CAD Forum

Rob wrote: ↑Thu Oct 28, 2021 8:07 am 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 wrote: ↑Thu Oct 28, 2021 8:29 am 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

mattpeneguy wrote: ↑Thu Oct 28, 2021 8:29 am 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

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

Rob wrote: ↑Thu Oct 28, 2021 9:28 am
It's a hack for sure but its working..

GrahamK wrote: ↑Thu Oct 28, 2021 10:02 am 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.

GrahamK wrote: ↑Thu Oct 28, 2021 10:02 am 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.

dpihlaja wrote: ↑Thu Oct 28, 2021 10:55 am 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?

colt wrote: ↑Thu Oct 28, 2021 10:54 am 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

Rob wrote: ↑Thu Oct 28, 2021 8:07 am 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.

Alin wrote: ↑Thu Oct 28, 2021 4:45 pm 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 wrote: ↑Thu Oct 28, 2021 5:24 pm Hmm. That works and should be a robust solution!

mattpeneguy wrote: ↑Thu Oct 28, 2021 5:24 pm BTW, who championed adding those planes and axes to the coordinate systems? I'd like to thank them.

mattpeneguy wrote: ↑Thu Oct 28, 2021 5:24 pm 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).

colt wrote: ↑Thu Oct 28, 2021 10:54 am 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