Select face to extrude instead of create sketch first

[Neil_Cross]

I just saw this in a Fusion 360 video, would be a nice simple addition to Inventor and makes perfect sense.

- Select a flat face

- Click Extrude

- Extrude will auto-create sketch and project all geometry on that face to use for extrude profile

Saves having to create sketch, click project geometry, pick face, exit sketch, launch extrude, pick profile.  Or a variation of that workflow.

[Neil_Cross]

Healthy debate 

@ic198 by all means create that idea, as much as I agree with @DRoam about there being a line needed to separate the application of extrude and thicken, I agree there should be some enhancements to thicken!

[ic198]

New idea here

http://forums.autodesk.com/t5/inventor-ideas/thicken-command-extents-enhancements/idi-p/6717447

@DRoam I would suggest that adding faces as a selection mode to Extrude would add more crossover than adding Extents to Thicken but ok

There are legitimate reasons (other than the multiple thicknesses you suggest) why Thicken To would be used where Extrude would not. I sometimes use it with the Automatic Blending option for extending solids- see screenshot below. Original solid in grey, has a draft and tapered fillet applied. Creating the blue part with an Extrude would be very difficult but with Thicken...

In this simple example Replace Face would also work, but for some reason in the more complex models I work with Replace Face rarely works. I haven't used Direct Edit before but trying it here I see that also works- though I still can't seem to get the angled end face without a second split?

[asiu]

Voted! No strings attached! 

[DRoam]

(So I almost hate to share this for fear that it will dampen efforts by Autodesk to implement this, but I'm going to anyway only because I hope it will help some people out in the meantime. However, this does not address the main pain-point that motivated this idea, which is that if you click Extrude with a face selected, you're assaulted with an annoying dialog box which you have to click away and then follow up with 3-4 extra steps before finally extruding your face. So while this workaround may be helpful, it should not dampen or delay any efforts to implement this Idea.)

With that said! ... Behold, the iLogic rule that will do what this post is requesting. You can either click a face and then run the rule, or just run the rule and then click a face. And then it will do the rest. I recommend adding it as an external rule and then adding a button for it to your Global Forms so you can always get to it quickly.

Hope this is helpful. If anyone runs into any issues with it please let me know so it can be fixed. Thanks!

'Set a reference to the active part document
Dim partDoc As Inventor.PartDocument
Try
	partDoc = ThisDoc.Document
Catch
	MessageBox.Show("The active document must be a Part document.", "Error: Extrude from Face iLogic Rule",MessageBoxButtons.OK,MessageBoxIcon.Error)
	Return
End Try


'Create sketch on selected face
Dim oSketch As Inventor.PlanarSketch
Try 'If a valid flat face is selected...
	oFace = ThisDoc.Document.SelectSet.Item(1)
	
	oSketch = partDoc.ComponentDefinition.Sketches.Add(oFace, False)
Catch 'If a valid flat face is not selected...
	'Prompt for face selection
	oFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllPlanarEntities, "Pick a face")
	
	If Not oFace Is Nothing Then
		'If a face was selected...
		oSketch = partDoc.ComponentDefinition.Sketches.Add(oFace, False)
	Else
		'If a face was not selected...
		Return 'Exit the rule
	End If
End Try

'Project all edges on selected face
Call ThisApplication.TransactionManager.StartTransaction(ThisDoc.Document, "Project Face Edges")
Dim oEdge As Edge
For Each oEdge In oFace.Edges
	oSketch.AddByProjectingEntity(oEdge)
Next
ThisApplication.TransactionManager.EndTransaction

'Execute the Extrude command
Call ThisApplication.CommandManager.ControlDefinitions.Item("PartExtrudeCmd").Execute

[nshove]

@DRoam You are the goat. Been struggling with trying to find an easy way to extrude faces with complex faces. This was extremely helpful and time saving. Thank you very much.