point then using this point and a Plane to define the Axis.

This works but the sketch point does not update when the COM moves.

To get an update I have to delete the sketch point coincident relation and reapply it, which is insanely tedious.

Is there a nicer way to do this? Seems like there should be.

In SW2022, you just need to define the Coordinate System. Its origin, planes and axes are now selectable and usable for many downstream operations (including sketching, mates and more).

[mattpeneguy]

In SW2022, you just need to define the Coordinate System. Its origin, planes and axes are now selectable and usable for many downstream operations (including sketching, mates and more).

Hmm. That works and should be a robust solution!

BTW, who championed adding those planes and axes to the coordinate systems? I'd like to thank them. I'd be testing this out in the Beta if we weren't stuck on Windows 7 (can't upgrade past 2020).

[Alin]

Hmm. That works and should be a robust solution!

Yes, the new functionality is pretty crazy. We can even achieve freedom from the ORIGIN!!!
I stress-test the enhancements and reported the results here:

https://www.engineersrule.com/coordinat ... -and-axes/

[Alin]

BTW, who championed adding those planes and axes to the coordinate systems? I'd like to thank them.

I asked the same question here:
https://r1132100503382-eu1-3dswym.3dexp ... NJjqu20FVg

[DanPihlaja]

Hmm. That works and should be a robust solution!

BTW, who championed adding those planes and axes to the coordinate systems? I'd like to thank them. I'd be testing this out in the Beta if we weren't stuck on Windows 7 (can't upgrade past 2020).

Its been in the top ten every single time I have ever participated in it.

[KevinC]

Another way is to create massless part that you can mate to the cg. Then you can mate to that object. It seems to follow the cg accurately on rebuild.

Capture.PNG

Along the lines of colt's post, if you use a surface instead of a solid body, then you needn't worry about any effects the CG ball has on the CG calcs as it is massless and its material selection is..immaterial.

EDIT:
And apply the black/while tile texture to the surface ball to give it a CG look: