Recording a Section View Going Through an Assembly

 

I discovered today that the section view cutting plane is no longer tied to the face or plane selected at the time of placement. That and there is no parameter created when typing in an offset.

Go back a few releases and you could place a half section view on an origin plane and then, using constraints, drive the cutting plane through the assembly. This could then be recorded, from the Drive Constraint dialog, creating a sweet animated section plane eating through the assembly. However the section plane now stays in place "relative to the sectioned parts" as things are moved around.. Today I was asked how to achieve this again. These section views do not transfer into the Inventor Studio environment so what to do?

I decided to use iLogic to drive an assembly extrusion and it ended up working pretty well. Make sure to first extrude through every part so they are all included in the assembly feature.

Then name a parameter that can later be referenced in an iLogic rule.

For the single part we used 3^rd part software and simply recorded the screen. However while creating this article, my 300+ part Lego assembly was talking nearly two minutes between cuts. That doesn't make for the smoothest of videos. I decided to have the While loop export a screen grab and then used Windows Movie Maker to string them all into a movie. http://windows.microsoft.com/en-US/Windows-Live/movie-maker#t1=overview

If you plan on doing multiple cuts through your assembly remember to save a View Rep first! If you crash or happen to rotate or pan the view will be different between the animations.

iLogic Code Used

Parameter("CutDepth")	=	0

oCount = 1000

'save iso view To jpg

oCount = oCount + 1

imagedoc = ThisDoc.PathAndFileName(False) & oCount & ".jpg"

oCamera = InventorVb.Application.ActiveView.Camera 'current iso view

'oCamera.fit

oCamera.apply

InventorVb.Application.ActiveView.SaveAsBitmap(imagedoc,1680,1050 )

While   Parameter("CutDepth") < 150

        Parameter("CutDepth") = Parameter("CutDepth") + .50

        InventorVb.DocumentUpdate()

        iLogicVb.UpdateWhenDone = True

        'save iso view to jpg

        oCount = oCount + 1

        imagedoc = ThisDoc.PathAndFileName(False) & oCount & ".jpg"

        oCamera = InventorVb.Application.ActiveView.Camera 'current iso view

        'oCamera.fit

        oCamera.apply

        InventorVb.Application.ActiveView.SaveAsBitmap(imagedoc,1680,1050 )

End While

I had a lot of fun creating this animation and I hope to see some of yours as well. Feel free to post a link to your own YouTube section cut video.