Can't find a way to chamfe/radius a face

[ToddPig]

I would like to select a face, either a flat surface, or a cylinder, and have a chamfer/radius placed at every edge of this surface.

[Curtis_Waguespack]

Hi ToddPig,

For a radius have a look at the Rule Fillet tool. Nothing is coming to mind for chamfers though.

You might need to enable the Plastic Part panel to find it.

On the ribbon, click 3D Model tab  >  Show Panel icon . Select Plastic Part panel to display the Plastic Part panel, and then select Rule Fillet

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016...

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

[ToddPig]

That's a good trick. Thanks. Do you have one for chamfer?

[Cadmanto]

Todd,

There is a way to select faces, but not the way you are describing.  In the fillet command you can pick one face and then an adjacent one, but that is cumbersome.  You can also select a feature and it will radius all edges that way, but not a face as you describe.  This looks to be a good candidate for the Inventor IdeaStation

If this solved your issue please mark this posting "Accept as Solution".

Or i you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[JDMather]

A face is bounded by a Loop, so if you set the selection to Loop and click the edge of face at loop.

[ToddPig]

Awesome, thanks JD.

Any ideas for applying a chamfer in the same manner.

For example, I have holes thru a part, and would like to select the cylindrical surface, and have the same chamfer applied to each side of the hole.

[Curtis_Waguespack]

---

@ToddPig wrote:
That's a good trick. Thanks. Do you have one for chamfer?

---

Hi ToddPig,

I have a trick to do that, but it's customization. I don't know of a way to do it otherwise.

Maybe it would be a good Idea Forum post:
http://forums.autodesk.com/t5/Inventor-IdeaStation/idb-p/v1232

This iLogic creates a chamfer on already chamfered edges, which is shouldn't do, but I didn't bother trying to filter those out.

Use at your risk!

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

oSize = InputBox("Enter a size for the chamfer", "iLogic", "")
If oSize = "" Then
Return
End If

oDoc = ThisDoc.Document

' Set a reference to the component definition.
Dim oCompDef As PartComponentDefinition
oCompDef = oDoc.ComponentDefinition

Dim oFace As face
' define the edge collection.
oEdgeCollection = ThisApplication.TransientObjects.CreateEdgeCollection

'Keep Selecting Faces, Hit Esc to finish
Do
	oFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Select Face (Press ESC to exit)")
	If Not oFace Is Nothing Then
	
		' Add all of the edges of the face to the edge collection.
		For Each oEdge In oFace.Edges
			oEdgeCollection.Add (oEdge)
		Next
		
		Dim oChamfer As ChamferFeature
		Try
		oChamfer = oCompDef.Features.ChamferFeatures.AddUsingDistance(oEdgeCollection, oSize)
		Catch
			MessageBox.Show("Chamfer could not be created.", "iLogic")
		End Try
		
	End If
Loop While Not oFace Is Nothing

[mcgyvr]

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@ToddPig wrote:


Any ideas for applying a chamfer in the same manner.

---

Just another thing..

If the edges are tangent then if you have the "All tangentially connected edges" (expand the >> for that option in the chamfer dialog) selected and the shape applies then it will select the loop

And yes.. If you select "Distance/Angle" you can select whole faces too..

[ToddPig]

very cool. might be more work than selecting all the edges, but still impressive.

[ToddPig]

The "Distance/Angle" does not really work, it only chamfers a single edge.

[mcgyvr]

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@ToddPig wrote:
The "Distance/Angle" does not really work, it only chamfers a single edge.

---

Oh yeah.. Sorry about that.. It worked for me because I had that "tangentially" option selected..

I didn't try it on a "non-tangential" area when I tried that..

oops...