Has anyone ever been able to use the Hole command to create the hole shown below?
I am not seeing an option to do this.
I know I can just create a sketch and revolve a cut feature, but when there are multiple holes in a block of wood, there is nothing convenient about that method. 🙁
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Solved! Go to Solution.
Solved by Curtis_Waguespack. Go to Solution.
Solved by Cadmanto. Go to Solution.
I did figure out another method. Create the counter bored hole then added a chamfer splitting the difference between the OD and ID. This works and is not too painful. It just would be a whole lot simpler if it was all under the hole command umbrella.
Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020
Hi Scott, this has been requested in the past, you better go vote... I think your vote is going to be the one to make it happen! 😉
https://forums.autodesk.com/t5/inventor-ideas/add-hole-type-counterbored-countersunk/idi-p/5497777
Hi Curtis,
As it stands, I already voted for it. I guess this is what happens when an idea is in the pipe line for too long. 😴 Like 5 years for this one. Should I add an English version of the idea to the station seeing this one is in Greek? 😁
I will add a comment with a link to this thread though.
Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020
I have a similar type need where I created a Punch tool, so that this works just like the Hole feature.
I simply:
Environments>Convert to Sheet Metal (even if it is absolutely nothing like a sheet metal part).
Create sketch with center point locations.
Place Punch (entering appropriate dimensions).
Environments>Convert to Standard Part.
Hi Scott,
This requires two hole features. You can create a spotface hole and then add a C'sink hole.
Many thanks!
@Cadmanto (and anyone else that might be interested)
Here's a quick ilogic rule that will add a chamfer to a counterbore to do this... I didn't test it that much so it you might find issues with it, but it worked for my limited testing.
Just create an ilogic rule and add this code, then run the rule and select the counter bore hole
Dim oDoc As Document oDoc = ThisApplication.ActiveDocument Dim oFeature As Object oFeature = ThisApplication.CommandManager.Pick( SelectionFilterEnum.kPartFeatureFilter, "Select Hole Features (press ESC to continue)") If not TypeOf oFeature is HoleFeature Then MessageBox.Show("Hole feature not selected", "iLogic") Return 'exit rule End If Dim oHole As HoleFeature oHole = oDoc.ComponentDefinition.Features.HoleFeatures.Item(oFeature.name) Dim oDiamParam As Parameter Dim oHDiam As Double oDiamParam = oHole.HoleDiameter oHDiam = oDiamParam.Value Dim CBoreDiameter As Parameter Dim oDCBore As Double CBoreDiameter = oHole.CBoreDiameter oDCBore = CBoreDiameter.Value Dim oEdgeCol As EdgeCollection oEdgeCol = ThisApplication.TransientObjects.CreateEdgeCollection() Dim oFace As Face Dim oEdge As Edge 'Dim CurveEval As CurveEvaluator Dim oDia As Double For Each oFace In oHole.Faces If oFace.SurfaceType = SurfaceTypeEnum.kCylinderSurface Then oDia = oFace.Geometry.radius*2 Logger.Info(oDia) Logger.Info(oHDiam) If oDia = oHDiam Then oEdgeCol.Add(oFace.Edges.Item(2)) End If End If oChamferLength = oDCBore-oHDiam Try oDoc.ComponentDefinition.Features.ChamferFeatures.AddUsingDistanceAndAngle _ (oEdgeCol, oFace, oChamferLength/2, 45 * PI/180) Catch End Try Next
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Hi Johnson,
That is kind of what I am doing as per my second post in this thread.
Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020
JD,
That sounds like a lot of work. No offense, buy I like my second suggestion better and even maybe @Curtis_Waguespack iLogic rule (which I am going to try).
Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020
Hi @Curtis_Waguespack ,
I tried this rule and it sort of worked. Meaning, I had a hole feature that encompassed 4 holes. The rule only worked on one of the four holes. When I selected another hole within the same hole feature, it did not convert.
Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020
You could just offset a work plane to control the depth, then place the c'sink on that work plane, and utilize the extend start to generate the hole.
Hope that helps.
@Cadmanto wrote:
Hi @Curtis_Waguespack ,
I tried this rule and it sort of worked. Meaning, I had a hole feature that encompassed 4 holes. The rule only worked on one of the four holes. When I selected another hole within the same hole feature, it did not convert.
Ooops!, I didn't write it to look at a hole feature with multiple holes within it... I'll have a look later and see if that can be achieved too.
@johnsonshiue wrote:Hi Scott,
This requires two hole features. You can create a spotface hole and then add a C'sink hole.
Many thanks!
This is what I had to do yesterday. The first time I've had to model this type of hole and was surprised it wasn't included in the Hole command.
Hi Scott,
Here's a more robust version, it'll chamfer multiple holes within the same hole feature, and it'll allow you to select multiple hole features in a row.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Dim oDoc As Document oDoc = ThisApplication.ActiveDocument Dim oFeature As Object While True oFeature = ThisApplication.CommandManager.Pick( SelectionFilterEnum.kPartFeatureFilter, "Select Counterbore Hole Features (press ESC to continue)") 'if nothing then exit If IsNothing(oFeature) Then Exit While If Not TypeOf oFeature Is HoleFeature Then MessageBox.Show("Hole feature not selected", "iLogic") Continue While End If Dim oHole As HoleFeature oHole = oDoc.ComponentDefinition.Features.HoleFeatures.Item(oFeature.name) If Not oHole.HoleType = HoleTypeEnum.kCounterBoreHole Then MessageBox.Show("Hole feature is not a Counterbore", "iLogic") Continue While End If oHole.SetEndOfPart(False ) 'clean up existing chamfer (mostly for testing) Try sHole = oHole.Name & "_Chamfer" oDoc.ComponentDefinition.Features.ChamferFeatures.Item(sHole).delete Catch End Try 'get the hole diameter Dim oDiamParam As Parameter Dim oHDiam As Double oDiamParam = oHole.HoleDiameter oHDiam = oDiamParam.Value 'get the counter bore diameter Dim CBoreDiameter As Parameter Dim oDCBore As Double CBoreDiameter = oHole.CBoreDiameter oDCBore = CBoreDiameter.Value 'create a collection hold the edges Dim oEdgeCol As EdgeCollection oEdgeCol = ThisApplication.TransientObjects.CreateEdgeCollection() Dim oFace As Face Dim oEdge As Edge Dim oDia As Double Dim oCir As Inventor.Circle 'find the planer face in the hole For Each oFace In oHole.Faces If oFace.SurfaceType = SurfaceTypeEnum.kPlaneSurface Then For Each oEdge In oFace.Edges 'find the edge in the face that is the same as the diameter If oEdge.CurveType = CurveTypeEnum.kCircleCurve Then If TypeOf oEdge.Geometry Is Inventor.Circle Then oCircle = oEdge.Geometry If oCircle.radius * 2 = oHDiam Then 'add the edge to the collection oEdgeCol.Add(oEdge) End If End If End If Next End If Next 'calc the chamfer distance oChamferLength = oDCBore - oHDiam 'create the chamfer feature Try oChamfer = oDoc.ComponentDefinition.Features.ChamferFeatures.AddUsingDistance _ (oEdgeCol, oChamferLength / 2) oChamfer.name = oHole.Name & "_Chamfer" Catch End Try oDoc.ComponentDefinition.SetEndOfPartToTopOrBottom(False) ' Set to bottom End While
Worked like a charm Curtis!!! Thank you!!
Saved the rule for future use locally.
Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020