Macro to create hole feature at center of selected face

Anonymous · ‎06-21-2017

Hi All,

I am looking for a macro, to create hole feature of 0.5" Diameter at the center of selected faces.

When I run the macro, it should ask for "SELECT FACE" once I select the face/faces, hole of 0.5" Diameter to be created at the center of selected face and should ask for "NEXT FACE" to repeat same operation and "DONE" for terminating the operation.

Please let me know if a code can be written for above mentioned case. Kindly need help from our community's experts on this.

Attached image for your reference.

Thank you..

Regards,

Harish

Mark.Lancaster · ‎06-21-2017

@Anonymous

Are you looking to automate your steps or can you use this workflow by creating a work point that centers based on a loop of edges?

Then use that point as your starting point for that hole. If the size of the face changes, the point automatically rec-enters.

Mark Lancaster

& Autodesk Services MarketPlace Provider

Autodesk Inventor Certified Professional & not an Autodesk Employee

Likes is much appreciated if the information I have shared is helpful to you and/or others

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.

Curtis_Waguespack · ‎06-21-2017

Hi hmanoharBYAYC,

Here's a quick iLogic macro to do this. Attached is a 2017 example file as well.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com


Dim oSheetMetalDoc As PartDocument
oSheetMetalDoc = ThisApplication.ActiveEditDocument

' a reference to the component definition.
Dim oCompDef As SheetMetalComponentDefinition
oCompDef = oSheetMetalDoc.ComponentDefinition

' a reference to the sheet metal features collection.
Dim oSheetMetalFeatures As SheetMetalFeatures
oSheetMetalFeatures = oCompDef.Features

Dim oFace As Face

'Keep Selecting Faces, Hit Esc to finish
Do
    oFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllPlanarEntities, "Select a face")
    If Not oFace Is Nothing Then 
        Exit Do
    End If
Loop While Not oFace Is Nothing

' Get the outer loop of the face.
Dim outerLoop As EdgeLoop
For Each outerLoop In oFace.EdgeLoops
    If outerLoop.IsOuterEdgeLoop Then
        Exit For
    End If
Next

' Create a workpoint at the edge mid-point
Dim oWorkPoint As WorkPoint
oWorkPoint = oCompDef.WorkPoints.AddAtCentroid(outerLoop)

Dim oPointPlacement As PointHolePlacementDefinition 
oPointPlacement = oCompDef.Features.HoleFeatures.CreatePointPlacementDefinition(oWorkPoint,oFace)

' Create the hole feature, 0.5 cm dia
Call oCompDef.Features.HoleFeatures.AddDrilledByThroughAllExtent( _
                        oPointPlacement, 0.5, kPositiveExtentDirection)
'turn off workpoint
oWorkPoint.Visible = False

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Curtis_Waguespack · ‎06-21-2017

@Anonymous wrote:

... and should ask for "NEXT FACE" to repeat same operation and "DONE" for terminating the operation.

Hi hmanoharBYAYC,

This version repeats as per your request.

Also just as a tip, you can search and ask programming questions of this type on the Inventor Customization forum too:
http://forums.autodesk.com/t5/Autodesk-Inventor-Customization/bd-p/120

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Dim oSheetMetalDoc As PartDocument
oSheetMetalDoc = ThisApplication.ActiveEditDocument

' a reference to the component definition.
Dim oCompDef As SheetMetalComponentDefinition
oCompDef = oSheetMetalDoc.ComponentDefinition

' a reference to the sheet metal features collection.
Dim oSheetMetalFeatures As SheetMetalFeatures
oSheetMetalFeatures = oCompDef.Features

Dim oFace As Face

'Keep Selecting Faces, Hit Esc to finish
Do
    oFace = ThisApplication.CommandManager.Pick _
	(SelectionFilterEnum.kAllPlanarEntities, _
	"Select a face, press Esc to finish")
    If Not oFace Is Nothing Then 
		' Get the outer loop of the face.
		Dim outerLoop As EdgeLoop
		For Each outerLoop In oFace.EdgeLoops
			If outerLoop.IsOuterEdgeLoop Then
				Exit For
			End If
		Next
		
		' Create a workpoint at the edge mid-point
		Dim oWorkPoint As WorkPoint
		oWorkPoint = oCompDef.WorkPoints.AddAtCentroid(outerLoop)
		
		Dim oPointPlacement As PointHolePlacementDefinition 
		oPointPlacement = oCompDef.Features.HoleFeatures. _
		CreatePointPlacementDefinition (oWorkPoint,oFace)
		
		' Create the hole feature, 0.5 cm dia
		Call oCompDef.Features.HoleFeatures. _
		AddDrilledByThroughAllExtent( _
		oPointPlacement, 0.5 * 2.54, kPositiveExtentDirection)
		'turn off workpoint
		oWorkPoint.Visible = False
    End If
Loop While Not oFace Is Nothing

Anonymous · ‎06-22-2017

Hello Sir,

Thank you so much for your response and the ilogic code provided.

Unfortunately the above ilogic code is not working at my end, its showing error:

------------------------------------------------------------------------------------------------------------

Error in rule: Rule0, in document: Part3.ipt

Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))

------------------------------------------------------------------------------------------------------------

Also i am not able to use the example part file provided, since i am using Inventor-2016 version.

Request you to send me a part file in 2016 version to see the ilogic fulfills my requirement.

As i went through the ilogic code, where i noticed that the center for hole is created by "Work Point". I am looking for an option, where the ilogic should enter into the sketch mode and insert "Point, Center Point" at the center of selected face.

Please help me on this..

Thank you,

Regards,

Harish

Anonymous · ‎06-22-2017

Hello Sir,

Thank you so much for your response.

I am looking for an ilogic and my requirement posted on Mr Curtis post.

Please let me know if you have nay solution.

Thank you Again,

Regards

Harish

S_May · ‎06-22-2017

Hi @Anonymous,

I could also make them an ifeature with which you can create the lick and the hole at once (example in the screencast).

If they work a lot with sheet metal there are 100 Solutions.

MFG

Sascha May

EXPERT ELITE

Anonymous · ‎06-23-2017

Hi Sascha May,

Thank you so much for your response and screencast provided.

The Screecast provided helped me to think in different way to improve my work process.

Problem is, right now we are not suppose to use ifeatures in our project, since these part designs are used globally and we need to set standards to use ifeature, which may happen in later stages.

Please let me know if you know any other method than this, where center point for hole should be sketch based.

Thanks a lot...

Regards,

Harish Kumar M

Curtis_Waguespack · ‎06-23-2017

Hi hmanoharBYAYC,

I looked at the example I provided in Inventor 2015 and I do see the Unspecified Error in that version. The error seems to be related to creating the workpoint, which you have updated this post to say that you do not want that result.

I think the method for hole placement from linear edges would be the method to use, but unfortunately I do not have the time today to look at this further. Below is that sample in case it helps you or someone else interested in this.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Hole feature linear placement API Sample

https://knowledge.autodesk.com/search-result/caas/CloudHelp/cloudhelp/2018/ENU/Inventor-API/files/Ho...

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Macro to create hole feature at center of selected face