Here we go! Part 5 in this series of blog posts, in which we will talk about the Part Modeler and Drafting. Mostly good news here – the Part and the Drafting scripting is very similar to V5.
For reference, here are all of the blogs in this series:
Part 1: Framework
Part 2: Creating, Opening, and Saving Files
Part 3: Services
Part 4: Product Modeler
Part 5: Part Modeling and Drafting
Part 6: Selections
Part 7: Deployment
Part Modeler
The Part, which is the 3D Shape in 3DX, object diagram is shown in Figure 1.
If you notice, the object diagram is pretty much the same as in V5. You’ve got your Bodies collection, HybridBodies collection, Sketches, Factories, and so on. Which means – once you got a hold of the Part object in 3DX, you have a good chance of using your V5 code as-is from there on. And your V5 part modeling scripting skills will very much apply.
Figure 1
Now, the question is – how do you get a hold of the Part object?
If the 3D Shape level is active, as in Figure 2, the ActiveObject property in the Editor is the Part object. So you can use the below code to access the Part.
01: Dim oPart As Part
02: Set oPart = CATIA.ActiveEditor.ActiveObject
Figure 2
However, it’s different if the 3D Part level is active, as in Figure 3 below.
Figure 3
The ActiveObject in this case is VPMRootOccurrence, and you have to get down to the VPMRepReference object, using the Product object diagram (Figure 5 in Part 4 of the series), which is where the Part object resides. The code would look something like below:
01: Dim o3DPart As VPMRootOccurrence
02: Set o3DPart = CATIA.ActiveEditor.ActiveObject ‘ get the root occurrence
03: Dim oVPMRef As VPMReference
04: Set oVPMRef = o3DPart.ReferenceRootOccurrenceOf() ‘ get its Reference
05: Dim oRepInstance As VPMRepInstance
06: Set oRepInstance = oVPMRef.RepInstances.Item(1) ‘ get the 1st Representation Instance
07: Dim oRepRef As VPMRepReference
08: Set oRepRef = oRepInstance.ReferenceInstanceOf() ‘ get the Rep Reference
09: Dim oPart As Part
10: Set oPart = oRepRef.GetItem("Part") ‘ finally, get the Part object
Drafting
Again, good news here. Drafting scripting in 3DX is very similar to V5, with just a few differences:
- Creating a new Drawing is different. See Part 2 in this series of blog posts for the how-to
- DrawingViewGenerativeBehavior object has been replaced with DrawingDefineGenView object.
- The drawing view properties are now modified using the DrawingGenService service.
The Drafting object diagram is shown in Figure 4.
Figure 4
The DrawingDefineGenView object in 3DX replaces the DrawingViewGenerativeBehavior from V5. Essentially, this is a “factory” that owns methods to create generative views from 3D:
- DefineFrontView
- DefineIsometricView
- DefineProjectionView
- DefineSectionView
- DefineStandAloneSection
- DefineAuxiliaryView
- DefineCircularDetailView
- DefinePolygonalDetailView
- DefineUnfoldedView
The DrawingDefineGenView object is owned by the DrawingViews collection, and can be retrieved using the following code:
01: Dim oDrwRoot As DrawingRoot
02: Set oDrwRoot = CATIA.ActiveEditor.ActiveObject
03: Dim cViews As DrawingViews
04: Set cViews = oDrwRoot.ActiveSheet.Views
05: Dim oGenViewFact As DrawingDefineGenView
06: Set oGenViewFact = cViews.DrawingDefineGenView
Drawing Services
There are two editor-level Drawing services in 3DX:
- DrawingGenService: Used to modify the generative view properties as well as check the integrity of the drawing links to 3D
- DrawingService: Used to work with drafting standards
For example, to change view properties such as hidden line mode, or fillet representation, in V5 you would have to use the DrawingViewGenerativeBehavior object. In 3DX, you use the DrawingGenService, like in the code below:
01: Dim oDrwGenService As DrawingGenService
02: Set oDrwGenService = CATIA.ActiveEditor.GetService("CATDrawingGenService")
03: Dim oGenViewProp As DrawingGenViewProperties
04: Set oGenViewProp = oDrwGenService.DrawingGenViewProp
05: oGenViewProp.HiddenLineMode = catHlrModeOn ' this activates the hidden line mode
06: oGenViewProp.FilletRepresentation = catFilletRepSymbolic ' this changes fillet rep
That’s all I have to say about the Part Modeling and Drafting! To summarize, probably you will have to modify your V5 code, but the tweaks should be minor and easy to implement.
We’re nearing the end of our blog series journey, only two posts remaining. In the next post, I’ll be explaining how to work with selections, and the last post will be dedicated to the deployment.
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