Trim solid with a plane using VBA

[danijel.radenkovic]

Hello to all,

I am wondering if there is a possibility to split (trim solid) using VBA.

I have found a code for surface splitting but not for solid:

Dim spFeature As SplitFeature
Set spFeature = oPrtFeats.SplitFeatures.TrimSolid(oSelectedTool, oSelectedOcc.Definition.SurfaceBodies(1),

 ),False)

 Regards

Danijel

[Jef_E · Accepted solution]

You might be surprised to know that the surfacebodies collection is a collection of solids.

You can put this to the test, create a part with multiple solids and run this rule in iLogic and it will show all the names for your solids.

Maybe the name is a bit confusing 😄

Dim oInvApp As Application
oInvApp = ThisApplication

Dim oDoc As PartDocument
oDoc = oInvApp.ActiveDocument

Dim oDef As PartComponentDefinition
oDef = oDoc.ComponentDefinition

For Each oSurfaceBody As SurfaceBody In oDef.SurfaceBodies
	MsgBox(oSurfaceBody.Name)
Next

*note that this code will only work for part documents!

[danijel.radenkovic]

Hi Jef,

I am suprised with the name "SurfaceBodies" for collection of Solid Bodies.

I have tried what you suggested and iLogic gave me the names of solids in multibody part, as you said.

So in my case, if I want to trim solid with a plane, this should looks like:

Dim oPartFeatures As PartFeatures
Set oPartFeatures = oPartDoc.ComponentDefinition.Features

Dim oSplit As SplitFeature
Set oSplit = oPartFeatures.SplitFeatures.TrimSolid(oRefPlane, oPartDef.SurfaceBodies(1), False)

Thank you, Jef!

Danijel

[danijel.radenkovic]

I have one more doubt.

Let's say that I decided to create split part using Plane1. How to edit the same split feature using Plane2?

I am not looking to delete feature and create a new one but to edit split feature.

I tried with:

Set oSplit = oPartFeatures.SplitFeatures.TrimSolid(oPlane2, oPartDef.SurfaceBodies(1), True)

But it creates new split feature so I have two of them.

Danijel

[Jef_E]

Well thats because you are adding a feature, when you refer to the existing the split you are able to edit it.

        Dim oInvApp As Application
        oInvApp = ThisApplication

        Dim oDoc As PartDocument
        oDoc = oInvApp.ActiveDocument

        Dim oDef As PartComponentDefinition
        oDef = oDoc.ComponentDefinition

        Dim oSplitFeature As SplitFeature
        oSplitFeature = oDef.Features.SplitFeatures.Item(1)

        oSplitFeature.SetToTrimSolid(oDef.WorkPlanes.Item(2), oDef.SurfaceBodies.Item(1), True)

Sorry for the late response, I intended to reply yesterday but apparently I did not hit sent.

[danijel.radenkovic]

There is something wrong with the last line of the code:

oSplitFeature.SetToTrimSolid(oDef.WorkPlanes.Item(2), oDef.SurfaceBodies.Item(1), True)

Also, would you like to explain me why sometimes I must to add "Set" to define some feature cause it says as on the image bellow , but sometimes works without adding "set"?

Regards

Danijel

[danijel.radenkovic]

---

@danijel.radenkovic wrote:

There is something wrong with the last line of the code:

oSplitFeature.SetToTrimSolid(oDef.WorkPlanes.Item(2), oDef.SurfaceBodies.Item(1), True)

Also, would you like to explain me why sometimes I must to add "Set" to define some feature cause it says as on the image bellow , but sometimes works without adding "set"?

Regards

Danijel

---

Solved. I forgot to call update of the feature.

Call oSplitFeature.SetToTrimSolid(oDef.WorkPlanes.Item(2), oDef.SurfaceBodies.Item(1), True)

Regards

Danijel