topic Re: Counting Blocks On A Sketch in Inventor Forum

Counting Blocks On A Sketch

Anonymous — Thu, 04 Apr 2019 06:01:33 GMT

Dear Friends,

I have a sketch for a building facade which uses different aluminium profiles.

Each profile (in blocks) has the same length through out the building.

Is there a way to count how many blocks on a sketch?

The goal now is to make material take-off and I do not have enough time to create them in all in 3d.

Thank you.

Re: Counting Blocks On A Sketch

3D4Play — Thu, 04 Apr 2019 06:43:53 GMT

Those blocks are in a sketch, so logically each block can be in its own sketch, then each sketch is (presumably) automatically in its own part, which you can then place into an assembly, just like you did with the sketch blocks in the sketch. You can then generate a BOM based on the number of "parts" even though they are really just sketches. If that doesn't work, then one can probably still use 2D AutoCAD for 2D sketch work, and to query the block. Inventor is for 3D and probably not the right tool for you if you want to generate things in 2D. Inventor doesn't query sketch geometry, but it does a decent job of generating a BOM, quickly. In summary: Create parts per sketch. Place the parts into an assembly, then generate a BOM. Hope that helps.

Re: Counting Blocks On A Sketch

Xun.Zhang — Thu, 04 Apr 2019 06:58:07 GMT

Hello @Anonymous,

You can easily get the sketch block count in a specific sketch via API.

Go to Tools -> VBA Editor, add below code in and fill in the name of the sketch node and then press Run icon to get the count number.

Sub SketchBlocks()
   Dim oDoc As PartDocument
   Set oDoc = ThisApplication.ActiveDocument

   Dim oCompDef As PartComponentDefinition
   Set oCompDef = oDoc.ComponentDefinition

   Dim oSketch As PlanarSketch
   Set oSketch = oCompDef.Sketches.Sketch1

   Debug.Print oSketch.SketchBlocks.Count

End Sub

Hope it helps!

Re: Counting Blocks On A Sketch

Anonymous — Thu, 04 Apr 2019 08:19:13 GMT

Sorry @Xun.Zhang and @3D4Play . I made a mistake, the question is actually "Is there a way to count how many blocks on a part? I have to know the quantity of each blocks for the whole (multi-body) part.

This is quit challenging model that Im trying to do.

Please see the snapshot below.

Im just started to learn api so the code that you gave me, I learned from it.

Thank you very much for your time.

Re: Counting Blocks On A Sketch

Sergio.D.Suárez — Thu, 04 Apr 2019 12:10:02 GMT

Hello, try with this ilogic rule, it will count all the blocks that you have in the part document and it will show you the total amount of each block

Dim oDoc As PartDocument = ThisApplication.ActiveDocument
Dim oCompDef As PartComponentDefinition
oCompDef = oDoc.ComponentDefinition

For Each oSketchBlockdef In oCompDef.SketchBlockDefinitions 
	Dim i As Integer =0
	For Each oSketch As PlanarSketch In oCompDef.Sketches
		For Each oSketchBlock1 As SketchBlock In oSketch.SketchBlocks
			Dim oSketchBlock1name As String
			oSketchBlock1name = Left(oSketchBlock1.Name, (InStrRev(oSketchBlock1.Name, ":", -1, vbTextCompare) - 1))
		    If oSketchBlockdef.name = oSketchBlock1name Then i=i+1
		Next
	Next
MessageBox.Show(oSketchBlockdef.name & " - Qty - " &  i)
Next

I hope it's useful